1
MANUFACTURING ESSENTIALS The Operation Navigatior The Manufacturing application allows you to interactively create NC machining programs, generate tool paths, visualize material removal, and postprocess.
This course will familiarize you with the essential functions used throughout the Manufacturing application. You will learn how to use the Operation Navigator and step through the process of creating a program. With few exceptions, this process is consistent throughout the Manufacturing application. Once you have completed this course, you will be ready to move on to courses that pertain to your specific areas of interest such as milling, drilling, turning, or wire edm. Audience This course is intended for users who require a general overview of the Manufacturing application. New users should complete this course before moving on. Subsequent courses allow you to selectively examine your particular areas of interest. Prerequisites The prerequisite for this course is the Unigraphics NX Essentials CAST Online Library course. In addition, you should be familiar with basic manufacturing processes and terminology. Course Contents The Operation Navigator — You will learn about the relationship between parent groups
and operations, how the Operation Navigator organizes objects, and how operations inherit parameters from parent groups. You will explore some of the essential functions of the Operation Navigator, including how to change views, edit parameters, cut and paste objects, and specify a machining environment.
2 Creating Objects — You will learn how to create Program, Tool, Geometry, and Method
objects. Creating Operations — You will learn how to create operations individually and how to edit
and respecify parent groups from within the operations.You will also learn how to customize dialogs to update legacy operations by adding the Main, Groups and Viewing tabs that are found on newly created operations. Creating Operation Sequences — You will learn how to use a Process Assistant to create a
program containing a predefined sequence of operations. UG/Post — You will learn how to postprocess using UG/Post. Graphics Postprocessor Module — You will learn how to create and edit a Cutter Location
Source File (CLSF) and how to postprocess the CLSF using the Graphics Postprocessor Module (GPM). Shops — You will learn how to use Shops, a product designed to step the occasional user
(such as the shop floor machine operator) through the process of creating an operation using a Process Assistant. Shop Documentation — You will learn how to create shop documentation in HTML format
for use by machine tool operators.
Parent Groups and Operations The Operation Navigator allows you to view and manage relationships between operations, programs, machining methods, geometry, and tools. Most importantly, it allows you to define parameters just once within parent groups and then use them in as many operations as desired, eliminating the repetitious and tedious task of specifying parameters separately for each operation. The Operation Navigator organizes objects (parent groups and operations) within in a tree structure. Objects that contain other objects are known as parent groups. Parent groups define parameters that can be passed down and used (inherited) by operations.
3
In the above illustration, the WORKPIECE object inherits parameters from its parent, the MCS_MILL object. The MILL_AREA object inherits parameters from its parent, the WORKPIECE object (which inherits parameters from the MCS_MILL object). The operations all inherit parameters from the MILL_AREA object (which inherits parameters from the WORKPIECE and MCS_MILL objects).
Parent Groups and Operations Opening the Part File You will open a part file and go into the Manufacturing application. You will then begin working with the operations and objects displayed in each view of the Operation Navigator. Open part file mfe_navigator_1.prt from the mfe subdirectory. Choose Application
Manufacturing.
Parent Groups and Operations Operation Navigator Tab
4 In Windows, you can display the Operation Navigator by clicking or double-clicking on the Operation Navigator tab in the resource bar. Clicking on the tab temporarily displays the Operation Navigator by sliding it to the left over the graphics display. Once you move the cursor out of the Operation Navigator the Operation Navigator disappears from the screen. Clicking on the pin at the upper left corner of the Operation Navigator allows the Operation Navigator to remain on the screen when you move the cursor out of the area.
Double-clicking on the tab displays the Operation Navigator in a separate window which can then be moved and docked (Ctrl key undocks). Clicking the Close icon at the upper right corner closes the window and restores the tab.
Practice using the Operation Navigator tab, pinning, docking, and undocking as described above.
Parent Groups and Operations MB3 Options Commonly used options available in the toolbar are also available in the pop-up menu by clicking MB3 on the Operation Navigator background.
5
Parent Groups and Operations Columns and Properties Columns and Properties options are displayed in a pop-up menu by clicking MB3 on the Operation Navigator background.
6
Parent Groups and Operations Adding and Removing Columns in the Operation Navigator Display the Program Order view in the Operatuion Navigator. Click MB3 on the Operation Navigator background and choose Columns and Configure.
7
Turn the Tool Description option on.
OK to accept the Operation Navigator Properties dialog. The Tool Description column now displays in the Operation Navigator (you may need to scroll to the right).
Click MB3 on the Operation Navigator background and choose Columns and Configure. Turn the Tool Description option off.
8 OK to accept the Operation Navigator Properties dialog.
Parent Groups and Operations Changing Operation Navigator Views The Operation Navigator displays in one of four views: the Machining Method view, Program Order view, Machine Tool view, or Geometry view. Each view organizes the operations according to the theme of the view. You can easily switch from one view to another by choosing one of the icons in the toolbar.
Parent Groups and Operations Displaying the Machine Tool View You will display the Machine Tool View. This view allows you to see the tools used by the operations.
Choose the Machine Tool View icon in the toolbar (or choose Tools Navigator View Machine Tool View in the menu bar).
Operation
Click on the plus (+) signs to fully expand the objects. The Machine Tool View organizes the operations according to tools. The three operations outlined below use the MILL_1 tool.
9
Parent Groups and Operations Displaying the Program Order View You will display the Program Order View. This view allows you to see the order in which the operations will be executed on the machine tool.
Choose the Program Order View icon
in the toolbar.
Click on the plus (+) sign to fully expand the PROGRAM object. The Program Order View displays the program that each operation belongs to and the order in which operations will be executed on the machine tool. This is the only view in which the order of the listed operations is relevant or important.
Parent Groups and Operations Displaying the Geometry View You will display the Geometry View. This view allows you to see the geometry objects and the operations contained within the objects.
Choose the Geometry View icon
in the toolbar.
Click on the plus (+) signs to fully expand the objects. The Geometry View organizes the operations according to machining geometry. Parameters such as part, blank, and check geometry, MCS orientation, and clearance plane are defined by geometry objects. The four operations outlined below use the MCS_MILL, WORKPIECE, MILL_AREA geometry objects.
10
Parent Groups and Operations Displaying the Machining Method View You will display the Machining Method View. This view allows you to see the cut methods the operations use.
Choose the Machining Method View icon
in the toolbar.
Click on the plus (+) signs to fully expand the objects. The Machining Method View organizes operations according to cut method (rough, finish, semi finish). Parameters such as Intol, Outtol, and part stock are defined by machining method objects. The program below consists of one roughing operation, two semi-finishing operations, and two finishing operations.
Remember, the only view in which the order of the listed operations is relevant is the Program Order view.
11
Cutting and Pasting Operations You can move objects within any view of the Operation Navigator by cutting and pasting. Cutting and pasting operations within the Program Order View allows you to change the order in which the operations are executed on the machine tool. Cutting and pasting operations within the Machine Tool View allows you to change the tool the operation uses.
Cutting and Pasting Operations Reordering Operations You will cut and paste an operation within the Program Order View to change the order in which it is executed on the machine tool.
Choose the Program Order View icon
in the toolbar.
Choose the CONTOUR_ZIGZAG icon and MB3
Cut.
The object you choose in the next step is the operation below which the pasted operation will appear. Choose the CONTOUR_AREA_DIR_STEEP icon and MB3
Paste.
12
CONTOUR_ZIGZAG is now the last operation in the program sequence.
Cutting and Pasting Operations Respecifying the Cutting Tool You will cut and paste an operation within the Machine Tool View to change the cutting tool the operation uses.
Choose the Machine Tool View icon
in the toolbar.
The CONTOUR_FOLLOW_1 operation currently uses MILL_1 as the parent group that defines cutting tool. Choose the CONTOUR_FOLLOW_1 icon and MB3
Cut.
The object you choose in the next step is the parent group inside of which the operation will be pasted. Choose the MILL_2 icon and MB3
Paste Inside.
13
CONTOUR_FOLLOW_1 now uses MILL_2 as the cutting tool.
A slashed red circle now appears in front of the pasted operation. This indicates that operation parameters have changed and that the tool path must be regenerated to reflect the change.
Operation Status Symbols
Operations and program groups in the Operation Navigator are preceded by one of three status symbols; Complete, Regenerate, or Repost as illustrated below. A green check mark
indicates a complete status
Complete status means that the operation or program has been generated, incorporating the current operation parameters, and has been either postprocessed or output to an operating system text file. A slashed red circle
indicates a regenerate status
Regenerate means that a tool path has not been generated for the operation or that operation parameters have changed and that the tool path must be regenerated to reflect the change. An exclamation point
indicates repost status
Repost status means that the tool path for the operation has been generated, but it has not been postprocessed or exported from the part file. The status symbols are dynamic and will update as the status of the operation or group changes.
14
Cutting and Pasting Operations Generating a Tool Path You will generate the tool path for the operation you just moved. The tool path will be recalculated using the new tool. Choose the CONTOUR_FOLLOW_1 icon and MB3
Generate.
OK the Tool Path Generation dialog. The new tool path is recalculated and generated using the MILL_2 tool. The tool path is graphically displayed by tracing the tip of the tool.
An exclamation point now appears in front of the operation and PROGRAM object indicating that the operations have been generated but have not yet been postprocessed or exported.
15
Cutting and Pasting Operations Replaying a Program You will Replay the entire program so you can see the tool paths displayed in the sequence in which they will be executed on the machine tool.
Choose the Program Order View icon Choose the PROGRAM icon and MB3
in the toolbar. Replay.
You can replay tool paths selectively by holding down the Ctrl key and choosing individual operations.
Cutting and Pasting Operations Visualizing the Tool Path You will use the Toolpath Visualization options to animate the cutter movement and dynamically display material removal. Choose the PROGRAM icon and MB3
Toolpath
Verify.
16
The Toolpath Visualization dialog displays with the Replay tab chosen.
Cutting and Pasting Operations Replaying a Program You will Replay the entire program.
Choose the Shaded icon
in the toolbar to display the part as a shaded solid.
Choose the Play Forward icon.
17 The tool paths replay in the program sequence with the tool tip tracing each path. Each operation highlights in the Operation Navigator as it replays.
Cutting and Pasting Operations Displaying Dynamic Material Removal You will dynamically display the material removal. This method of visualization allows you to clearly see the material as it is removed by each successive tool path. Choose the Dynamic tab. Choose Reset. This option resets the program so that the operations are again played in order from first to last. Choose the Play Forward icon.
The material removed by each successive tool path is displayed in a contrasting color. OK to complete the tool path visualization. More About: Dynamic Material Removal Colors
The colors displayed for dynamic material removal are determined by the Preference settings (Preferences Manufacturing).
18
Once the colors have been defined in the Manufacturing Preferences dialog, the Verify function uses these colors in the order defined when displaying Dynamic Material Removal.
Redefining the Machining Environment You can delete the current Machining Environment associated with the part and define a new CAM Session Configuration and CAM Setup. In doing so, all operations and parent groups are deleted from the part. It essentially enables you to "start over" as though the part file is being brought into the Manufacturing module for the first time.
19
Redefining the Machining Environment Deleting the Machining Environment You will delete the current configuration file and CAM setup data associated with the part. Choose Tools
Operation Navigator
Delete Setup from the main menu bar.
A confirmation message warns you that all manufacturing data will be deleted and cannot be recovered. OK to delete the setup. All CAM data, operations, tools, geometry, etc., have been deleted from the part file. The Machining Environment dialog displays requiring you to specify a configuration file and setup. The Machining Environment dialog displays when a part file has been brought into the Manufacturing module for the first time or when the setup has been deleted.
More About Machining Environment
When Unigraphics NX starts, it reads the ugii_env.dat file to define a large number of environment variables setting system defaults, the location of resource files, etc. One of the things that is set by the ugii_env.dat file is the location of the configuration directory. This is done by the environment variable UGII_CAM_CONFIG_DIR. This directory contains a number of files with the file extension. ".dat".
20
Unigraphics NX reads the names of these files and displays this list in the top half of the Machining Environment dialog, in the CAM Session Configuration list box.
A default Configuration is also defined in the ugii_env.dat file by the environment variable UGII_CAM_CONFIG. It is set to point to cam_general.dat. That is why the Machining Environment initially displays with the cam_general configuration highlighted. Cam_general.dat sets up a number of environment variables pointing towards template files for documentation, postprocessors that are correct for the machine tool you're using, feeds and speeds, etc. One environment variable it defines is TEMPLATE_OPERATION. This is pointed towards an "opt" file. By default, for cam_general.dat, this environment variable points towards cam_general.opt. Cam_general.opt contains a list of template part files: mill_planar.prt mill_contour.prt mill_multi-axis.prt drill.prt turning.prt wire_edm.prt A list of these part files is displayed in the CAM Setup list box.
21
When you selected the lathe configuration, the CAM Setup list box was updated to show the only files listed in lathe.opt, lathe.prt and legacy_lathe.prt.
The general flow of definition of environment variables is something like the illustration below:
22
Any changes to all these dat and opt files to customize them to your own manufacturing environment must be done carefully. In most cases, it will require system administrator privileges to make these changes.
Redefining the Machining Environment Choosing the Session Configuration You will choose a CAM Session Configuration that allows you to create all types of operations including Milling, Drilling, Turning, and Wire EDM. The CAM Session Configuration defines the available machining processors, tool libraries. postprocessors, and other high level parameters for the logon session. Choose the cam_general configuration file.
23 The cam_general configuration allows you to create all types of operations including Milling, Drilling, Turning, and Wire EDM. Other session configurations such as lathe or mill_contour restrict you to a specific type of operation.
Redefining the Machining Environment Choosing the CAM Setup You will choose a CAM Setup that allows you to create planar milling operations and then initialize the new machining environment. Choose the mill_planar setup.
Choose Initialize. The new machining environment is complete. The geometry objects required to create planar mill operations are created automatically. They give you a basic starting point from which you can begin creating operations and other objects.
Redefining the Machining Environment Viewing the Geometry and Machining Method Objects You will look at the Geometry and Machining Method Views of the Operation Navigator and notice that the objects required to create planar mill operations are created automatically based on the specified CAM Setup.
Choose the Geometry View icon Choose the Expand All icon
in the toolbar. in the toolbar to fully expand the objects.
Notice that the MCS_MILL and WORKPIECE geometry objects have been created. The machining method objects required to create planar mill operations are also created automatically.
24
Choose the Machining Method View icon
in the toolbar.
In the next lesson, you will learn more about creating objects and the parameters they define. Close the part file.
Creating Objects In this lesson, you will learn how to create Program, Tool, Geometry, and Method objects.
Tool, Geometry, and Method objects define operation parameters. These parameters can be inherited by operations contained within the objects. By specifying these objects as parent groups, you can eliminate the repetitious and tedious task of respecifying parameters each time you create an operation. Program objects do not define operation parameters. Instead, they simply contain operations and determine the sequence in which operations are executed on the machine tool. For
25 example, the sequence of operations required to machine the top of a part may be contained in one program while the sequence of operations required to machine the end of a part may be contained in another program.
Creating Tool Objects In this section, you will learn how to create tool objects. You will learn how to define new tools as well as how to retrieve existing tools from a library. Open part file mfe_objects_1.prt from the mfe subdirectory. Choose Application
Manufacturing.
Creating Tool Objects Displaying the Machine Tool View Choose the Machine Tool View icon in the toolbar (or choose Tools Navigator View Machine Tool View in the menu bar). Choose the Expand All icon in the toolbar (or choose Tools Navigator Expand All in the menu bar).
Operation
Operation
The Operation Navigator shows that both the PLANAR_MILL and FACE_MILLING operations use the same tool: MILL.
26
Creating Tool Objects Creating a Face Mill Tool Object You will create a 5-parameter face mill tool object and then cut and paste the FACE_MILLING operation into that object so that the operation uses the new tool.
Choose the Create Tool icon
in the toolbar.
The Type determines the available Subtypes you have to choose from. In the Create Tool dialog, Set the Type option to mill_planar.
The Subtype section displays only tools that are appropriate for milling operations. Choose the FACE_MILL icon.
Be sure GENERIC_MACHINE is chosen as the parent group. This way, the tool you create will have the same parent as the existing mill tool.
The tool name defaults to FACE_MILL based on the subtype you chose. You may name the tool using the following rules: Up to 20 characters Start with an alphabetic character The only acceptable special characters are the dash (-) and period (.) No spaces are allowed. OK to begin defining the FACE_MILL tool parameters.
27
Creating Tool Objects Defining the Tool Parameters You will specify parameters that define the size and material of the tool. Key in the following values to define the tool.
The tool material is one of several parameters that the Reset from Table option uses to determine the speeds and feeds for cutting. Choose Material: CARBIDE.
Highlight TMCO_00001 HSS and OK.
OK to create the FACE_MILL tool object.
Creating Tool Objects Respecifying the Tool You will respecify the tool the operation uses by dragging and dropping the operation onto the tool object. Highlight the FACE_MILLING operation with the mouse button 1 and hold the button down while you drag the icon on top of the FACE_MILL object. Release the mouse button
28 to drop the operation.
The FACE_MILLING operation now uses FACE_MILL as the cutting tool.
This can also be accomplished by cutting and pasting the operation inside the tool object. The slashed red circle indicates that operation parameters have changed and that the tool path must be regenerated to reflect the change.
Creating Tool Objects Generating the Tool Path You will generate the tool path using the FACE_MILL tool. This will update the operation status. Choose the FACE_MILLING icon and MB3
OK to accept the tool path generation.
Generate.
29
An exclamation point now appears in front of the operation indicating that the operation has been generated not yet been postprocessed or exported.
Creating Tool Objects Visualizing the Tool Paths You will use the Toolpath Visualization options to animate the cutter movement and dynamically display material removal for the program.
Choose the Shaded icon
in the toolbar to display the part as a shaded solid.
Choose the Program Order View icon
in the toolbar.
Highlight the PROGRAM object.
Choose the Verify Toolpath icon
in the toolbar or MB3
Toolpath
The Toolpath Visualization dialog displays with the Replay tab chosen. Choose the Dynamic tab.
Drag the slider bar to the left to slow down the Animation Speed to 7.
Verify.
30
Choose the Play Forward icon. Because the part does not contain or inherit blank geometry, the Automatic Blank for Visualize dialog displays allowing you to define blank geometry temporarily to perform dynamic material removal.
Creating Tool Objects Defining the Blank Geometry You will define the blank geometry as a solid body bounding the part geometry. OK to accept Auto Block as the Blank Type.
Auto Block creates a solid body bounding the part geometry with faces parallel to the WCS. The material removed by each successive tool path is displayed in a contrasting color allowing you to clearly see that the face milling operation leaves some uncut material behind.
The tool changes to the FACE_MILL tool for the second operation. OK to complete the tool path visualization.
31
Creating Tool Objects Retrieving a Tool From the Library You will now retrieve a predefined tool from the library.
Choose the Create Tool icon
in the toolbar.
Choose Retrieve Tool and OK.
Click on the plus (+) sign next to Milling to expand the list and choose End Mill (non indexable).
OK to accept the selection.
Creating Tool Objects Specifying Search Criteria You will use the Search Criteria Dialog to narrow down the library search by specifying parameters. Choose Count Matches.
A number appears next to the button (in this example, 64). This indicates the number of tools in the library that match the parameters you have specified so far. You can narrow the search even further by specifying exact numeric values or a range of values using <, >, <=, and >= signs.
32 Key in 0.50 in the Diameter field.
Choose Count Matches. You have narrowed the search to only those tools in the library with a diameter of 0.50. Choose Result Info. This displays an Information listing of all the tools matching the search criteria. It will allow you to determine the values (Flute Length and Corner Radius for example) that can be specified to continue narrowing the list. Dismiss the Information window. Key in the following values.
Choose Count Matches. You have narrowed the search to the only those .50 diameter tools in the library with a flute length greater than 1 and a corner radius greater than or equal to .05 . OK to accept the search criteria.
Creating Tool Objects Choosing Tools You will use the Search Result listing to choose the desired tool or tools. Use the left mouse button to choose a single tool. Use the left mouse button in combination with the Shift key to choose a range of tools. Use the left mouse button with the Ctrl key to selectively choose tools from the list. The Ctrl key also enables you to deselect. Choose the two tools indicated below.
OK to accept the tools.
33
Choose the Machine Tool View icon
in the toolbar.
The tools retrieved from the library appear in the Machine Tool view of the Operation Navigator and are now available to be used in operations.
You can easily obtain information about the tools. Highlight the UGTI0201_064 icon and MB3
Properties.
Dismiss the Information window.
Creating Tool Objects Respecifying the Tool You will respecify the tool that the PLANAR_MILL operation uses by dragging and dropping the operation onto the UGTI0201_064 tool object. Drag and drop the PLANAR_MILL operation onto the the UGTI0201_064 object.
The PLANAR_MILL operation now uses UGTI0201_064 as the cutting tool.
34
The red circle indicates that operation parameters have changed and that the tool path must be regenerated to reflect the change.
Creating Tool Objects Generating the Tool Path You will generate the tool path using the new tool. Choose the PLANAR_MILL icon in the Operation Navigator and MB3
Generate.
OK to accept the tool path generation.
Close the part file.
Creating Machining Method Objects In this section, you will learn how to create Machining Method objects. These objects allow you to organize operations according to cut method (rough, finish, semi finish) by defining parameters such as , Outtol, and part stock.
35 Open part file mfe_objects_2.prt from the mfe subdirectory. Choose Application
Manufacturing.
Creating Machining Method Objects Displaying the Machining Method View Choose the Machining Method View icon Choose the Expand All icon below.
in the toolbar.
in the toolbar to see all of the objects as illustrated
The PLANAR_MILL operation uses the MILL_ROUGH method and the FACE_MILLING operation uses the MILL_FINISH method. The SEMI_FINISH_LEVELS operation does not use a method.
Creating Machining Method Objects Creating a Semi-Finish Machining Method Object You will create a semi-finish machining method object to use as parent group.
Choose the Create Method icon
in the toolbar.
36 The Type determines the available Subtypes. Choose mill_planar as the Type. MILL_METHOD is the only available Subtype.
Be sure METHOD is chosen as the parent group. This way, the object you are creating will have the same parent group as the other machining method objects. Key in SEMI_FINISH for the name.
OK to begin creating the SEMI_FINISH machining method object. Key in 0.01 or the Part Stock. Part Stock is the amount of material remaining on the part after roughing and semi-finishing operations. This is the parameter that primarily determines the difference between a roughing, semifinishing, and a finishing operation. Intol and Outtol define an allowable range the tool may use to deviate from the part surfaces. The smaller the values, the more accurate the cut. Intol allows you to specify the maximum amount by which the tool may penetrate through the surface. Outtol allows you to specify the the maximum amount by which the tool may avoid contacting the surface.
OK to create the SEMI_FINISH object. The SEMI_FINISH object is not a parent group because it does not contain any operations.
37
Creating Machining Method Objects Moving an Operation into the Object You will drag and drop the SEMI_FINISH_LEVELS operation onto the SEMI_FINISH machining method object. Highlight the SEMI_FINISH_LEVELS operation with mouse button 1 and hold the button down while you drag the icon on top of the SEMI_FINISH object. Release the mouse button to drop the operation.
The SEMI_FINISH machining method is now a parent group containing the SEMI_FINISH_LEVELS operation.
Creating Machining Method Objects Generating the Tool Path You will generate the tool path using SEMI_FINISH as the machining method. Choose the SEMI_FINISH_LEVELS icon and MB3 OK to accept the tool path generation.
Generate.
38
Creating Machining Method Objects Visualizing the Tool Paths Visualization allows you to see the material removal as the program progresses through the sequence of rough, semi-finish, and finish operations. Choose the Shaded icon in the toolbar to display the part as a shaded solid. Choose the Program Order View icon
in the toolbar.
Choose the PROGRAM object.
Choose the Verify Toolpath icon
in the toolbar.
Choose the Dynamic tab.
Drag the slider bar to the left to slow down the Animation Speed to 7. Choose the Play Forward icon.
39 Because the part does not contain or inherit blank geometry, the Automatic Blank for Visualize dialog displays allowing you to define blank geometry temporarily to perform dynamic material removal.
Creating Machining Method Objects Defining the Blank Geometry You will define the blank geometry as a solid body bounding the part geometry. OK to accept Auto Block as the Blank Type. Auto Block creates a solid body bounding the part geometry with faces parallel to the WCS.
The material removed by each successive tool path is displayed in a contrasting color. OK to complete the tool path visualization. Close the part file.
Creating Geometry Objects Different types of operations require different types of geometry. Planar milling operations require boundaries while surface contouring operations require faces or bodies. In this section, you will learn how to create geometry objects for planar milling operations. Open part file mfe_objects_3.prt from the mfe subdirectory. Choose Application
Manufacturing.
40
Creating Geometry Objects Displaying the Geometry View Choose the Geometry View icon
in the toolbar.
The PLANAR_MILL and SEMI_FINISH_LEVELS operations are contained in the MCS_MILL parent group. This parent group defines the location and orientation of the Machine Coordinate System.
Machine Coordinate System
Like other applications, Manufacturing uses the WCS, or Work Coordinate System. However, the Manufacturing application has its own coordinate systems as well - the Machine Coordinate System (MCS). As illustrated below, the WCS and MCS are in the same location. The MCS is displayed similar to the WCS, but the axes are labeled XM, YM, and ZM.
41 What is the significance of these coordinate systems for the Manufacturing application? WCS - All the parameter values that you input (for example, values for the Start Point, a Z value for the Clearance Plane, or I,J,K values for the tool axis vector, and other vector data) will be in relationship to the WCS. MCS - All coordinate values in the tool path (all of the output coordinates) are in relationship to the MCS. The ZM axis of the MCS is particularly important since, if no tool axis is specified, the ZM axis is the default tool axis. The output tool path consists of a number of different commands. The most frequent command is probably the linear positioning move, GOTO. There are at most 6 coordinate fields in a GOTO: X, Y, Z, I, J and K. The X, Y and Z fields are the coordinates of the tool tip relative to the MCS and the I, J, K values indicate the tool axis vector. Depending on the circumstances, you may want to specify your Machine Coordinate System and Work Coordinate System in the same location to avoid confusion. Before you start creating any machining operations, you should always display the Work Coordinate System and Machine Coordinate System and check their location and orientation. A MCS is one of the default CAM objects created by all templates. The name assigned to this MCS varies, dependent upon the CAM template part file selected in creating the setup. The default MCS is created coincident with the absolute coordinate system. You can edit the location of the default MCS to change the coordinates of the output tool path or create a new MCS. Even though you may have many MCS objects created, only one machine coordinate system is displayed at a time.
Creating Geometry Objects Creating a Mill Boundary Object Part geometry is required to generate tool paths. You will create an object that defines part boundaries.
Choose the Create Geometry icon
in the toolbar.
The Type determines the available Subtypes you have to choose from. Be sure mill_planar has been chosen as the Type. Choose the MILL_BND icon.
42 Be sure MCS_MILL has been chosen as the Parent Group. The object you are creating inherits the Machine Coordinate System parameters. The name defaults to MILL_BND based on the chosen subtype. OK to begin defining the MILL_BND object.
Creating Geometry Objects Defining Part Boundaries You will create the part boundaries required to generate the tool paths. You will first define the main containment boundary. Choose the Part icon and Select.
Choose the Curve Boundary icon.
Choose Outside for the Material Side.
This specifies that the material retained is outside the boundary and allows the tool to cut only inside the boundary. Choose the Custom Data tab. Turn on the Offset option under Custom Boundary Data and key in -0.1.
This defines a negative stock that assures the material along the outside edge of the part is completely removed.
43
Creating Geometry Objects Defining the Main Containment Boundary You will select the edges that define the main containment boundary. This boundary defines the overall part and encloses other boundaries that define islands. Select the four outside edges in order as illustrated below.
Choose the Main tab. Choose Create Next Boundary. The main containment boundary should display as illustrated below.
Creating Geometry Objects Defining Boundaries at Island Tops
44 You will create boundaries that define the top of each island. Choose the Face Boundary icon.
Choose Inside for the Material Side. This specifies that the material retained is inside the boundary and does not allow the tool to cut inside the boundary. Select the first face as illustrated below.
Select the second and third faces as illustrated below.
OK to accept the part boundary definition. OK to finish creating the MILL_BND object.
45
Creating Geometry Objects Moving Operations into the Object You will cut and paste the two operations into the MILL_BND geometry object. Highlight the PLANAR_MILL operation and MB3
Highlight the MILL_BND object and MB3
Cut.
Paste Inside.
MILL_BND is now a parent group of the PLANAR_MILL operation.
Cut and paste the SEMI_FINISH_LEVELS operation inside the MILL_BND object so that MILL_BND contains both operations.
46
Creating Geometry Objects Generating the Tool Paths You will generate the tool paths for both operations. Choose the first operation and hold down the Ctrl key to choose the second operation.
MB3
Generate.
OK to accept the first tool path generation. OK to accept the second tool path generation.
MB3
Refresh to remove the tool path display.
Creating Geometry Objects Creating a Workpiece Object
47 You will create a workpiece object that defines the part material and the blank geometry. The part material is one of several parameters used in determining the cut feed rate. Adding operations to the program such as Cavity Milling will require blank geometry. Choose Edit
Blank
Reverse Blank All in the menu bar.
This displays the body you will select to define the blank geometry.
Choose the Create Geometry icon
in the toolbar.
Be sure mill_planar has been chosen as the Type. Choose the WORKPIECE icon.
Be sure MCS_MILL is chosen as the parent group so that the object you are creating inherits the Machine Coordinate System parameters defined in MCS_MILL.
The name defaults to WORKPIECE based on the subtype you chose. OK to begin defining the workpiece.
Creating Geometry Objects Specifying the Part Material You will specify the part material. This is one of several parameters that the Reset from Table option uses to determine the speeds and feeds for cutting.
48 Choose Material: CARBON STEEL.
Highlight MATO_00266 ALUMINUM and OK.
Creating Geometry Objects Defining Blank Geometry You will select the solid body to define the blank geometry. Choose the Blank icon and Select. Select the body.
OK to accept the blank geometry. OK to finish creating the workpiece object.
Choose Edit
Blank
Reverse Blank All in the menu bar to display the part.
Creating Geometry Objects Moving the Mill Boundary Object
49 You will cut and paste the MILL_BND object into the WORKPIECE object. In doing so, you will also move the operations. Highlight the MILL_BND object and MB3
Cut.
Highlight the WORKPIECE operation and MB3
Paste Inside.
The PLANAR_MILL and SEMI_FINISH_LEVELS operations are still contained in the MILL_BND parent group.
Creating Geometry Objects Generating the Tool Path You will generate the tool paths. Choose the Program Order View icon in the toolbar. Choose the PROGRAM object and MB3
OK to accept the first tool path generation.
Generate.
50 OK to accept the second tool path generation.
Creating Geometry Objects Visualizing the Tool Paths You will use the Toolpath Visualization options to animate the cutter movement and dynamically display material removal for the program. Choose the PROGRAM object in the Operation Navigator. Choose the Verify Toolpath icon. Choose the Dynamic tab. Choose the Play Forward icon.
Because the part inherits blank geometry from the workpiece object, the Automatic Blank for Visualize dialog does not display as it did in the previous examples. OK to complete the tool path visualization. Close the part file.
51
Creating Program Objects In this section, you will learn how to create program objects. Program objects allow you to gather and order operations into logical programs. For example, one program may contain operations that machine the top of the part while another program may contain operations that machine the side of the part. Open part file mfe_objects_4.prt from the mfe subdirectory. Choose Application
Manufacturing.
Creating Program Objects Displaying the Program Order View Choose the Program Order View icon in the toolbar. Expand the program by clicking on the (+) sign so you can see all the operations. The Operation Navigator shows that all operations are contained in a single program object.
52
Creating Program Objects Visualizing the Tool Paths The program machines both the top and the side of the part. Choose the PROGRAM object in the Operation Navigator. Choose the Verify Toolpath icon. Choose the Dynamic tab. Choose the Play Forward icon.
OK to complete the tool path visualization.
Creating Program Objects Creating a Program Object You will create a program object to contain the operations that machine the top of the part.
53
Choose the Create Program icon
in the toolbar.
PROGRAM is the only available Subtype.
Key in TOP for the name. OK to create the TOP program object. The TOP currently does not contain any objects and is not a parent group.
Creating Program Objects Copying a Program Object You will copy the TOP program object to create an object that will contain the operations that machine the side of the part. Choose TOP and MB3
Copy.
The object you choose in the next step is the object below which the pasted objects will appear.
54 With TOP chosen, MB3
Paste.
TOP_COPY is now the last object in the program.
Creating Program Objects Renaming a Program Object You will change the name of TOP_COPY to SIDE. Be sure TOP_COPY is still highlighted. Choose Tools
Operation Navigator
Rename in the menu bar.
Key in side and press the Enter key.
Creating Program Objects Moving Operations into the Top Program You will cut and paste operations into the TOP program object.
55 Choose the PLANAR_MILL operation and hold down the Ctrl key to choose the SEMI_FINISH_LEVELS and FACE_MILLING operations. MB3
Cut.
Highlight the TOP object and MB3
Paste Inside.
TOP is now a parent group of the three operations.
This can also be accomplished by dragging and dropping multiple objects.
Creating Program Objects Moving Operations into the Side Program You will cut and paste operations into the SIDE program object. Cut and paste the PLANAR_MILL_SIDE, SEMI_FINISH_LEVELS_SIDE, and FACE_MILLING_SIDE operations inside the SIDE object.
56
Creating Program Objects Deleting an Object You will delete the PROGRAM object since it is no longer needed. Choose PROGRAM and MB3
Delete.
OK to delete the object.
Creating Program Objects Visualizing the Tool Paths You can now visualize each program separately. Choose the TOP object. Choose the Verify Toolpath icon. Choose the Dynamic tab. Choose the Play Forward icon.
57 OK to complete the tool path visualization. Choose the SIDE object and visualize the program as you did for the TOP object.
You can visualize the entire program by choosing the NC_PROGRAM object. OK to complete the tool path visualization. Close the part file.
Creating Operations In this lesson, you will learn how to create individual operations and edit and respecify parent groups from within the operations.
You will also learn how to customize dialogs to update legacy operations by adding the Main, Groups and Viewing tabs that are found on newly created operations.
Creating an Operation
58 Although some of the parameters for milling, drilling, turning, and wire edm operations differ, the process of creating any operation is basically the same. You first specify the Type, Subtype, and Parent Groups. You then define any additional parameters required for the specific operation. Finally, you generate the tool path and make any necessary modifications. Open part file mfe_operation_1.prt from the mfe subdirectory. Choose Application
Manufacturing.
Creating an Operation Beginning the Operation You will begin creating a planar mill operation that roughs out material in multiple cut levels.
Choose the Create Operation icon
in the toolbar.
Be sure mill_planar is displayed as the Type.
The Type determines the subtype icons and the parent groups that are available to choose from in the dialog. Choose ROUGH_FOLLOW as the subtype.
Choosing the appropriate operation subtype will set many of the required operation parameters and can save a significant amount of time and effort in defining the operation.
59 Specify the following parent groups.
Parent groups determine common parameters that can be used by multiple operations. This operation is automatically named ROUGH_FOLLOW based on the Subtype you chose. OK to begin creating the operation.
Creating an Operation Specifying the Cut Depth You will specify multiple cut levels at a fixed depth. Choose Cut Depths. Choose Fixed Depth.
Fixed Depth generates cut levels at a constant depth. Key in 0.1 in the Maximum field.
Maximum defines the largest allowable cut depth for each level. OK to accept the cut depth.
Creating an Operation Calculating Feeds and Speeds
60 You will allow the system to recommend appropriate feed rates and speeds based on the user specified part material, tool type and material, cut method, and cut depth parameters. Choose Feed Rates. Notice that the current Surface Speed and Feed per Tooth values are set to zero.
Choose Reset from Table. The system extracts Surface Speed and Feed Per Tooth values from tables (maintained by system administration) based on the user input. The other values are then calculated.
OK to accept the Feeds and Speeds.
Creating an Operation
61
Generating the Tool Path You will observe how the operation generates the tool path at the specified cut depths. Generate the tool path. Turn the Pause After Display and Refresh Before display options off. This will allow you to generate all the cut levels at once and continue viewing them after they have generated. OK the generate the tool paths.
Refresh the display.
Creating an Operation Displaying the Part Boundaries A planar mill operation must contain properly defined part boundaries in order to generate a tool path. You will display the part boundaries for visual verification. Choose the Part icon. Choose Display to highlight the part boundaries.
Notice that the Select/Reselect button is blanked. Part boundaries are inherited from the MILL_BND parent group and can only be modified by editing the parent group. In just a moment, you will see how to edit the MILL_BND parent group from this dialog.
62
Refresh the graphics display.
Creating an Operation Displaying the Floor Plane A planar mill operation must contain a floor plane in order to generate a tool path. You will display the floor plane for visual verification. Choose the Floor icon. Choose Display to highlight the floor.
Notice that the Select/Reselect button is blanked. The floor plane is inherited from the MILL_BND parent group and can only be modified by editing the parent group that defines it. Refresh the graphics display.
Creating an Operation Visualizing the Tool Path
63 You will use the Toolpath Visualization options to animate the cutter movement and dynamically display material removal for the program. Choose the Verify icon
at the bottom of the dialog.
Choose the Dynamic tab. Choose the Play Forward icon. Because the part inherits blank geometry from the workpiece object, the Automatic Blank for Visualize dialog does not display as it did in the previous examples. The operation leaves a thin wall of uncut material along the outside edge of the part.
OK to complete the Toolpath Visualization.
Creating an Operation Editing the Geometry Parent Group You will edit the MILL_BND parent group so that the material along the outside edge of the part is completely removed. The options at the top of the operation dialog allow you to edit and reselect parent groups. Choose the Groups tab. Choose Geometry: MILL_BND and Edit.
64 A message displays informing you that the MILL_BND parent group contains more than one member and that editing it will affect all members. MILL_BND is a parent of the operation you are currently creating as well as the existing FINISH_FLOOR operation. Editing the part boundaries defined in this parent group will therefore affect both operations. OK the message. The MILL_BND dialog displays allowing you to edit the parent group.
Creating an Operation Editing the Main Containment Boundary You will edit the main containment boundary so that the operation no longer leaves a thin wall of uncut material along the outside edge of the part. Choose the Part icon and Edit.
The part boundaries highlight with the main containment boundary selected.
Turn the Offset option on and key in -0.1.
65
This defines a "negative stock" that assures the material along the outside edge of the part is completely removed. OK to accept the part boundary offset. OK to finish editing the MILL_BND parent group. OK to complete the ROUGH_FOLLOW operation. The ROUGH_FOLLOW operation now appears in the Operation Navigator.
Creating an Operation Generating Tool Paths You will generate the tool path to remove the material along the outside edge of the part.
Choose the Program Order View icon
in the toolbar.
Notice that slashed red circles appear in front of both operations. This indicates that the tool paths for both operations must be regenerated to reflect the changes made in the MILL_BND parent group. Choose the PROGRAM icon and MB3
Generate.
OK to accept the first tool path generation. OK to accept the second tool path generation. Refresh the display. Exclamation points now appear in front of the operations indicating that the operations have been generated but have not yet been postprocessed or exported.
66
Creating an Operation Reordering Operations The Program Order View displays the order in which operations will be executed on the machine tool. Notice that the finishing operation precedes the roughing operation. You will change the order in which operations are listed in the program so that the finishing operation follows the roughing operation. Choose the FINISH_FLOOR icon and MB3
Cut.
The operation you choose in the next step is the object below which the pasted operation will appear. Choose the ROUGH_FOLLOW icon and MB3
Paste.
FINISH_FLOOR is now the second operation in the program sequence.
Creating an Operation Visualizing the Tool Paths
67
You will now verify that the negative boundary offset you specified earlier in the parent group removes the excess material along the outside edge of the part. Choose the PROGRAM object.
Choose the Verify Toolpath icon
in the toolbar.
Choose the Dynamic tab. Choose the Play Forward icon. The operations execute in the correct order and the excess material along the outside edge of the part is completely removed.
OK to complete the Toolpath Visualization.
Creating an Operation Reselecting the Tool Parent Group You will change the tool used in the finishing operation.
Choose the Machine Tool View icon
in the toolbar.
Expand the tool object so you can see the operations. Double-click on the FINISH_FLOOR icon.
68
The FINISH_FLOOR dialog displays, allowing you to edit the operation. Choose Tool: UGTI0201_063 and Reselect.
The Reselect Tool dialog displays, allowing you to choose a new parent group or to define a new tool. Choose UGTI0201_076.
The tools available in this list are the same as those that appear in the Machine Tool view of the Operation Navigator. OK to accept the tool. The dialog now displays UGTI0201_076 as the tool used in the operation.
Remember, you can also respecify the tool by dragging and dropping, or by cutting and pasting the operation onto the tool object.
69
Creating an Operation Completing the Operation You will complete the operation and observe how the Operation Navigator now displays UGTI0201_076 as the parent group. OK to complete the FINISH_FLOOR operation. Expand the object to see the operation. The Operation Navigator now displays UGTI0201_076 as a parent of the FINISH_FLOOR operation.
A slashed red circle change.
indicates that the tool path must be regenerated to reflect the tool
Creating an Operation Generating the Tool Path You will generate the tool path to update the operation status. Choose the FINISH_FLOOR icon and MB3
OK to accept the tool path generation. Close the part file.
Generate.
70
Updating a Legacy Operation Dialog Legacy operation dialogs can be customizing so that they appear the same as the dialogs for newly created operations.
Updating a Legacy Operation Dialog Opening the Part File Open part file mfe_legacy_1.prt from the mfe subdirectory. Choose Application
Manufacturing.
Updating a Legacy Operation Dialog Viewing the Legacy Operation Dialog You will first view an existing legacy operation dialog. You will then customize it by distributing the parameters among property pages to make the dialog shorter. In the Program Order View of the Operation Navigator, double-click on the
71 ROUGH_TURN_OD icon to display the operation parameters dialog.
The dialog is very large and in some cases it may be too large for the viewing screen. Click on the dialog so that it is active and press the Esc key to dismiss it.
Updating a Legacy Operation Dialog Customizing the Operation Dialog You will customize the dialog box and make it smaller by adding Main, Groups and Viewing property pages. Highlight ROUGH_TURN_OD in the Operation Navigator.
Press MB3 and choose Object
Customize.
The Customize Dialog dialog displays.
Updating a Legacy Operation Dialog Adding a Main Page The first property page you will add is the Main property page.
72 Key in Main in the Label field and choose the Property Pages icon.
Start Page Main and End Page Main are added to the Items Used list box. Moving the End Page Main to the bottom of the items used will put all those items on the Main page. With End Page Main highlighted, choose the Move Down arrow until End Page Main is the last item in the list.
When you are finished moving End Page Main to the bottom, the list box will appear as illustrated below.
Updating a Legacy Operation Dialog Adding a Groups Page The second property page you will add is the Groups property page. Key in Groups in the Label field and choose the Property Pages icon.
73
Start Page Groups and End Page Groups are displayed at the bottom of the list box.
Scroll to the top of the Items Used list box, highlight Group Editing, and choose the Move Down arrow until Group Editing is between the Start Page and End Page of Groups.
When you are finished moving Group Editing, the list box will look as illustrated below.
Updating a Legacy Operation Dialog Adding a Viewing Page The last property page you will add is the Viewing property page.
74 Key in Viewing in the Label field and choose the Property Pages icon.
Move End Page Viewing and Start Page Viewing to the end of the list box using the Move Down arrow. The list box should look as illustrated below.
Highlight Save View and choose Add.
Choose the Move Up arrow so that Save View is between the Start Page and End Page of Viewing as illustrated below.
OK to complete the dialog customization.
Updating a Legacy Operation Dialog Viewing the Dialog
75 The parameters have been divided among three property pages. Double-click on the ROUGH_TURN_OD icon to display the operation parameters dialog.
The top of the dialog displays the three tabs found in newly created turning operations.
Cancel the Dialog. Close the part file.
Creating Operation Sequences In this lesson, you will learn how to create a program containing a predefined sequence of operations. A Process Assistant will provide step-by-step instructions on how to create the sequence of operations.
76
Creating a Sequence You will create a sequence of operations designed to machine a die. Although specific parameters may vary, the process of creating any sequence is similar.
Open part file mfe_sequence_1.prt from the mfe subdirectory.
77
Choose Application
Manufacturing.
Creating a Sequence Defining the Machining Environment Because this part has not yet been saved in the Manufacturing application, the Machining Environment dialog displays. You will choose a CAM Session Configuration and a CAM Setup Choose mill_contour as the CAM Session Configuration.
Die_Sequences and Mold_Sequences are generic sequence setups supplied with the system. Other setups may also be available depending on your working environment. Choose die_sequences as the CAM Setup.
Choose Initialize.
Creating a Sequence Using the Process Assistant
78 You will begin following the step-by-step instructions provided by the CAM Process Assistant. OK to continue with the assistant.
Creating a Sequence Defining the MCS Step 1 of the Process Assistant prompts you to define the Machine Coordinate system. You may specify new MCS parameters or accept the current MCS. OK to accept the current MCS.
Creating a Sequence Defining the Clearance Plane Step 2 of the Process Assistant prompts you to define the clearance plane. Be sure Clearance has been turned on and choose Specify.
79
Choose Plane Subfunction. Choose Two Lines. Select the two lines illustrated below.
OK to continue to the next step.
Creating a Sequence Defining the Part Geometry Step 3 of the Process Assistant prompts you to define the part geometry. Choose Select. Select the part body as illustrated below.
80
OK to complete the selection. OK to continue to the next step.
Creating a Sequence Defining the Blank Geometry Step 4 of the Process Assistant prompts you to define the blank geometry. Choose Select. Select the blank body as illustrated below.
OK to complete the selection. OK to continue. At this point in the process, the Setup has been created and you are prompted to follow the instructions in the Information window.
81 OK to continue.
Creating a Sequence Creating the Geometry Parent Group The next set of steps defines the geometry parent group. You will follow these steps to create a sequence of operations:
Choose the Create Geometry icon
in the toolbar.
Choose Sequence_Zlevel as the Subtype and Workpiece as the Parent Group.
OK to create the geometry parent group. Dismiss the Information window.
Creating a Sequence Defining the Cut Area The next step prompts you to define the cut area. Choose Select.
Choose Features as the Selection Option.
82 Select the Surface Region as illustrated below.
OK to complete the selection. OK to continue to the next step.
Creating a Sequence Defining the Trim Boundary The next step prompts you to define the trim boundary. A trim boundary is used to constrain the cut area. Because you are going to machine the entire part, the program does not require a trim boundary. OK to proceed to the next step.
Creating a Sequence Choosing the Operation Types The next step prompts you to choose optional flowcut operations to include in the sequence.
You will not include these operations. OK to proceed to the next step.
Creating a Sequence
83
Completing the Sequence The final step prompts you to specify whether or not the tool paths are to be generated immediately after creating the operations. Due to the potential processing time involved for this sequence, you will not generate the tool paths. Be sure Generate Tool Paths is off.
OK to create the sequence of operations. In the Program Order View of the Operation Navigator, expand the objects to display the sequence of operations.
The operations would machine the part as illustrated below.
Creating a Sequence Respecifying the Session Configuration
84 The CAM Session Configuration you specified at the beginning of this lesson provides CAM Setups only for mill contour type operations. Before continuing on to other courses, you should choose a CAM Session Configuration that allows you to create all types of operations including Milling, Drilling, Turning, and Wire EDM. Choose Tools
Operation Navigator
Delete Setup from the main menu bar.
OK to delete the setup. The cam_general configuration file provides the widest range of available setups for your current work session. Choose cam_general in the CAM Session Configuration list. The specific setup you choose at this time is not critical since the setup can be respecified when creating an operation. Choose the mill_planar setup. Choose Initialize. Close the part file.
UG/Post Postprocessing is the preparation of machine code used to drive a specific machine tool. In this lesson, you will learn how to postprocess using UG/Post.
85
Postprocessing with UG/Post UG/Post converts the internal tool path containing events and motions into a format compatible to the machine tool's controller. To postprocess, UG/Post requires a tool path and a postprocessor. Open part file mfe_ugpost.prt from the mfe subdirectory.
Choose Application
Manufacturing from the menu bar.
86
Postprocessing with UG/Post Replaying an Operation Operations must contain internal tool paths in order to be postprocessed. You will replay the existing tool path. Expand the objects so you can see the operations. Repost status ( ) means that the tool paths for the operations in the program have been generated, but they have not been postprocessed or exported from the part file. Choose the operation named FIXED_CONTOUR.
Choose MB3
Replay.
The tool path is a simple follow pocket cut pattern.
Postprocessing with UG/Post Listing the Internal Tool Path The tool motion to cut the path you just displayed is stored in the part file as an internal tool path. A machine tool cannot use the internal path as commands because they are written in Standard APT. You will display the internal tool path using the List function.
87 Choose MB3
Toolpath
List.
The internal tool path is listed in an Information window.
UG/Post converts the internal tool path containing events and motions into a format compatible to the machine tool's controller. For example, the FEDRAT/MMPM,250.0000 command might be converted to the format F250.0 and the GOTO/0.0000.45,0000,3.0000 might be converted to G00X0.0000Y45.0000Z3.0000. Dismiss the Information window.
Postprocessing with UG/Post Accessing the UG/Post Postprocessor UG/Post will process only one program or operation at a time. You will postprocess a simple program containing two operations. Choose the PROGRAM icon.
88
Choose UG/Post Postprocess from the toolbar. An alternate way to access UG/Postprocess is to choose Tools Output UG/Post Process from the menu bar.
Operation Navigator
Postprocessing with UG/Post Choosing a Postprocessor The generic postprocessors provided by the system are displayed in the Available Machines list box. You will choose a postprocessor for a 3 axis milling machine tool. Highlight the MILL 3_AXIS postprocessor.
All of the operations contain 3 axis tool paths, so the MILL_3_AXIS machine is appropriate to use here.
More About: Postprocessors
The postprocessors provided by the system are displayed in the Available Machines list box.
89
These postprocessors are stored in the main directory in Mach/resource/postprocessor. The environment variable UGII_CAM_POST_CONFIG_FILE in ugii_env.dat points to a file named template_post.dat. The Available Machines are listed in the template_post.dat file and each machine entry points to the correct tcl and def files for that machine tool. System administrator privileges are required to change these files.
Postprocessing with UG/Post Specifying a Write Directory By default, the postprocessor will create a file in the mfe directory with the root name of the part file and a "ptp" extension. You probably cannot write to the mfe directory and will need to change to a directory you can write to. Choose Browse.
Set the Look in: field to a directory you can write to. Key in ugpost_output.ptp in the File name: field.
The file extension "ptp" is an abbreviation for paper tape punch file, a historical holdover from the use of paper tape to read n/c programs into machine tool controllers. You can use any file extension you prefer.
90 OK to accept the output specification. OK to postprocess the tool paths. This will take some processing time. The tool paths are postprocessed and listed in an Information window. The file has been created and saved in the specified directory. Dismiss the Information window. Close the part file.
Graphics Postprocessor Module (GPM) Postprocessing prepares machine code for use in driving a specific machine tool. In this lesson, you will learn how to create and edit a Cutter Location Source File (CLSF) and how to postprocess the CLSF using the Graphics Postprocessor Module (GPM).
91
GPM is a legacy product. It is covered here because it is still commonly used at many sites. Postprocessing should now be done using UG/Post.
Creating a CLSF The CLSF is an ASCII text file containing Standard APT commands. A CLSF is required when using a 3rd party postprocessor or the legacy Graphics Postprocessor Module (GPM). The first step in creating a Cutter Location Source File (CLSF) is to select the operations from which you would like to write the internal tool paths to the operating system file. A single part file might contain tool paths for different machine tools (for example, lathes and 3 axis mills) and you would not want to have tool paths for different machine tools in the same CLSF. If this were the case, you would organize the different types of machining into separate programs, such as a 3 axis mill program and a lathe program, so that you could create separate CLSF's. In the current part file, all the tool paths are for a 3 axis milling machine and are all included in the NC_PROGRAM object.
Creating a CLSF Opening the Part File
92 Open part file mfe_post_1.prt from the mfe subdirectory.
Choose Application
Manufacturing from the toolbar.
Ten operations with a Repost status ( ) are displayed in the Program Order View of the Operation Navigator. Repost status means that the tool path for the operation has been generated, but it has not been postprocessed or exported from the part file.
Creating a CLSF Selecting the Operations You will select the operations from which you would like to write the internal tool paths. Highlight the NC_PROGRAM object.
Highlighting the object selects all of the operations contained within the object.
Creating a CLSF Outputting the CLSF You will specify the file name and directory to which you will output the CLSF.
93
Choose the Output CLSF icon in the toolbar. An alternate way to Output CLSF is to choose Tools CLSF in the menu bar.
Operation Navigator
Output
Choose Browse.
Make sure the Look in field is a directory to which you have write access. Key in 3axis_mill_program in the File Name field and OK to accept it.
CLSF_STANDARD is the default format. OK to accept CLSF_STANDARD as the format and write the file. CLSF_STANDARD is the default format. OK to write the file. The Information window displays a listing of the output written to that file. Dismiss the Information window. More About: CLSF Formats
When you choose the Output
CLSF option, a string of environment variables is executed.
The variables are, roughly, UGII_CAM_CONFIG_DIR UGII_CAM_CONFIG, in the ugii_env.dat file, which points to cam_general.dat. The file cam_general.dat has a pointer TEMPLATE_CLSF that points to the file template_clsf.dat in the Mach/resource/template_set/tool_path directory. The cam_general.dat file determines what you will see in the list box of the CLSF formats dialog. Notice the five text strings on the far left above. These text strings are the ones displayed in the dialog below:
94
The first of the formats listed, CLSF_STANDARD, uses two files to create output in the APT-like format familiar to Unigraphics NX users. These two files are clsf.tcl and clsf.def. clsf.tcl is a tcl file -Tcl (Tool Command Language) is a programming language. Tcl is distributed free from a number of different web sites and the programs written in it are very portable between different operating systems. The clsf.tcl file is an event handler; it tells the Manufacturing Output Manager (MOM) what to do with the information stored in the operations which have been selected for output. One command in this tcl file, set mom_kin_clsf_generation TRUE, is particularly important as it tells MOM to use an alternate path to a faster, optimized C code executable for generating either the GOTO values or the Post commands. clsf.def defines the format for the output generated by MOM from the event handler, clsf.tcl and the post commands generated by the parameters stored in the operations being processed. The MOM is multifunctional in managing manufacturing output. Some of its functionality can be visualized in the illustration below:
95
The Output CLSF selection on the left leads to various intermediate clsf formats, while the UG/Post Postprocessor option on the right leads directly to machine code. The MOM analyzes the relationships between the various CAM objects and the pointers from operations to sections of the Internal Tool path. These relationships and the tcl and def files, determine the format of the output. The CLSF_STANDARD is designed to handle legacy manufacturing data. To run faster, the switch set mom_kin_clsf_generation TRUE is set to use previously generated post commands.
96 CLSF_COMPRESSED provides a shortened form of the CLSF useful for determining which tools are used and when. The output is the same as CLSF_STANDARD, without the GOTO values. CLSF_ADVANCED will extract operation parameters, such as tool information and automatically generated post commands, in addition to the tool positioning (X,Y,Z,I,J,K) data CLSF_BCL generated binary centerline information for controllers requiring that output. CLSF_ISO will generate International Standard format center line files. A user defined output format can be added by editing the template_clsf.dat file and adding a format type, e.g. MY_CUSTOM_OUTPUT, linked with a tcl file and a def file. A good starting point for these would be to copy and rename the bcl.tcl and bcl.def files, perhaps to something like custom.tcl and custom.def. CLSF_IDEAS_MILL and CLSF_IDEAS_MILL_TURN are formats specifically for the IDEAS postprocessor.
Creating a CLSF The CL Source File Manager The CLSF exists as an independent ASCII file. You will now use the CLSF Manager to examine CLSF file. The CLSF Manager allows you to Edit, Reorder, Delete and Replay tool paths, and to List the CLSF. Editing the CLSF should be avoided if possible, and will therefore be discussed only briefly. It is always better to edit the operation and regenerate the tool path because the operation parameters are permanently stored with your part file. Choose Tools
CLSF in the toolbar.
You must choose the CLSF that you want to open. The file mfe_tpmgr_1.cls is the same as the file you just created. Select mfe_tpmgr_1.cls from the mfe directory and then OK.
The CLSF Manager dialog displays. The dialog contains a list of all the tool paths in the current CLSF.
97
Creating a CLSF Filtering the Tool Path Names You can restrict the list of tool paths to only those that are blanked or unblanked, or to only those that do not have an associated operation in the part file.
A Blanked tool path is temporarily removed from the paths displayed during a tool path replay. An Orphan is a tool path that has no associated operation. An Orphan is also anything that can be inserted into the CLSF ( a PPRINT, macro call, etc.) that does not have a Start-of-Path or End-of-Path statement. Choose Blanked from the option menu. Notice that one tool path, CORNER5, is listed. Set the Show option back to All. All the tool paths are listed again.
Creating a CLSF Reordering Tool Paths You can use Cut and Paste to remove one or more tool paths or to reposition them in the CLSF. You will cut the MULTI-LEVEL tool path that roughs out the pocket and paste it before POCKET1. Choose MULTI-LEVEL from the listing window.
98 Choose Cut.
Highlight TLCHG1.
The cut tool path will be pasted after the highlighted tool path (after TLCHG1). Choose Paste.
If you had not highlighted TLCHG1, the cut tool path would have been placed as the first tool path in the list.
Creating a CLSF Deleting Tool Paths You can also permanently delete one or more tool paths from the CLSF. Remember that you are only removing the tool path from the CLSF - the operation and the internal tool path which are stored in the part file are not affected. Highlight POCKET2 and choose Delete.
99
A confirmation message appears listing the names of the tool paths that will be deleted. If you delete the tool path, you will not be able to get it back using Paste. To get it back, you would have to regenerate the tool path and create another CLSF. OK to delete the tool path from the CLSF.
Creating a CLSF Listing Tool Paths You can list the text of one or more tool paths in the CLSF. Select CORNER1 in the list box. Be sure you do not use the List button in the CLSF Actions section - that will list the entire CLSF. Choose List in the Tool Path Actions section.
The selected tool path is listed in the Information Window.
100
Dismiss the Information window.
Creating a CLSF Replaying Tool Paths You can replay the tool paths in the CLSF. First, you will use the Filter Methods section to display just the corner tool paths. Key in c* in the By Name field. Turn on the By Name button.
Only those tool paths beginning with "c" are now listed. Choose Select All. You can stop the display of the tool paths at any time by choosing Stop on the Work in Progress dialog. Choose Replay in the Tool Path Actions section.
101 The tool paths display graphically on the part. Turn off the By Name option to deselect the tool paths. All the tool paths are listed again.
Creating a CLSF Optimizing the CLSF Optimization is very useful when it is time to send the program to the shop floor. It can help with some of the tedious cleanup. Optimization allows you to: preselect a tool for the next tool path. suppress duplicate tool change commands in consecutive tool paths. remove postprocessor commands which are generated (or inserted) at the end of each tool path. verify that a tool change command is output when the tool parameters change. Choose List from the CLSF Actions section.
All of the tool paths in the CLSF are listed in the Information window. Look at line 50 in the listing. It is the first LOAD/TOOL, 1 ... command.
Look at line 160 in the listing. It is an unnecessary duplicate LOAD/TOOL , 1 ... command.
Dismiss the Information window. Optimizing will strip out the duplicate tool changes.
102 Choose Optimize.
The CLSF CONTROL dialog displays. The default settings will remove the duplicate tool changes. OK to optimize the CLSF.
Creating a CLSF Verifying the Optimization You can verify that the duplicate tool changes have been removed. Choose List from the CLSF Actions section. The duplicate tool change that was located at line 160 has been removed.
Dismiss the Information window.
Postprocessing with GPM There are two elements necessary for postprocessing with the Graphics Postprocessor Module: CLSF - The tool path Cutter Location Source File. MDF - The Machine Data File The Graphics Postprocessor Module (GPM) uses the Machine Data File (MDF) to convert the CLSF into a format compatible to the machine tool's controller. The CLSF is an ASCII text file containing Standard APT commands. A CLSF is required when using a 3rd party postprocessor or the legacy Graphics Postprocessor Module (GPM).
103 The Machine Data File (MDF) describes the characteristics of a machine and the required format for its accompanying controller. Each MDF contains data the GPM needs for postprocessing tool paths. The MDF is an ASCII file and has an extension of .mdfa. When you are postprocessing, the GPM does the following in this order: Reads a specified CLSF and MDF Formats the CLSF according to the MDF instructions Outputs a postprocessed tool path This sounds involved, but it actually is not. The GPM is provided by Unigraphics NX and the MDF probably already exists at your company.
Postprocessing with GPM Beginning to Postprocess You will begin postprocessing with the GPM. Choose Postprocess in the CLSF Actions section.
First, you must specify the GPM, CL file, and MDF. You can change the GPM using the Specify option under Postprocessor Name.
You will not need to specify a different postprocessor for this exercise because the system defaults to the GPM program provided with the current distribution of Unigraphics NX. You can use the Specify option under Input File Name to change the CLSF. Notice that it has defaulted to mfe_tpmgr_1, which is the CLSF you want to postprocess.
104
Postprocessing with GPM Specifying the MDF You must supply the name of the MDF. Choose Specify under MDF Name.
Choose mfe_3axis.mdfa from the mfe subdirectory and OK.
The name of the MDF file displays on the NC Postprocessing dialog.
Postprocessing with GPM Run Time Options Run time options override the non-machine related options in the MDF. For example, you can change the MDF setting for the printed format of the postprocessed tool path, or change the output units from inches to millimeters.
105
NC Output - Selects the destination for the finished machine tool program. This program is frequently referred to as the tape image, punch file (in the past it was usually punched out on paper tape) or M and G code file. Listing Output - Selects the destination for the listing output. The Listing Output is a combination of the CLSF input and the NC Output and is frequently used for debugging and other tasks. Input Units - Specifies the input units to be used. Listing Format - Can be set to Column (the listing is formatted into columns), Packed (the listing is packed without column divisions), or MDF Defined. Listing Commentary - Controls the listing of commentary data. It can be set to Yes, No, or MDF Defined.
Postprocessing with GPM Specifying the NC Output NC Output options allow you to set the destination of the output.
File - The output is an ASCII format file having a ".ptp" extension. You can edit this file. Paper Tape - Outputs the file to a tape punch. None - All postprocessor output is suppressed. MDF Defined - Defaults to the setting in the MDF. Set NC Output to None.
106
Postprocessing with GPM Specifying the Listing Output There are five Listing Output options.
File - Sends the listing to a file with the specified file name. Line Printer - Sends the output to the system printer. Terminal - The listing is displayed in the status window of your terminal. None - All postprocessor output is suppressed. MDF Defined - Defaults to the setting in the MDF. Set Listing Output to Terminal.
Postprocessing with GPM Initiate Postprocessing Postprocess initiates postprocessing on the current CLSF file. Choose Postprocess.
The CLSF is postprocessed and the output is displayed in a window.
107 If you had directed the postprocessing output to a file, machine code as below would have been written to the file:
A Message is displayed informing you that the postprocessing is finished and instructing you to press Return to continue. Press the Enter key. Cancel the NC Postprocessing dialog. Cancel the CLSF Manager dialog. Ordinarily, you would save the file at this time. Cancel the Save CLSF dialog. Close the part file.
Shops Shops setups are template files that utilize a Process Assistant designed to step the occasional user (such as the shop floor machine operator) through the process of creating an operation.This lesson provides one general example of how to use a Shops template and how to follow the Process Assistant to create a single operation.
108
Open part file mfe_shops_1.prt from the mfe subdirectory. Choose Application
Manufacturing.
Defining the Setup You will follow the steps provided by the Process Assistant to define the setup. You will define the Machine Coordinate system, the clearance plane, and the blank geometry.
Defining the Setup Defining the Machining Environment
109 Because this part has not yet been saved in the Manufacturing application, the Machining Environment dialog displays requiring you to choose a configuration and a setup. Choose shops_diemold as the CAM Session Configuration.
If you have purchased the Shops bundle, only one Shops choice appears here. Shops setups are templates supplied with the system. Additional setups may also be available, depending on how your system has been customized. Choose shops_mill_contour as the CAM Setup.
Choose Initialize.
Defining the Setup Defining the MCS A sequence of Process Assistant dialogs will now begin stepping you through the process of defining the setup. Step 1 of the Process Assistant prompts you to define the Machine Coordinate system. You may specify new MCS parameters or accept the current MCS. OK to accept the current MCS.
110
Defining the Setup Defining the Clearance Plane Step 2 of the Process Assistant prompts you to define the clearance plane. Turn on the Clearance option and choose Specify.
Choose Plane Subfunction. Choose Two Lines. Select the two lines illustrated below.
111
OK to continue to the next step.
Defining the Setup Defining the Blank Geometry Step 3 of the Process Assistant prompts you to define the blank geometry. Choose Select. Select the blank body as illustrated below.
OK to complete the selection. OK to accept the blank geometry. At this point, the setup has been created.
Choose the Geometry View icon
in the toolbar. and click on the plus (+) sign to fully
112 expand the object.
The MCS_MILL and WORKPIECE objects have been created using the parameters you just defined.
Creating the Operation You are now ready to begin creating the operation. Choose WORKPIECE and MB3
Insert
Operation.
Choosing WORKPIECE assures that it will the parent group of the operation. Be sure shops_mill_contour is displayed as the Type. The Type determines the available Subtype icons and parent groups. Choose ZLEVEL_FOLLOW_CORE as the Subtype.
The Subtype determines parameters specific to the operation such as the cut pattern. OK to begin creating the operation.
Creating the Operation Specifying the Tool
113
A sequence of Process Assistant dialogs will now begin stepping you through the process of defining the operation. The first step in creating the operation is to define the tool and the method. Be sure Tool: None is chosen. Choose Select.
Choose New. Choose the MILL icon.
The tool name defaults to MILL based on the Subtype you chose. OK to begin defining the MILL tool parameters. Key in the following values to define the tool.
OK to finish defining the tool.
Creating the Operation Verifying the Method The method defines parameters such as Intol, Outtol, and part stock. Be sure MILL_ROUGH has been specified as the Method and OK to accept it.
114
Creating the Operation Displaying the Blank Geometry Blank geometry has been defined in the Workpiece parent group. Choose Display to highlight the Blank geometry.
OK to continue to the next step.
Creating the Operation Specifying the Part Geometry The third step in creating the operation specifies the part geometry. Choose Select. Choose the part body as illustrated below.
115
OK to complete the selection. OK to accept the part geometry.
Creating the Operation Specifying the Cut Depth The fourth step defines the depth of each cut level. OK to accept the default of 6.0.
Creating the Operation Generating the Tool Path You will now generate the tool path.
Choose the Generate icon. Turn off the Pause After Display and Refresh Before display options. This allows you to generate all the cut levels at once and to continue viewing them after they have generated. OK the Display Parameters dialog.
116 OK the error. The error message simply informs you that the tool cannot cut to the bottom of the part.
At this point in the process, you are free to modify operation parameters as you choose. OK to complete the ZLEVEL_FOLLOW_CORE operation. Refresh the display. Choose Edit Blank Blank in the toolbar and select the blank geometry so that only the part geometry displays as illustrated below.
Creating the Operation Visualizing the Uncut Material The Show 3D option creates a faceted model of the remaining uncut material.
Choose the Shaded icon
in the toolbar to display the part as a shaded solid.
117 Choose ZLEVEL_FOLLOW_CORE and MB3
Workpiece
Show 3D.
It will take a moment to generate the faceted model.
The faceted model graphically represents the uncut material that remains after generating the ZLEVEL_FOLLOW_CORE operation. Refresh the display. Close the part file.
Shop Documentation In this lesson, you will learn how to create shop documentation for use by machine tool operators. There are two formats for shop documentation: text format and HTML (Hyper Text Markup Language) format. The text format is standard plain text. HTML format (illustrated below) is the type of format read by web browsers and allows you to include graphics and other visual enhancements to your documentation.
118
Creating Shop Documentation The following is a simple example of how to create and save a tool list in text format. Open part file mfe_shop_doc_1.prt from the mfe subdirectory.
Choose Application
Manufacturing.
119
Creating Shop Documentation Displaying the Program Order View Choose the Program Order View icon
in the toolbar.
Expand the objects so you can see the operations.
You will create shop documentation for these two operations.
Creating Shop Documentation Creating the Tool List Choose Information
Shop Documentation in the menu bar.
You can also use the Shop Documentation icon Documentation.
on the toolbar to access Shop
Templates defining different formats for the output of shop documentation display in the Part Documentation dialog. Choose Tool List (TEXT).
Choose Browse and select a directory to which you have write access.
120
The default output file name is the same as the part file, with the extension .txt. OK to accept the default output file name. The text file is written to the specified directory and displayed in an Information window. This file can be sent with the N/C program to the machine operator with instructions on how to set up the stock for machining, etc. Dismiss the Information window. Close the part file.
Creating a Tool List for a Selected Program A tool list can be created for a selected program when postprocessing. This is useful when you wish to create shop documentation for a single program, and not the entire part.
121 To create a tool list for a program, select the program in the Operation Navigator, choose the UG/Post Postprocess icon in the toolbar, and choose one of the Program Tool List templates in the list box.
Creating a Tool List for a Selected Program Opening the Part Open part file mfe_shop_doc_2.prt from the mfe subdirectory.
Choose Application
Manufacturing.
Creating a Tool List for a Selected Program Displaying the Program Order View Choose the Program Order View icon
in the toolbar.
The Operation Navigator displays three programs. Choose PROGRAM2 so that it highlights.
Creating a Tool List for a Selected Program Creating the Tool List Choose the UG/Post Postprocess icon in the toolbar. Templates defining different formats for the output of shop documentation display in the Part Documentation dialog.
122 Choose Tool List (text). Choose Browse and select a directory to which you have write access.
The default output file name is the same as the part file, with the extension .txt. OK to accept the default output file name. The text file is written to the specified directory. This file can be sent with the N/C program to the machine operator with instructions on how to set up the stock for machining, etc. Close the Browser. Close the part file.
123
PLANAR AND CAVITY MILLING Planar Milling - Profiling This course will teach you how to create Planar and Cavity Milling operations. Planar and Cavity Milling operations create tool paths that remove material in planar layers, by cutting levels perpendicular to the tool axis.
Planar Milling is intended for parts with vertical walls and planar islands and floors normal to the tool axis. Part and blank material is defined using boundaries. It is used for roughing and finishing. Cavity Milling is intended for parts with tapered walls and contoured floors. Part and blank material can be defined using boundaries, faces, curves, and bodies. It is used for roughing. Audience The audience for this course is Unigraphics NX Manufacturing application users who want to machine 3-axis parts containing pockets, profiles, or cavities. Prerequisites The prerequisite for this course is the Manufacturing Essentials CAST Online Library course. Course Contents Planar Milling - Profiling — You will learn how to create single pass Planar Milling tool
paths that follow open boundaries to machine reference surfaces for precise placement in fixtures. Planar Milling - Single Level — You will learn how to create a single-level Planar Milling
operation.
124 Planar Milling - Multi-Level — You will learn how to create multi-level Planar Milling
operations, clean up islands, and create and edit boundaries. Planar Milling - Multi-Region — You will learn how to create a multi-region Planar Milling
operation that will cut several pockets with varying depths. Face Milling — You will learn how to create a Face Milling operation that finishes the faces
of a part. You will also learn several ways to cut across open and closed voids and learn how to create mixed and manual cut patterns. Cavity Milling — You will learn how to create Cavity Milling operations that rough out
cavities and cores. You will also learn how to use a faceted body to perform rest milling. Z-Level Milling — You will learn how to profile the part at each cut level and then constrain
the cut region using the silhouette or "shadow" of the part. You will specify a Steep Angle to profile only the steep areas left unmachined by a previous Fixed Axis Surface Contouring operations. You will also learn how define a Cut Area and then further constrain the cut region using a trim boundary. Planar and Cavity Milling Project — You will create a program that roughs, semi-finishes,
and finishes a part containing multiple cavities.
Creating the Master Model Assembly You will use the Master Model concept to setup the part. This metric part file will be the top level assembly part file containing the machining operations. It has some predefined geometry in it which has been modeled to allow positioning of the part in the fixture
You will enter the Manufacturing application and define the part and blank geometry in the Workpiece parent group. Operations can then inherit the parameters defined in the Workpiece parent group.
125
Creating the Master Model Assembly Opening the Part The first step is to open a top level assembly part. Open part file pln_assy_1.prt from the pln subdirectory. Choose Application
Assemblies.
Creating the Master Model Assembly Adding Components to the Assembly You will add a component that defines the part geometry.You may have to turn on the Assemblies toolbar under View Toolbars Customize
Choose the Add Existing Component icon
from the Assemblies toolbar.
Choose Choose Part File. Choose pln_pmp_1.prt from the pln subdirectory and OK to accept it. The Add Existing Part dialog displays with the Positioning set to the Absolute coordinate system. OK to accept this part file and positioning mode. Make sure the values in the Base Point coordinate fields are all set to 0.000 and WCS and OK to accept them.
126
Cancel the Add Existing Part dialog.
Creating the Master Model Assembly Entering the Manufacturing Application Choose Application
Manufacturing.
The Machining Environment dialog displays because the part file has never been saved in the Manufacturing application. Be sure cam_general has been chosen in the CAM Session Configuration listbox. Choose mill_planar in the CAM Setup: listbox.
Choose Initialize.
Creating the Master Model Assembly Creating a Permanent Boundary Planar Milling operations can use boundaries to control the tool motion. Choose Tools
Boundary in the toolbar.
You will create an open boundary using the line extending across the top of the part. You will make it an "On" condition boundary so that the the tool center point positions directly on the boundary.
127 Choose Create. Set Tool Position to On and Boundary Type to Open. Select the line at the left end as illustrated below.
OK twice to create the boundary. The origin of a boundary (indicated by a small circle) is determined by where the curve is selected. The origin should be at the left end. The "tick mark" displays on both sides to indicate that it is an "On" boundary, meaning that the center of the tool will follow the boundary.
Cancel the Boundary Manager dialog.
Creating the Master Model Assembly Editing the Workpiece You will edit the Workpiece object so that it defines the part and blank geometry.
Choose the Geometry View icon
in the toolbar.
Expand the MCS_MILL object in the Operation Navigator. Double-click on the WORKPIECE icon to edit the geometry group.
128
Creating the Master Model Assembly Defining Blank Geometry Choose the Blank icon, then Select.
Select the white rectangular block as the blank geometry.
OK the Blank Geometry dialog.
Creating the Master Model Assembly Defining Part Geometry Choose the Part icon, then Select.
Select the green solid as the part geometry.
129
OK the Part Geometry dialog. OK the MILL_GEOM dialog.
Creating the Master Model Assembly Grouping Operations It is convenient to group operations under program objects by the type of machining they do, by the setups they use, or other criteria particular to your manufacturing processes.
Choose the Program Order View icon
in the toolbar.
Highlight PROGRAM.
Choose MB3
Rename.
Change the program name to ROUGHING_PROG.
This program name is easy to recognize as containing all the roughing operations. Finishing operations could be contained in another program such as FINISHING_PROG.
Creating the Master Model Assembly Creating a New Tool The open boundary was created in order to cut the top face of the stock with a single pass. To provide safe clearance to bring the tool to the cut depth, the boundary begins 60 mm in negative XC from the left side of the stock. The boundary ends 60 mm in the positive XC direction from the right side of the stock.
130
Choose the Create Tool icon
in the toolbar.
You will create a 100 mm diameter tool that is 25 mm long and has 20 inserts. Choose the T_CUTTER icon and key in TMAX100 in the Name field.
OK to begin creating the tool. Key in 100.00 in the Diameter field.
Key in 20 in the Number of Flutes field.
The tool diameter and number of flutes are used in the calculation of the feeds and speeds generated by using the Reset from Table option on the Feeds and Speeds dialog. The Material for the tool is set to HSS, High Speed Steel. Choosing this option and changing the tool material will also affect the speeds and feeds.
OK to create the tool. Choose the Machine Tool View icon
in the toolbar.
The tool displays in the Operation Navigator.
Facing the Top of the Stock
131 You will create a Planar Mill operation that uses a large cutter (100 mm diameter) to machine the top face in a single pass.
Facing the Top of the Stock Creating the Operation Choose the Create Operation icon
in the toolbar.
Be sure mill_planar is specified as the Type. Choose the PLANAR_MILL icon.
Key in RUFTOP100MM in the Name text field.
Specify the following parent groups.
132
Choose OK to begin creating the operation.
Facing the Top of the Stock Displaying the Tool Choose the Groups tab and choose Display to view the tool.
The tool will cover the entire top of the stock in one pass.
Refresh the graphics window.
Facing the Top of the Stock Startup Post Commands Before the part can be cut on the machine tool, the controller needs to be told to load the milling tool, turn on the spindle, and usually to turn on the coolant to flush away chips and
133 cool the tool and workpiece. You will define several beginning of path and end of path commands. Choose the Main tab. Choose Machine.
Choose Edit below the grayed-out Startup Commands option.
The number and types of available events in the Available list is determined by the setup of the configuration files.
Facing the Top of the Stock Adding a Load Tool Command Highlight the Tool Change command.
At the bottom of the dialog, the Add option is now available allowing you to add the Tool change command to the top of the tool path. Choose Add.
Since this is the first tool to be used in the program, you might want to have it loaded into tool position one in the magazine. Key in 1 in the Tool Number field and OK to accept it.
134
The User Defined Events dialog displays with the Tool Change event set to "Status=Active,Tool Number=1,Head Designation=None,Manual Tool Change-FALSE".
Facing the Top of the Stock Adding a Spindle On Command Highlight Spindle On and Add it. The Spindle On dialog displays. The RPM specified for a tool depends on the material to be cut, the cutting tool (whether it is a tool using inserts or various kinds of tool steel), the diameter of the tool, the strength or rigidity of the machine tool, machine tool horse power and the desired finish. Key in 194 in the Speed field and OK to accept it.
The Spindle On user defined event displays in the Defined list listbox.
Facing the Top of the Stock Adding a Coolant On Command Highlight Coolant On in the Available Functions listbox and Add it. OK to return to the User Defined Events dialog.
135 Three startup events have been defined so far.
These three commands are probably the most frequently used. There are many more commands listed under the Available list. The postprocessor might not require these user defined events in order to output the machine tool commands to load a tool or turn on the spindle to a given RPM. These T and S words can be automatically output based upon the stored data in the generated tool path and the structure of the machine tool's definition files. Highly variable commands, such as coolant, which can be set to on, flood, mist or tap, might be most easily defined as user defined events. User defined events might override the automatic events which would be output by UG/Post. The output is ultimately determined by the structure of the machine tool's postprocessor. OK to return to the Machine Control dialog. Note that the Startup Commands option is now On.
Facing the Top of the Stock End-Of-Path Post Commands End-Of-Path post commands can be added to turn off the spindle and turn off the coolant after the tool machines the top of the stock. Choose Edit located below the grayed-out End-Of-Path Commands option.
Highlight Coolant Off in the Available Functions list and choose Add. OK to return to the User Defined Events dialog. The user defined event Coolant Off is listed in the Defined list box.
136 Highlight Spindle Off and choose Add The Spindle Off dialog displays. OK to return to the User Defined Events dialog. The Spindle Off event is listed in the Defined list.
OK to return to the Machine Control dialog. Notice that the End-Of-Path Commands option is now On. OK to return to the PLANAR_MILL dialog. The commands you have just defined will be added to the output tool path when it is generated.
Facing the Top of the Stock Selecting the Open Boundary Choose the Part icon and Select.
Choose Boundary to define the Mode.
To select the boundary, you should center the cursor on the tic mark. Select the boundary.
137
OK the Boundary Geometry dialog.
Facing the Top of the Stock Specifying a Manual Engage Move The beginning of the engage move should be specified far enough off the part to provide a safe movement of the tool into the stock. The retract move should adequately disengage the part before beginning its rapid motion back to the home position. Choose Method under Engage/Retract.
Choose Ang Ang Dist for the Initial Engage.
The Distance, Angle 1, and Angle 2 text fields are now available. The Distance is the length of the engage move. Angle 1 is measured from the direction of the first cut move, counterclockwise in the plane of the part surface. Angle 2 is measured clockwise in a plane normal to the part surface. Specify the following Distance, Angle 1, and Angle 2 values.
138
These values will create an engage move in the direction of the cut, moving down at an angle of 45 degrees for a distance of 40 mm.
Facing the Top of the Stock Specifying a Manual Retract Move You will use the retract to a point method to disengage the tool from the boundary, by selecting the right end point of the line and specifying a rectangular offset relative to the WCS. Choose Point for the Final Retract.
Choose Rectangular for the Offset.
Select the line end point as illustrated below.
Key in the following offset values.
139
OK to return to the Engage/Retract dialog. An asterisk displays at the calculated retract point.
OK to return to the PLANAR_MILL dialog.
Facing the Top of the Stock Specifying the Floor The tool should cut the top of the part which is 2 mm below the white enclosing stock. To do this, you need to define the top of the part as the floor. Choose the Floor icon and Select.
Change the Filter to Face.
Select the top of the part (the top of the narrow wall).
140
OK to return to the PLANAR_MILL dialog.
Facing the Top of the Stock Changing the Cut Direction The current Cut Method is Follow Part. You will change it to Profile so that the tool can cut along the open boundary. Set the Cut Method to Profile.
You want the cut direction to be from left to right, so you must change the type of cut from Climb to Forward. By setting the Cut Direction to Forward, the tool motion is from the origin of the boundary (indicated by the small circle) to the end of the boundary in the direction indicated by the "tic" marks on the boundary. Choose Cutting. Choose Follow Boundary as the Cut Direction.
OK to return to the PLANAR_MILL dialog.
Facing the Top of the Stock Changing the Feed Rates The default feed rates are either 0.000, which results in tool motion at the rapid rate, or 250.0000 mmpm for the cut feed rate. While the program is being proofed, a slower motion is desirable.
141 The cut feed rate depends on the spindle rpm, type of cutter being used, the type of material being cut, and several other factors. The system will calculate these feed rate and spindle rpm values for you from data that your system administrator can customize. Choose Feed Rates. Note the Reset from Table option at the bottom of the dialog. Choosing this option will automatically set the spindle RPM and feed rates to those appropriate for the current tool and calculated from information in a database that can be customized for your site and machine tools. Choose Reset from Table. The values for the various feeds and speeds are automatically entered into the appropriate fields. Notice that the Spindle Speed has been calculated to be 194.0000 rpm, which you already set. OK to return to the PLANAR_MILL dialog.
Facing the Top of the Stock Setting the Display Options The display options can be set to make it easier for you to interpret the tool motion. The direction of the tool motion is more easily seen if directional arrows are painted on the tool path. Different types of tool motion can be painted in distinctive colors and the feed rates of the motion also displayed. Painting the tool in a 3D wireframe display makes it easier to visualize potential interference with clamps, and also provides a rough approximation of machining coverage. Choose Edit Display.
Set the Tool Display to 3-D. This will display the tool at every GOTO point and help you to visualize the tool motion. Another aid to visualizing the tool motion is to paint direction arrows on the tool path. Choose Other Options. Turn the Paint Arrows option on and OK. OK the Display Options dialog.
142 The default Part Stock is set to 1.0 mm. This value is automatically set by the selected Method, which is MILL_ROUGH. You will change the part stock value to bring the cutter into contact with the top of the part face selected as the floor. Choose Cutting. Change the Part Stock to 0.00 and OK to accept it.
Facing the Top of the Stock Generating the Tool Path All of the parameters have now been specified and you will generate the tool path. Generate the tool path. OK to continue generating the tool path.
OK to complete the operation.
Profiling Two Sides of the Stock You will profile the left side and front of the part geometry using the two white lines and fillet to define the tool path. This operation will machine reference surfaces for precise placement in the fixture.
143
Profiling Two Sides of the Stock Creating the Operation Choose the Create Operation icon in the toolbar. Be sure mill_planar is specified as the Type. Choose the PLANAR_MILL icon. Key in PROFILE-2SIDES in the Name field. Specify the following parent groups.
Choose OK to begin creating the operation.
Profiling Two Sides of the Stock Creating a New Tool You will create a 40.0 mm diameter tool. Because this tool is created within the operation, it does not display as an object in the Machine Tool view of the Operation Navigator. Choose the Groups tab.
144 Choose Reselect with the Tool option turned on.
Choose New. Choose the Mill icon, key in EM40 in the Name field, and OK to begin creating the tool.
Key in 40 in the Diameter field, 100 in the Length field and 8 in the Number of Flutes field. OK to finish creating the tool.
Profiling Two Sides of the Stock Setting Speeds and Feeds Choose the Main tab. Choose Feed Rates. Choose Reset from Table. The Spindle Speed has been calculated to be 484.0000 rpm for this tool. Remember this value. Change the First Cut feed rate to 98.00.
OK to accept the feeds and speeds.
Profiling Two Sides of the Stock Creating a Temporary Boundary
145 You will create a boundary that the operation will use to define the cut path. Unlike the part boundaries defined in the Workpiece parent group, this boundary can only be used by this operation. Choose the Part icon and Select.
Profiling Two Sides of the Stock Specifying Custom Boundary Member Data Custom Feed Rate and other commands can be added to individual members of a boundary. With the temporary boundary you are about to create, the tool motion through the fillet connecting the two lines will be made without the tool contacting any material. The move can be done at a feed rate greater than the cutting feed rate of 98.00 mmpm. Choose Custom Boundary Data. Set the Mode option to Curves/Edges.
Set the Type option to Open and the Tool Position option to on.
Choose MB3 and refresh the graphics window. Select the end of the white line as illustrated below.
146
Choose Custom Member Data.
Profiling Two Sides of the Stock Specifying Cut Feedrate The next piece of geometry you select will be given the custom data you specify. Turn the Cut Feedrate option on and key in 200 in the text field.
Select the fillet as illustrated below.
Key in 98 as the Cut Feedrate for the next boundary member.
147
Select the end of the white line.
OK twice to complete the boundary.
Profiling Two Sides of the Stock Displaying the Boundary You can display the temporary boundary you have just created. With the Part icon chosen, choose Display.
The temporary boundary displays in magenta. Notice that the tic marks are displayed on each side of the boundary, indicating that it is an On condition boundary.
148
Choose MB3 and Refresh the graphics window.
Profiling Two Sides of the Stock Setting the Floor Geometry Using an Arc The last operation you created used a face to define the floor geometry. You will use the arc filleting the two white lines this time to define the floor. Choose the Floor icon and Select.
Select the arc.
OK to define the floor.
149 The tip of the tool will position to this floor plane.
Profiling Two Sides of the Stock Using the Standard Drive Cutting Method The Standard Drive cut method is the only boundary cutting method which allows the tool to cross boundary members and cut them in the order in which they were selected. Choose Standard Drive as the cut method.
Profiling Two Sides of the Stock Setting the Cut Direction The Cut Direction is currently set to Climb. You will change it to Follow Boundary. Choose Cutting. Set the Cut Direction option to Follow Boundary and OK the Cut Parameters dialog.
150
Profiling Two Sides of the Stock Setting the Display Options You will set the display options to more easily visualize the tool motion. Choose Edit Display.
Set the Tool Display option to 3-D. Choose Other Options. Turn the Paint Arrows option on and OK. Turn off the Display Cut Regions and Pause After Display options. OK to complete the display options.
Profiling Two Sides of the Stock Generating the Tool Path All of the parameters have now been specified and you will generate the tool path. Generate the tool path. The tool path is generated and displayed without the pause that occurred when you generated the first operation. You might find turning off the pause very useful for multi-level operations.
151
Profiling Two Sides of the Stock Listing the Tool Path Choose the List icon to list the tool path.
Note the 200.0000 mmpm feed rate between the moves at 98.0000 mmpm for the circular move which you specified. The User Defined Events are displayed as Standard APT commands.
Dismiss the Information window. OK to complete the operation.
152
Visualizing the Tool Paths You will use Toolpath Visualization to see the material removal. Choose the ROUGHING_PROG object in the Program Order view of the Operation Navigator.
Choose the Verify Toolpath icon. Choose the Dynamic tab at the top of the dialog. Drag the slider bar to the left to slow down the Animation Speed to 4. Choose the Play Forward icon. The operations execute in the order of the program and material on the top and along the edge of the part is removed.
OK to complete the Toolpath Visualization. Close the part file.
153
Planar Milling - Single Level Planar Milling operations create tool paths that remove material in planar layers. This type of operation is most commonly used to rough out material in preparation for finishing operations. Planar Milling is intended for parts with vertical walls and planar islands and floors normal to the tool axis.
In this lesson, you will learn how to create single-level Planar Milling tool paths.
Creating a Planar Mill Operation You will create single-level Planar Milling operation.
Creating a Planar Mill Operation Opening the Part Open part file pln_pms_1.prt from the pln subdirectory.
154
This is a simple part, designed to illustrate the basic procedures involved in removing material from a pocket containing an island. Choose Application
Manufacturing.
Creating a Planar Mill Operation Creating the Operation Choose the Create Operation icon
in the toolbar.
Be sure mill_planar is specified as the Type. As a general practice, Program, Geometry, Tool, and Method parent groups should be specified in this dialog box. These parent groups, however, may be respecified within the operation. For this exercise, you will initially specify only the Tool parent group and the operation name. Choose the PLANAR_MILL icon.
Key in PLNR_M_PKT_1 in the Name field. Specify the following parent groups.
155
OK to begin creating the operation.
Creating a Planar Mill Operation Displaying the Tool Choose the Groups tab. With the Tool option on, choose Display.
The tool displays with its axis aligned to the ZC axis.
Creating a Planar Mill Operation Specifying Boundaries Planar Mill operations use boundaries to define the part, blank, check, and trim geometry. The volumes defined by these boundaries result from their projection to the floor plane. The blank geometry volume minus the part geometry volume defines the material to be removed (cut volume).
156 Choose the Main tab. Choose the Part icon and Select.
Be sure the Mode option is set to Face. You must define the side of the boundary you are going to cut. Since you are going to use this boundary to cut a pocket, you will retain the material on the Outside of the boundary. Set the Material Side option to Outside. When the Ignore Islands option is turned on, the system will ignore any islands that rest on the face that you select. In this case, if Ignore Islands were turned on, the island in the middle of the part would be cut off. Choose Ignore Islands to turn the option off. Select the face at the bottom of the pocket.
Both the pocket and island boundaries are created.
157 OK to complete the part boundary creation.
Creating a Planar Mill Operation Specifying the Floor Plane The floor plane is the lowest or last cut level. All cut levels are generated parallel to the floor plane. Choose the Floor icon and Select.
Select the face at the bottom of the pocket.
A vector displays originating from the selected face. OK the Plane Constructor dialog.
Creating a Planar Mill Operation Changing the Tool Path Display Colors Before you generate the tool path for this operation, look at the current settings of the tool path display colors. Choose the Edit Display icon. Choose Specify Colors. The Path Display Colors dialog shows the colors that each type of tool motion will display in.
158
Creating a Planar Mill Operation Changing the Step Over Color Since the part is green, you do not want the step over moves to also be green. Choose the Step Over color.
Set the color to Pink or a similar color.
Creating a Planar Mill Operation Changing the First Cut Color Notice that the First Cut and Cut moves are both cyan. You will change the First Cut color so that you can distinguish these moves. Choose the First Cut color. Set the color to White. OK to return to the Display Options dialog. OK to return to the PLANAR_MILL dialog. Creating a Planar Mill Operation Changing the Retract Feed Rate Choose Feed Rates.
Key in 99 in the Retract field.
159
OK to accept the feed rate.
Creating a Planar Mill Operation Generating the Tool Path Generate the tool path. The cut regions display.
OK to continue processing the tool path.
OK to complete the operation. Refresh the graphics display.
Creating a Planar Mill Operation Creating a Profiling Operation Profiling creates a single or specified number of cutting passes to finish part walls. Choose the Create Operation icon in the toolbar.
160 Be sure mill_planar is specified as the Type. Choose the PLANAR_PROFILE icon. Key in PLNR_M_PKT_2 in the Name field. Specify the following parent groups.
OK to begin creating the operation.
Creating a Planar Mill Operation Specifying Boundaries Choose the Part icon and Select. Set the Material Side option to Outside. Choose Ignore Islands to turn the option off. Select the face at the bottom of the pocket.
Both the pocket and island boundaries are created.
OK to complete the part boundary creation.
161
Creating a Planar Mill Operation Specifying the Floor Plane Choose the Floor icon and Select. Select the face at the bottom of the pocket.
A vector displays originating from the selected face. OK the Plane Constructor dialog.
Creating a Planar Mill Operation Generating the Tool Path Choose Edit Display. Set the Tool Display option to 2-D and OK to accept it. Generate the new tool path. OK twice to continue processing the tool path.
162
Creating a Planar Mill Operation Outputting Contact Data You will edit the operation and change the tool path output so that it is defined by cutter contact positions. Output Contact Data causes the tool path to be generated from cutter contact positions along the boundaries and walls of the part rather than from cutter end point positions.
Output Contact Data complements the traditional application of cutter compensation, which is to compensate for the wear of the cutter. By using the contact data, the machine operator has the flexibility of choosing a range of cutter sizes (based on the nominal cutter size specified in the operation) with which to machine the part while maintaining the same cutting accuracy along the tool path. This feature is only available for Planar Profile operations. Choose Machine. Choose Cutter Compensation. Set the Cutcom option to Engage/Retract. Turn the Output Contact Data option on.
OK twice to accept Output Contact Data and return you to the Planar Profile dialog.
Creating a Planar Mill Operation Generating the Tool Path Generate the new tool path. OK twice to continue processing the tool path.
163
OK to complete the operation.
Creating a Planar Mill Operation Specifying a Zig-Zag Cut Method Zig-Zag machines a closed pocket in a series of parallel straight line passes. Climb or conventional cut directions are not maintained because the cut direction changes from one pass to the next. Double-click the PLNR_M_PKT_1 icon to edit the operation.
Set the Cut Method to Zig-Zag.
Creating a Planar Mill Operation Generating the Tool Path You will generate the tool path and see the difference in cut motion due to the change in the cut type. Choose Edit Display. Set the Tool Display option to off and OK to accept it. Generate the new tool path.
164 OK to continue processing the tool path.
This time the tool does not follow the boundary. Instead, it makes parallel cuts back and forth with a stepover between cuts. Change to a Front view. You can see that the rapid moves (dashed red) cut into the island. There are options that you can set to avoid collisions like this, but for now you will only look at the cut types methods.
Reject
the tool path.
Creating a Planar Mill Operation Specifying a Follow Part Cut Method Set the Cut Method back to Follow Part.
Follow Part creates a tool path using concentric offsets from the part geometry. This method computes the tool path by offsetting from the outer edges of the pocket and the island. Climb (or Conventional) cutting is maintained throughout the tool path.
Creating a Planar Mill Operation
165
Generating the Tool Path You will generate the tool path and see the difference in cut motion due to the change in the cut type. Generate the tool path. OK to continue processing the tool path.
The tool path is generated. The tool does not collide with the island. This cut type is better suited for this part because the island's edges are taken into account when calculating the tool path. Reject the tool path.
Creating a Planar Mill Operation Changing the Stepover Moves The stepover establishes how the cutter moves from one cut pass to the next.
The stepover distance can be constant or variable. You have four options for controlling it. Constant - A fixed distance between passes. Scallop - The stepover is calculated based on the height of the scallops left between passes.
166 Tool Diameter - The stepover is determined based on the percentage of the effective tool diameter. Variable - Uses a variable stepover and number of passes or a minimum and maximum. Currently, the stepover distance is being controlled using a percent of the tool diameter. It is actually calculated using the effective tool diameter, which is the flat bottom of the tool.
The default percent value is 50.
Creating a Planar Mill Operation Changing the Diameter Percent You will see what happens to the tool path when the stepover is increased. Key in 70 in the Percent field.
Generate the tool path. OK to continue processing the tool path.
The increased stepover causes the cutting moves to be calculated differently. Compare your current tool path with what the tool path looked like with a 50% stepover. Reject the tool path.
167
Creating a Planar Mill Operation Changing the Scallop Height You will change the stepover so that the distance between cuts is controlled by the scallop height. Set the Stepover option to Scallop. The Percent option changes to Height.
The Scallop size is the height of material left by the corner radius of the tool. The stepover taken may vary from cut to cut depending on the boundary. 1. Scallop Size 2. Calculated Stepover 3. Cutter Corner Radius
Generate the tool path.
The tool makes fewer passes to cut the material while maintaining the scallop height.
168 Reject the tool path. Try some different combinations of Cut Method and Stepover. After you generate each tool path Reject it. (Do not change any defaults. Just compare the differences you get). After your last combination, refresh the graphics screen and continue with the lesson.
Creating a Planar Mill Operation Completing the Operation Set the Stepover option to Tool Diameter. Set the Percent value to 80. Generate the tool path. OK the PLANAR_MILL dialog to complete the operation. Notice that PLNR_M_PKT_1 is listed in the Operation Navigator. The exclamation point ( ) next to it indicates that the operation contains an internal tool path.
Close the part file.
Editing a Planar Mill Operation You will explore many of the Planar Mill parameters by editing an existing operation. Among these will be engages and retracts, transfer moves, clearance planes, avoidance geometry, floor planes, stock, feed rates, and trim boundaries.
169
Editing a Planar Mill Operation Opening the Part Open part file pln_pms_2.prt from the pln subdirectory.
Choose Application
Manufacturing from the menu bar.
Editing a Planar Mill Operation Editing an Existing Operation Choose PLNR_M_PKT_1 in the Program Order View and choose MB3
Edit.
Editing a Planar Mill Operation Defining Engage and Retract Moves Engage and Retract options determine the direction and distance that the tool moves toward or away from the part. In the Engage/Retract section, choose Method.
170
The Engage/Retract Dialog
There are two types of Engages and Retracts. Initial Engage is the first engage of the operation. Internal Engage is an engage move to a new cut region.
Final Retract is the last retract move of the operation. Internal Retract is a retract move prior to moving to a new cut region.
The clearance distances are the distances the tool stays away from the machining geometry when it moves to a cutting region.
In the following illustration, the tool begins the engage .100 away from the bottom of the part. This distance is called the Vertical Clearance distance.
171
The last option that you will look at is the Transfer Method. This option defines where the tool will retract to when moving from one cut level or one region to another. The tool path that you have just generated does not make any transfer moves. You will see this later in the Planar Milling Multi-Region lesson.
All of the moves are set to automatic, meaning that they are calculated for you. The engage and retract moves are based on the cutting condition of the operation, the geometry of the part, and different parameters that you enter. Cancel to return to the PLANAR_MILL dialog.
Editing a Planar Mill Operation The Ramp Options When the tool initially engages the part, it ramps at the angle set in Ramp Angle from the Vertical Clearance distance to the workpiece. Choose Automatic.
It is difficult to see the engage move in your tool path because the cutting tool moves are covering up the ramp engage.
172
Later you will learn how to apply a Helical Engage for the Initial Engage. Cancel to return to the PLANAR_MILL dialog.
Editing a Planar Mill Operation Circular Engage and Retract Some of the engages and retracts in the tool paths that you generated earlier are circular. Look at the circular engage applied when the tool engages the island boundary. Notice again, the circular engage used when the tool engages the wall of the part.
You also have circular retracts applied when the tool leaves the part wall and on the Final Retract. Circular Engage and Retract does not apply to Zig-Zag or any other Zig routine.
Editing a Planar Mill Operation Creating Linear Engage and Retracts Choose Automatic. Set the Automatic Type option to Linear.
173
OK to return to the PLANAR_MILL dialog.
Editing a Planar Mill Operation Generating the Tool Path Generate the tool path. The tool path generates and the circular engages and retracts convert to linear moves.
Choose Reject.
Editing a Planar Mill Operation The Overlap Distance Choose Automatic. Take a closer look at the retract move along the wall of the part
The tool cuts past the start point of the cut before it retracts. This is because of the Overlap Distance.
174 This move assures a full cleanup at the point where the engage and retract occur. The Overlap distance is also applied to engage moves.
Editing a Planar Mill Operation The Retract Clearance Look at the final retract. The tool moves .150 past the final cut point, then ramps up from the bottom of the part, to the .05 Retract Clearance.
This time you will change the overlap distance and the Retract Clearance and look at the difference. Refresh the graphics display. Key in 0.000 in the Overlap Distance field. Key in .300 in the Retract Clearance field.
OK to accept the changes.
Editing a Planar Mill Operation Generating the Tool Path Generate the tool path. The tool path is generated. The tool does not overlap at any point in the tool path. The tool retracts lifting .300 from the bottom of the part.
175 Choose Reject.
Editing a Planar Mill Operation Setting the Arc Radius Value for Circular Moves Choose Automatic. Set the Automatic Type to Circular. The Arc Radius field is no longer grayed out. You will define a larger arc the tool will track when making the internal engage and the final retract moves. Key in .500 in the Arc Radius field.
OK to accept the change.
Editing a Planar Mill Operation Generating the Tool Path Generate the tool path. Your tool path shows the enlarged circular engage (orange) and retract (cyan) move.
Choose Reject. Next you will create a helical engage for your initial engage move into the part.
176
Editing a Planar Mill Operation Creating Helical Engages In all of the previous tool paths, the tool ramped into the part on the initial engage. This is because a circular engage is only applied when engaging into a wall. You can use a Helical engage with the Follow Part cut method to avoid ramping into the part. Choose Method. Choose Automatic Engage/Retract. A helical engage move will be applied to the Initial Engage move of a Follow Pocket tool path. Set the Ramp Type to Helical.
OK to return to the Engage/Retract dialog. You will change the Vertical Clearance Distance setting to engage further away from the floor plane. This will enable you to see the helical move more clearly. Choose Method. Key in .300 in the Vertical field.
OK to return to the PLANAR_MILL dialog.
Editing a Planar Mill Operation Generating the Tool Path Generate the tool path. Your tool path is generated with a helical engage.
177
OK to complete the operation.
Editing a Planar Mill Operation Setting the Avoidance Geometry Avoidance geometry controls the non-cutting motions of the tool. These non-cutting motions are made to avoid clamps, set a safe approach to the part stock, or for other reasons detailed in the technical documentation. You are going to define a Clearance Plane, a From Point, and a Start Point. Double-click on PLNR_M_PKT_2.
The Avoidance option lets you define clearance motions for the tool as it moves toward or away from the part. This is different from the Engage and Retracts in that the tool moves toward or away from points in the tool path. Choose Avoidance. Avoidance Options
The options are described below: From Point - The FROM Point is a reference point only. The FROM/ command is output as the first entry in the tool path. Start Point - The Start Point outputs a GOTO/ command at the rapid feed rate after the FROM/ and post commands and before the first Engage move. Return Point - After the cutter reaches the last point of the cutter path, or the end of a Retract move if one has been defined, the cutter moves straight up to the Clearance Plane, then moves to the Return Point.
178 GOHOME Point - The GOHOME Point defines the final tool location. The From Point is often used as the GOHOME point. This point is a physical location that the tool moves to. GOHOME Point outputs a GOHOME/ command as the final entry in the tool path. Clearance Plane - The Clearance Plane defines a safe plane for the tool to move before and after an operation and when moving from one cutting region to another. Lower Limit Plane - The Lower Limit Plane is a plane which, when violated by the tool, issues a warning in the CLSF. You can specify what to do with points that occur below the lower limit plane. Redisplay Avoidance Geometry - Displays the active Avoidance Geometry (points and plane symbols) and the Reference Coordinate System (RCS).
Editing a Planar Mill Operation Defining the Clearance Plane The tool can move to the Clearance Plane before the Engage move, after the Retract move, and when moving between cut regions (Transfer moves). You will specify a Clearance Plane. Choose Clearance Plane - None.
The Clearance Plane dialog displays. You can use the Specify option to define the Clearance Plane. Then you can use the other options to temporarily omit and then reinstate the Clearance Plane, to verify the settings you have specified, and to graphically display the Clearance Plane. Choose Specify. Choose Plane Subfunction. Choose Principal Plane. Choose ZC Constant. You will create a clearance plane one inch above the XC-YC plane. Key in 1.0000 in the ZC field.
179 OK to accept the value. Notice that the ZC value for the Clearance Plane displays in the dialog and a plane symbol displays in the graphics window at ZC=1.0000.
Editing a Planar Mill Operation Defining when the Clearance Plane will be used Notice the Use at - Start_End option. You can use the Clearance Plane at the beginning of the tool path, at the end, or both. Choose Use at - Start_End.
The options for the use of the Clearance Plane are displayed. These settings will cause retract to the Clearance Plane when the tool moves from one cutting region to another. As you saw in the previous tool paths, this is necessary to prevent the tool from crashing into the island. OK to accept the default of Start and End. OK again. OK to return to the PLANAR_MILL dialog.
Editing a Planar Mill Operation Generating the Tool Path Generate the tool path. As you can see in the Front and Right views, the tool moves from the Clearance Plane to the engage point (red dashed line). Then at the end of the tool path, the tool moves from the last cut point back to the Clearance Plane (blue dashed line).
180
Reject the tool path.
Editing a Planar Mill Operation Defining a From Point The FROM Point is only a Reference Point. It does not cause any tool motion. It is used to establish the directional relationship between the tool and the part and as the origin of graphical display of the tool path. Choose Avoidance in the Machining Parameters section. Choose From Point- None from the dialog.
Choose Specify. Key in the following values for the Base Point and OK to accept them.
The FROM Point displays in the graphic window. You may have to rotate the view to see the displayed point.
181 OK to accept the From Point. The From Point is defined. Next, you will define the Start Point.
Editing a Planar Mill Operation Defining a Start Point The Start Point should be located below the Clearance Plane because the tool moves first to the Clearance Plane and then to the Start Point. Choose Start Point- None.
Choose Specify. The Point Constructor dialog displays. You are going to use XC, YC, ZC coordinates again. Key in the following values for the Base Point and OK to accept them.
The START Point displays in the graphic window.
Choose OK to accept the Start Point. Both the From Point and the Start Point are active.
182
OK to return to the PLANAR_MILL dialog.
Editing a Planar Mill Operation Generating the Tool Path You are ready to generate the tool path using the From and Start points. Generate the tool path. The tool path is generated. The tool moves from the From Point to the Clearance Plane. It then moves to the Start Point. Once it reaches the Start Point, it moves to the Engage Point.
OK to complete the operation.
Editing a Planar Mill Operation Editing the Boundary and Boundary Members You can make changes to an entire boundary or to individual boundary members. In this section, you will move the boundary plane. The tool in the previously generated tool path moved to the Clearance Plane, then to the Start Point, and then to the Engage point .300 above the floor. Then the tool moved to the boundary plane, which was the plane of the face you selected at the bottom of the part. This is OK for finishing because the roughing stock has already been removed. For roughing operations you must start cutting from the top of the stock material. To do this, you must move the boundary Plane to the top plane of the stock material. Double-click on the BOUND_EDIT operation. The PLANAR_MILL dialog displays. The operation is the same as the PLM_M_PKT_2 operation. It includes the Avoidance geometry and Feed Rates changes you made previously.
183 You are going to move the outermost boundary to the top of the part and the island boundary to the top of the island. Choose Edit in the Geometry section.
Notice that the outermost boundary highlights for editing.
Editing a Planar Mill Operation Editing the Plane of the Outermost Boundary The Plane option determines the plane in which the boundaries are created. You will move the outermost boundary from the bottom of the part to the top of the part. Set the Plane option to User Defined.
Choose Two Lines. Choose any linear edge at the top of the part
184
Choose a second linear edge at the top of the part.
You have defined the new boundary plane for the outermost boundary.
Editing a Planar Mill Operation Editing the Plane for the Island You will edit the boundary plane for the island. Choose the Next arrow key at the bottom of the dialog one time.
The island boundary highlights in white. Also notice that the outermost boundary now displays at the top of the part.
185
Once again, set the Plane option to User Defined. Choose Plane of Curve. Choose any arc edge on the top of the island.
OK the Edit Boundary dialog.
Editing a Planar Mill Operation Displaying the Boundaries You can display the boundaries to verify that changes are correct. Choose Display from the Geometry section.
The boundaries display.
186
Editing a Planar Mill Operation Generating the Tool Path Generate the tool path.
This time the tool moves to the Clearance Plane (ZC 1.0), down to the Start Point (ZC .4) then to the Engage Point. Remember, you set the Vertical Clearance in a previous operation to .300 above the Engage Start Point. The tool is moving at the Engage Feed Rate the Vertical Clearance distance into the material. It is also using the Helical engage motion. Choose Reject. Refresh the graphics window.
Editing a Planar Mill Operation Editing Members of a Boundary You can edit individual members of a boundary. This time you are going to slow down the feed rate as the tool cuts part of the island. Choose Edit in the Geometry section. Choose Previous or Next icon at the bottom of the dialog until the island boundary highlights.
187
Editing a Planar Mill Operation Editing the First Member Choose Edit.
Choose the Previous or Next icon to highlight the member illustrated below.
You will slow down the feed rate inside the "U" shape. Choose Custom Member Data. The Edit Member dialog expands to display the custom values which can be applied to a boundary member. You can customize each object in the boundary in many ways. You can add Post Commands, add Stock, or even change the selected geometry to be the first member of the boundary. Turn the Cut Feedrate option on and key in 6.00 into the value field.
188
Editing a Planar Mill Operation Editing the Next Member Choose the Previous icon to highlight the previous boundary member.
Turn the Cut Feedrate option on and key in 5.00 into the value field.
Editing a Planar Mill Operation Editing the Remaining Members Choose the Previous icon to highlight the previous boundary member.
Turn the Cut Feedrate option on and key in 5.00 into the value field. Choose the Previous icon to highlight the previous boundary member.
Turn the Cut Feedrate option on and key in 5.00 into the value field. Choose the Previous icon to highlight the previous boundary member.
189
Turn the Cut Feedrate option on and key in 6.00 into the value field. OK the Edit Member dialog. OK to return to the PLANAR_MILL dialog.
Editing a Planar Mill Operation Generating the Tool Path Generate the tool path. List the tool path FEDRAT/5.000.
and scan for the custom feedrates FEDRAT/6.000 and
Dismiss the Information window. Reject the tool path. Now you are going to look at a few more Display options that can be used to help display the tool path.
Editing a Planar Mill Operation More About Display Options In this section, you will change some more of the Display options. Choose Edit Display.
190 In the Display Options dialog, notice that the paint speed is still set to 8, as you set it earlier in the lesson. Set the Tool Display option to 3-D. Key in 5 in the Frequency field. This specifies that the tool will be displayed at every fifth Cutter Location point. Choose Other Options. Paint Feeds - Displays the feed rate each time it changes. Paint Arrows - Displays an arrow at the end of each tool path segment showing its direction. Paint Line Numbers - Displays the CLSF line number of the first CL-point of each tool path when you Replay an accepted tool path. Turn the Paint Feeds and Paint Arrows options on.
OK twice to return to the PLANAR_MILL dialog.
Editing a Planar Mill Operation Generating the Tool Path Generate the tool path. You can see the effect of all the changes you made to the display options.
The tool displays as a wireframe at every fifth point in the tool path There is an arrow at the end of each tool path segment Feed rate changes are shown as "F#"
191 Because the Display settings are modal, they remain in effect until they are changed. OK to accept the tool path. You are finished using this part file. Next you are going to learn more about blank geometry and boundaries. Close the part file.
Editing a Planar Mill Operation Defining Blank Geometry Blank geometry is the material that surrounds some or all of the part. The cut volume (material to be removed) is the blank material minus the part material. In this portion of the lesson, you will define blank geometry and then remove the portion that surrounds the perimeter of the part. Open part file pln_pms_3.prt from the pln subdirectory.
Choose Application
Manufacturing.
Editing a Planar Mill Operation Creating an Operation You are going to create a Planar Mill operation that removes the blank geometry around the perimeter of the part.
Choose the Create Operation icon
in the toolbar.
Be sure mill_planar is specified as the Type. Choose the PLANAR_MILL icon.
192
Specify the following parent groups.
OK to begin creating the operation.
Editing a Planar Mill Operation Defining the Part Boundary With the Part icon chosen, choose Select.
The Boundary Geometry dialog displays. The Material Side is set to Inside. This means that the material will be retained inside the boundary. Set the Mode option to Curves/Edges. Select the four curves in order as illustrated below.
193
OK to create the boundary.
OK to return to the PLANAR_MILL dialog.
Editing a Planar Mill Operation Using Side Stock for Blank Geometry You will create Blank geometry using the Side Stock option. This creates a specified amount of stock equally surrounding the sides of the part. Choose the Blank icon, then Select.
Turn the Ignore Holes option on. Choose Custom Boundary Data. Turn the Stock option on and key in1.00.
194
This creates an extra inch of stock surrounding the part that will be used as the Blank boundary. The tool will cut from the 1 inch outer edge of the Blank boundary to the Part boundary. Be sure the Mode is set to Face. Select the bottom face of the part.
OK to complete the boundary geometry.
Editing a Planar Mill Operation Defining the Floor You are going to use the bottom face of the part as the Floor. Choose the Floor icon and Select.
195
Select the bottom face of the part.
OK to accept the face and return to the PLANAR_MILL dialog. A plane symbol and vector display, indicating the face selected and the normal vector direction away from its interior.
Editing a Planar Mill Operation Generating the Tool Path Generate the tool path.
OK to complete the operation. Close the part.
196
Planar Milling - Multi-Level A multi-level tool path cuts material in successively deeper levels. The tool begins at the top level and works its way down to the floor plane.
In this lesson, you will learn how to create multi-level tool paths, clean up islands, create and edit boundaries, and control many other aspects of multi-level planar mill operations.
Creating a Multi-Level Planar Mill Operation You will create multi-level Planar Milling operation.
Creating a Multi-Level Planar Mill Operation Opening the Part Open part file pln_pmm_1.prt from the pln subdirectory.
197
Choose Application
Manufacturing.
Before you start, there are two terms that you should understand. Region - this is the area within the cut levels that can be accessed by the tool without it having to retract from within the part. There can be multiple regions cut in one operation. Cut Level Planes - are planes that define the levels in the pocket where the cuts take place.
Blank and Part Geometry Definition Blank and part geometry have already been defined in the Workpiece object. You will examine the blank and part geometry in the Workpiece object and then define part boundaries and the floor plane.
198
Blank and Part Geometry Definition Examining the Workpiece Parent Group Set the Operation Navigator to the Geometry View. Expand the MILL_ORIENT and WORKPIECE objects. Highlight WORKPIECE.
Choose MB3
Edit.
With the Part option chosen, choose Display.
Refresh the graphics display. Choose the Blank icon and then Display.
OK the WORKPIECE dialog. Set the Operation Navigator to the Program Order view.
199
Blank and Part Geometry Definition Editing the Operation You are going to edit an existing operation. Double-click on the operation named PMMULTI.
Blank and Part Geometry Definition Defining the Boundaries You will create three part boundaries using the Curve/Edge mode - first the main boundary, then two island boundaries. With the Part icon chosen, choose the Select option.
Set the Mode option to Curves/Edges.
You are cutting a pocket, so the material to remain is on the outside of the pocket boundary. The Material Side option needs to be changed to Outside. Set the Material Side option to Outside.
You are ready to select the objects for the first boundary.
200
Blank and Part Geometry Definition Creating the Main Boundary You can select the boundary objects individually or by chaining. Choose Chaining. You will select the first segment of the boundary at the end that indicates the chain direction. Select the linear edge at the left end as illustrated below.
Select the arc edge as shown.
All the elements are chained and highlighted.
The system will automatically bridge the gap to create a closed boundary.
201
Blank and Part Geometry Definition Creating the Next Boundary The Create Next Boundary option lets you finish creating the current boundary and then start another without leaving this dialog. Choose Create Next Boundary.
Because the Type was set to Closed, the boundary was automatically closed by extending the first element to meet the last.
Blank and Part Geometry Definition The Boundary Plane The boundary is created in the boundary plane. The boundary plane does not necessarily have to be in the same place as the objects that you select. There are two boundary plane choices: Automatic - The plane is determined by the first element selected (if it is an arc) or the first two elements (if the first is not an arc). This is the default. User-Defined - You define the plane using the Plane Subfunction. Leave the Plane option set to Automatic.
202
Blank and Part Geometry Definition Creating an Island Boundary You are ready to create an island boundary. This island is the mid-level face containing the two counter bored holes. It is red in the illustration below.
You are cutting the top of an island, so the Material Side is on the inside of the boundary this time. The material will be retained on the inside of the boundary, preventing the island from being cut away. Set the Material Side option to Inside.
The tool will not remove material from inside the boundary. The plane of island boundaries should be located at the top of the island, so you can let the system use the edges you select to automatically define the plane for this boundary.
Blank and Part Geometry Definition Chaining the Elements Choose Chaining.
203 When you are chaining, the crosshair placement determines the success of the chaining operation.The selection ball must capture the edge that you are selecting and The crosshair must pierce the island face that contains the edges you wish to chain.
Select the first linear edge toward the right end as shown.
OK to create the chain. All the objects around the top of the island are selected. The system used the plane defined by the two end points of the object selected to determine the boundary plane. It then chained the contiguous objects in that plane to form the boundary.
Make sure your Cue line says "Select object #9". This means you have successfully selected 8 objects.
Blank and Part Geometry Definition Creating the Third Boundary Again, you are defining an island and will create this boundary by chaining the edges on the top face of the object. (You could use the face selection method, but for instructional purposes
204 use the chaining method.) Material Side should be set to Inside. The material will be retained on the inside of the boundary, preventing the island from being cut away. Choose Create Next Boundary. Choose Chaining. Select the linear edge toward its lower end, as shown below.
Select the arc edge as the end of the chain.
After you accept the selection, all the elements on the top of the island are selected highlighted. OK to create the boundary.
OK to return to the PLANAR_MILL dialog.
Blank and Part Geometry Definition Establishing the Floor Plane
205 The floor plane is the lowest plane in your pocket. The cut levels of the tool path will be parallel to this plane. The default of the XC-YC plane is currently set. With the Floor icon selected, choose Select.
Select the face on the bottom of the pocket.
OK to return to the PLANAR_MILL dialog.
Blank and Part Geometry Definition Generating the Tool Path Generate the tool path. OK to continue processing the tool path. The tool path is generated at one level (the floor plane). You need to set cut levels to create a multi-level operation. Also, you can see that the engage move does not look right. This will be corrected later.
206
Reject the tool path. Refresh the graphics area.
Defining Cut Levels In order to create a multi-level tool path, you must define cut levels. You will add stock, define the cut depth and define engages and retracts.
Defining Cut Levels Defining the Cut Depth Choose Cut Depths.
You are going to define the cut depths by defining the maximum and minimum depths. First you will define the largest amount of material to be cut at any level. If you use the default of 0, you would generate a single level tool path at the floor plane.
207 Key in 1.30 in the Maximum field.
Now you will set the Minimum cut depth to 0.100. This is the smallest amount of material that you can cut at any level. Key in 0.10 in the Minimum Field.
If you accept the Minimum default value of 0, and specify a larger Maximum value, the tool will cut at the Maximum value depth and,at the top of each island.
Cut Levels
There are five types of cut levels.
User Defined - You define the depths of cut. You can set the Maximum, Minimum, Initial, and Last depths of cut Floor Only - Generates a single cut level at the floor plane. Floor & Island Tops - Generates one cut level at the floor plane and then generates a cleanup cut at the top of each island. Levels at Island Tops - Generates a cut level at the top of each island. Fixed Depth - Generates cut levels at a constant depth, using the Maximum field. Initial - Defines the depth of cut for the first cut level of the tool path.
208 Final - Defines the depth of cut for the last cut level of the tool path. Increment Side Stock - Adds side stock to each cut level. Cut level one will leave the specified stock. Cut level two will leave twice the specified stock, and so on. Top Off Islands - Causes the tool to cut the tops of the islands if they could not be cut at one of the cut levels. Notice that this option is on by default. When there are islands in the part file and the maximum and minimum depths of cut are defined, the system will try to use the tops of the islands as one of the cut depths. This is subject to the number of islands defined and the specified maximum and minimum cut depths.
OK to accept the Cut Depth and return to the PLANAR_MILL dialog.
Defining Cut Levels Adding Stock You can add stock to the floor and/or walls of your part. Choose Cutting.
Key in 0.03 for the Part Stock field.
OK to return to the PLANAR_MILL dialog.
Defining Cut Levels Stock Options The Stock values are near the bottom of the Cut Parameters dialog.
209
Part Stock - This is the remaining material on the walls at the completion of the tool path. Final Floor Stock - This is the amount of material that is left on the floor and on top of the islands at the completion of the tool path. Blank Stock - This is the distance the tool will be positioned from the defined blank geometry. Blank Distance - This is the offset distance applied to the part boundary or part geometry to produce the blank geometry. Check Stock - Is the distance the tool will be positioned from the check geometry. Trim Stock - Is the distance the tool will be positioned from the trim geometry.
Defining Cut Levels Defining a Clearance Plane You will define the Clearance Plane for this operation. Choose Avoidance.
Choose Clearance Plane - None. Choose Specify. Choose Plane Subfunction. Choose Principal Plane. Choose ZC Constant. Key in 0.10, then OK. The ZC value for the Clearance Plane displays on the dialog.
210
A plane symbol displays at the WCS ZC 0.0.
OK twice to return to the PLANAR_MILL dialog. Before you generate the tool path, be sure that all 4 views are displayed, since you want to be able to see the tool path from several directions.
Defining Cut Levels Generating the Tool Path Generate the tool path. Turn on the Refresh Before Display option. Notice that the cut region extends out to the entire pocket, including the island on the right end. You can see in the Front or Right view that the cut is above this island. OK to generate the first cut level. OK to display the second cut region. This time, you can see that the cut is right on top of the island on the right end. OK to generate the second cut level. Choose OK each time this dialog displays and generate the entire tool path. The final level cuts the bottom of the pocket and around the middle island. Each time the tool goes from one cut level to the next, it moves back up to the Clearance Plane, as shown below.
211
You will eliminate this unnecessarily large tool move by changing the Transfer Method.
Defining Cut Levels Calculating the Cut Levels Choose List.
The tool path displays in the Information window. Notice that the depth of the first cut is .900. You specified 1.3.
The distance from the top of the part to the top of the first island is 1.800. You also specified Top of Island as a cut level. Since this distance (from the top of the part to the top of the first island is greater than the 1.300 the maximum depth you specified, the actual distance of 1.800 is divided into two equal steps of .900. 1. First Cut Level 2. Second Cut Level (top of island) 3. Top of Part
212 Dismiss the Information window. Reject the tool path.
Defining Cut Levels Specifying the Transfer Method Transfer Method refers to the way the tool moves from one Cut Level to the next or from one region to another. These moves occur between the retract from one level or region and the engage move to the next. You will set the transfer method so that the tool does not move to the clearance plane with each internal engage/retract move or cut level. Choose Method in the Engage/Retract parameters section. In the Transfer Method section, choose Clearance Plane.
Transfer Methods
There are four methods available: Clearance Plane - This is the default. The tool moves to the clearance plane for the engage and retract moves. Previous Plane - Uses the current completed cut level (plus the vertical clearance distance) to position and engage to the next cut level or region. Blank Plane - Moves the tool to the blank plane (plus the vertical clearance distance) before moving to the next cut start point. Direct - Makes a straight line move from the current position to the start of the engage move, or to the cut point if no engage move is specified. The transfer method does not affect the initial tool engage or the final tool retract moves. Those moves are determined by your Engage/Retract settings.
Set the Transfer Method to Previous Plane.
213
The default Vertical and Horizontal Clearance Distances are .1. This means that the tool will retract .1 above the previous plane before engaging to the next cut and come no closer than .1 inch to any wall geometry. You will change these values to ensure that the tool will not gouge the top of the island. Key in .200 in the Horizontal value field. Key in .200 in the Vertical value field.
OK to accept the values.
Defining Cut Levels Changing the Feed Rates You are going to slow down the engage moves. Choose Feed Rates. Change the Engage feed rate to 5 ipm and the Cut feed rate to 8 ipm.
OK to accept the values.
Defining Cut Levels Generating the Tool Path Generate the tool path and OK the dialogs as needed to generate all the levels of the tool path.
214 Notice the dashed lines, indicating the move between levels at the previous plane plus the vertical distance of .2.
Reject the tool path.
Defining Cut Levels More Cutting Options In this section, you will change the Region Connection status and compare the differences in the final cut levels of the tool paths. Choose Cutting. Cut Order - determines the order in which multiple regions are cut. Direction - sets the cut direction so the cutting tool either climb cuts or conventional cuts. Set the Cut Direction option to Conventional Cut.
OK to accept the cut parameters.
Defining Cut Levels Generating the Tool Path Generate the tool path and OK as needed to generate all of the cut levels.
215
The tool cuts the part using the conventional cut direction. The resulting tool path is the same, but the tool path is developed differently. When the last level is cut the tool starts on the right side of the part rather than the left. The tool also cuts around the island in the opposite direction. Refresh the graphics display. Reject the tool path.
Defining Cut Levels Specifying a Helical Engage With the advent of high performance cutting tools, which eliminate the need to drill relief or start holes, tool engagement can be controlled using a helical engage to prevent cutting tool damage. Choose Automatic under Engage/Retract. Set the Ramp Type option to Helical.
Notice the Helical Diameter % defaults to 90.0. Key in 100 for the Helical Diameter %.
216
Helical Diameter %
The most effective way of engagement is through the milling of a "start" hole using helical interpolation. Associated with this method of ramping is the parameter Helical Diameter % which describes the maximum diameter path used by the tool for a Helical engage and is used for the Helical ramp type only. When using the helical method, there is a minimum and maximum hole diameter that can be utilized, leaving no center or cone material at the bottom of the hole. The maximum hole diameter is equal to:
The minimum hole diameter is equal to:
217 If the hole diameter is greater than the calculated maximum hole diameter, material remains in the center of the hole but has no effect on the tool since the material is on the outside of the cutter.
If the hole diameter is less than the calculated minimum hole diameter, material remains in the center of the hole, causing the tool to break.
If the hole diameter is equal to the calculated minimum hole diameter, no material remains in the hole and the cutting tool will cut normally.
218
If the hole diameter is equal to the calculated maximum hole diameter, the bottom of the hole is completely flat. This is the preferred method for helical interpolation.
If the area is not large enough to allow the Helical Diameter, the diameter of the path will be reduced and an attempt is made to perform the engage again. This process will continue until either the Helical Engage is successful or the path diameter becomes less than the Minimum Ramp Length. If the area is not large enough to allow the path diameter that is equal to the Minimum Ramp length, the system will attempt to ramp into the area.
OK to accept the Automatic Engage/Retract dialog.
219
Defining Cut Levels Generating the Tool Path Generate the tool path and OK as needed to generate all of the cut levels.
Reject the tool path.
Defining Cut Levels Specifying a Linear Ramp Engage In cases where helical interpolation is impractical (i.e. long narrow cut areas) ramping into the part may be more suitable. Choose Automatic under Engage/Retract. Set the Ramp Type option to On Lines.
Key in 80 in the Min Ramp Length-Dia % field. Minimum Ramp Length
When using an inserted cutting tool, the ramping motion must be long enough to eliminate any uncut material. Associated with the ramp method is the parameter Min Ramp LengthDia% - which is used by all three Ramp Types (On Lines, On Shape, Helical). For On Shape and On Lines, the Minimum Ramp Length-Dia% represents the minimum path distance used by the tool from the top to the bottom of the ramp. For Helical Ramp Type, the parameter represents the minimum diameter path used by the tool. The minimum ramp length can be calculated as follows: 2 x Tool diameter - 2 x Insert Width
220 If the ramp length is less than the calculated minimum, material remains which results in tool breakage.
If the ramp length is greater than or equal to the calculated minimum, no material remains and the tool will cut normally.
OK to accept the linear ramp engage. When ramping into a part, a check is made to verify that at least some portion of the region is long enough to allow ramping motion using the Minimum Ramp Length. If this is impossible, a warning message will be displayed.
221
Defining Cut Levels Generating the Tool Path Generate the tool path and OK as needed to generate all of the cut levels.
OK to complete the operation.
Defining Cut Levels Visualizing the Tool Path A shaded display of the material removal can help you to visualize the machining operation. MB3 Expand in the TFR-ISO view so that this is the only view that appears in the window. Highlight PMMULTI.
Choose MB3
Toolpath
Choose the Dynamic tab. Choose Play Forward.
Verify.
222 Cancel the tool path visualization. MB3
Expand so that all four views again appear in the window.
Uncut Region Boundaries Many times when developing a tool path you may have areas of uncut material. This may be caused by a number of different conditions such as a tool that is too big or stock left on the part walls or corners. There is an option available in Planar Milling that can automatically create boundaries for the uncut regions. You can then use these boundaries to create a tool path to clean up these areas. In the following portion of this lesson, you are going to create a profile tool path using a tool that will leave material in the corners while it removes the 0.030 part stock left by the previous operation. You will save the uncut regions as boundaries and use them in a second tool path to cleanup the corners.
Uncut Region Boundaries Creating Uncut Region Boundaries You are going to create a tool path using a 1 inch tool. This tool is intentionally larger than the corner radii in order to leave behind uncut material. You will save the uncut regions as boundaries. There are two different ways you can create and save boundaries for uncut regions: Under Edit Display, if the Process Display Parameters are set properly ( that is, with Pause After Display enabled), the Display Parameters dialog will give you the options
223 of displaying and saving the uncut regions. This interactive method allows you some control over the number and location of the boundaries which will be created. Under the Cutting section of the Planar Mill dialog, the Auto Save Boundary option can be selected. This method will automatically create boundaries at all the locations where uncut material is detected. Double-click on UCUT.
Uncut Region Boundaries Creating Boundaries for Uncut Regions by Setting Display Options It is important that the tool path display options are set correctly. The option that you use to save the Uncut Region Boundaries is located on the Display Options dialog. You want to make sure that it is displayed when you need it. Pause After Display must be turned On. Choose Edit Display.
Turn the following Process Display Parameters options on.
OK the settings.
Uncut Region Boundaries Generating the Tool Path You are going to generate the tool path. While the tool path is generating, you will also display the uncut regions. Generate the tool path.
224 The first cut level displays along with the Display Parameters dialog. The Overlap Distance is an offset to be applied to the boundary into the cut region to insure clean up. Four uncut regions are displayed in this cut level.
You can see the material left in the corners. You could select the Save option, but you will wait for the last cut level before saving. OK to continue processing the tool path. The Display Parameters dialog displays. Notice that you do not have the option of saving the uncut regions at this time. OK to continue processing the tool path. The second cut level displays along with the Display Parameters dialog. Once again, you have the option to Save the uncut regions but you will not. OK to continue processing the tool path. The Display Parameters dialog displays without the Save Uncut Region option. OK to continue processing the tool path. The third cut level displays along with the Display Parameters dialog.
225
There are more boundaries displayed this time. Continue to process this tool path. You will save on the next level. Choose OK to continue processing the tool path. OK to continue processing the tool path. The final cut level displays along with the Display Parameters dialog. Now there are additional Uncut Regions displayed at the U shape near the island.
Uncut Region Boundaries Saving the Uncut Regions as Boundaries You are going to Save the uncut regions as boundaries.
Choose Save from the Uncut Regions section.
226 At this point you will get an Uncut Boundary Output Warning message saying "Previously saved Uncut Boundaries will be replaced. Do you want to proceed?". This means that the boundaries you did not create at the higher levels in this operation will be overwritten by the boundaries you are about to create. This is just an informative message and will cause no problems.
OK the warning. The boundaries are created and displayed in green. As you have developed this operation, you may have noticed that some of the same boundaries are displayed at each level. Only one boundary is saved for each location thus eliminating boundary duplication.
OK to continue processing the tool path. The final cut level is developed and the PLANAR_MILL dialog displays. This is one method of creating the Uncut Regions as boundaries. You are going to Cancel this tool path. If you Cancel the operation, the boundaries will not be saved. Cancel this operation.
227
Uncut Region Boundaries Creating Boundaries for Uncut Regions Automatically You are going to edit the same operation, only this time you will use the Automatic method of saving the uncut regions. Double-click on UCUT.
Choose Cutting. The Cut Parameters dialog displays. Notice the Auto Save Boundary option in the Uncut Regions section at the bottom of the dialog. Choose the Auto Save Boundary option to turn it on. OK to return to the PLANAR_MILL dialog.
Uncut Region Boundaries Setting the Display Options Now you will edit the display options to eliminate the user interaction in creating the uncut region boundaries. Choose Edit Display at the bottom of the PLANAR_MILL dialog. Turn off Pause After Display. Turn on Refresh Before Display.
OK the settings.
Uncut Region Boundaries Changing the Cut Method to Profile The bulk of the interior material of the part was removed by operation PMMULTI. Part stock of 0.030 was left for removal.
228 You will set up the current operation so that it will remove the part stock. You only need to machine the walls of the part and its island. The profile cut method will eliminate the interior tool motion that was generated in PMMULTI. Set the Cut Method to Profile.
Uncut Region Boundaries Generating the Tool Path and Automatically Saving the Uncut Regions as Boundaries You are going to generate the tool path. While the tool path is generating, you will also be displaying and saving the uncut region as boundaries. Generate the tool path. The boundaries are created at each cut level as the tool path is generated.
OK to complete the operation.
Uncut Region Boundaries Creating an Operation Using the Uncut Region Boundaries Now you are going to create a tool path using the uncut region boundaries that were created from the previous operation. You are going to copy the previous operation and make your boundary and tool changes to the copy. Copying the operation rather than creating a new one saves time in that you do not have to redefine many of the options you had set (i.e., Boundaries, Avoidance Geometry, Floor Plane). If necessary, highlight the operation name UCUT.
229
Choose MB3
Copy, then MB3
Paste.
The copied operation displays in the Operation Navigator underneath operation UCUT with the name UCUT_COPY.
Uncut Region Boundaries Defining Blank Boundaries You are going to define the new uncut region boundaries as blank geometry. Remember, the system sees blank geometry as material that needs to be removed. Double-click on UNCUT_COPY. Choose the Blank icon, then Select from the Geometry section.
The Material Side is set to Inside. Set the Mode option to Boundary. Select all 8 of the uncut region boundaries in order as illustrated below.
230
OK to complete the blank geometry.
Uncut Region Boundaries Redefining the Tool You are going to use a smaller tool for this cleanup operation. Choose the Groups tab. Choose Reselect.
Choose EM-.375-.03 and OK to accept it.
Choose the Main tab. Choose Edit Display, turn on the Pause After Display option. OK to accept the display options.
231
Uncut Region Boundaries Generating the Tool Path Generate the tool path. The first cut level is displayed. The tool is only going to cut the blank boundary material and will avoid gouging any of the part geometry.
OK to continue processing the tool path. The tool cuts the first corner at the first cut level.
Turn Off the Pause After Display option. Choose OK to continue to process the tool path.
232
The tool cuts all of the boundaries at each level, then moves down to the next level to cut all of the boundaries at that level. This continues until all boundaries are cut to the floor plane. You could specify that the tool cut one boundary to the finish depth before moving to the next boundary. Reject the tool path.
Uncut Region Boundaries Changing the Cutting Order You can control the cutting order of the tool path to cut by Levels or by Depth. The previous tool path cut all of the boundaries by levels. When all of the cutting at one level was complete, then the tool moved down to the next level to start cutting. Cutting by Depth cuts one region or boundary to the finish depth before moving to the next region or boundary. Choose Cutting. Set the Cut Order option to Depth First.
OK the Cut Parameters dialog.
Uncut Region Boundaries Generating the Tool Path Generate the tool path. The first cut level displays. It looks the same as the previous tool path.
233
Turn Off the Pause After Display and Refresh Before Display options. OK to continue generating the tool path. The tool path is generated. This time the tool cuts each boundary to the finish depth before moving to the next boundary.
OK to complete the operation.
Uncut Region Boundaries Visualizing the Tool Path MB3 Expand in the TFR-ISO view so that this is the only view that appears in the window. Highlight NC_PROGRAM.
234
Choose the Verify Toolpath icon
in the toolbar.
Choose the Dynamic tab. Choose Play Forward. The colors displayed for dynamic material removal may differ from those illustrated and are determined under Preferences Manufacturing Visualize.
OK the Toolpath Visualization dialog. Close the part file.
Using Corner Control and Slowdown In this portion of the lesson, you will create a Profile tool path to machine a corner of the part. You will create and edit an open boundary, add an additional roughing pass, and use the Corner Control and Feed Rate options.
235
Using Corner Control and Slowdown Opening the Part Open part file pln_pmm_2.prt from the pln subdirectory. The part file is very similar to pln_pmm_1.prt. Choose Application
Manufacturing.
Using Corner Control and Slowdown Editing an Operation You are going to edit an existing operation. Set the Operation Navigator to Program Order View. Double-click on operation PMOPEN.
Using Corner Control and Slowdown Creating an Open Boundary With the Part icon selected, choose the Select option in the Geometry section.
Choose Curves/Edges as the Mode. Choose Open as the Type. Notice the Material Side option. It now reads Material Side Left. The option settings are Left and Right for open boundaries. The material side is determined relative to the direction in which the boundary members are selected. Choose the Material Side option and change it to Right. Choose the three edges in the order shown (you may want to zoom in on the area first).
236
OK to accept the edges.
OK to accept the boundary.
Using Corner Control and Slowdown Defining the Cut Method You will machine the corner with a Profile cut method. Choose Profile as the Cut Method.
Using Corner Control and Slowdown Editing the Boundary End Points If you created your tool path now, it would cut all the way from the beginning of the first edge in the boundary to the end of the last. But you really only need to cut a small amount from the corner. You can do this by editing the boundary members. Choose Edit in the Geometry section.
237
Choose Edit.
The Edit Member dialog displays. Notice that the first boundary member is highlighted.
Using Corner Control and Slowdown Moving the Start Point You are going to move the start point, which is on this boundary member at the circle which indicates the origin. Choose Start Point.
The Modify Boundary Start Point dialog displays and a directional arrow displays in the graphics window to indicate the boundary direction.
238
Key in 60 in the Percentage field and OK.
The start point is moved.
Using Corner Control and Slowdown Moving the End Point You will move the end point of the last segment so that the two linear boundary segments are about the same length. Choose the Next arrow
twice until the last boundary member is highlighted.
Choose End Point. Using the slider bar, move the end point towards 35%.
239 The shortened boundary displays. The white cone head indicates the boundary direction.
OK three times to return to the PLANAR_MILL dialog.
Using Corner Control and Slowdown Adding a Roughing Pass You will add a roughing pass to this operation .060 away from the part wall. Set the Stepover option to Constant.
Key in .06 in the Distance field and 1 in the Additional Passes field.
Using Corner Control and Slowdown Specifying the Floor Plane You will define the floor plane at the top of the island. Choose Floor and Reselect. A dialog warns you that the default floor geometry (the XC-YC plane) will be removed. OK the warning. Select the face on the top of the island.
240
The face highlights and a directional vector appears.
OK to return to the PLANAR_MILL dialog.
Using Corner Control and Slowdown Setting the Cut Level Since you only need to cut at the floor plane, you must eliminate the multi-level passes. Remember, Floor Only generates a single cut level at the floor plane. Choose Cut Depths. The Depth of Cut Parameters dialog displays. Set Type to Floor Only.
OK to return to the PLANAR_MILL dialog.
241
Using Corner Control and Slowdown Applying Slowdowns Choose Corner. The Corner and Feed Rate Control dialog displays. You can use these options to control the machining of inside and outside corners.You will slow down the feed rate as you enter corners and accelerate as you leave them. Turn on the Slowdowns option. The Length value determines how far ahead of the beginning of the corner radius you want the tool to slow down. The default of Percent Tool determines the length using a percentage of the current tool diameter. Make sure the Length setting is Percent Tool. The Length option toggles between Percent Tool and Previous Tool. The previous tool option allows you to set the slowdown to coincide with the end of material cutting for a previous, perhaps larger, tool. Key in 50 in the Percent Tool field. The Slowdown % value determines the slowest feed rate during slowdown, as a percentage of the present feed rate. Key in 4 in the Number of Steps field. The Number of Steps value affects the abruptness of the slowdown. The greater the number, the more even the slowdown. The feed rate reduction per step is: (100% - Slowdown %) / No. of Steps The number of acceleration steps is approximately one-half of the number of deceleration steps. This is a small corner - you really do not need four steps to slow the feed rate down but you can easily see the results in the tool path. OK to return to the PLANAR_MILL dialog.
Using Corner Control and Slowdown Setting the Engage and Retract Choose Automatic from the Engage/Retract section.
242 Notice that the Automatic Type is set to Circular and the activation range is set to .100. You will change the Activation Range to 0. Key in 0 in the Activation Range field. The tool path that you generate with this setting will use a circular engage on the final pass only. OK to return to the PLANAR_MILL dialog.
Using Corner Control and Slowdown Generating and Listing the Tool Path Generate the tool path. After the Cut Region displays, OK to generate the tool path.
Notice that the first pass is .060 away from the part wall. The tool makes a circular engage into the wall on the final pass, then moves to cut the radius and retracts in a circular fashion along the remaining wall. You can also see the feed rate changes as the tool machines the corner. There are several stacked up in the corner where the slowdown occurred.
Choose List at the bottom of the dialog. The slowdowns are listed in the tool path is listed in the listing window.
243 The feed rate changes as the tool slows down going into the corner and then accelerates as it moves away from it. The number of acceleration moves is approximately half of the decelerations. Dismiss the Information window. OK to complete the operation. Close the part file.
Cutting the Blank Geometry and Pocket in One Operation In this portion of the lesson, you are going to cut the blank material and the pocket of the part in one operation. You are going to define the blank material using the Blank Distance option. You used this option in the previous lesson. You are also going to define a different Cut Depth.
Cutting the Blank Geometry and Pocket in One Operation Opening the Part Open part file pln_pmm_3.prt from the pln subdirectory.
244
Choose Application
Manufacturing.
Cutting the Blank Geometry and Pocket in One Operation Editing an Operation You are going to define a total of 5 boundaries. Some of the boundaries have been defined as permanent boundaries (b1 and b3) for you to speed the selection process. Even though the boundaries are blanked, you can still select them. Double-click on operation PMBLANK_3.
In order to cut multiple depths, you must specify: the top of a pocket as Material Retained Outside (creating a pocket boundary) the bottom of the pocket as Material Retained Inside (creating an island boundary). Calling the bottom of a pocket an island may seem inconsistent, but when you specify the Depth of Cut Type to Levels at Island Tops, the tool will cut to the "island" boundary at the bottom of the pocket. This allows you specify the floor plane somewhere else in your part, such as the very bottom of the part, in order to remove blank material.
245
Cutting the Blank Geometry and Pocket in One Operation Defining the Blank Material In this operation you will cut several different depths. You will cut to the very bottom of the part to remove the blank material. You will then cut to the island tops and the bottom of the pocket. With the Part icon selected, choose the Select option in the Geometry section.
The Boundary Geometry dialog displays with the Material Side set to Inside. This is the correct setting for this operation. Choose Custom Boundary Data. Turn on the Blank Distance option and key in 1.00.
This creates an extra inch of stock surrounding the part boundary that will be used as the blank material. You are going to use the top outer edge of the part. The boundary b1 has been created for you. Set the Mode option to Boundary. Key in b1 into the Name field.
OK to accept the boundary.
Cutting the Blank Geometry and Pocket in One Operation Defining the First Part Boundary The first boundary is going to define the inside of the pocket.
246 Turn off the Blank Distance option. You want the boundary located at the top of the part, on the inside of the pocket, with the Material Retained Outside/Right. Set the Material Side to Outside/Right. Key in b3 into the name field. OK to accept the boundary.
Cutting the Blank Geometry and Pocket in One Operation Defining the Second Part Boundary The next part boundary is going to define the top of the island step. Change the Material Side to Inside/Left. The Mode needs to reflect the type of object you are selecting. Change the Mode to Face. You are going to use the top face of the island as the boundary. You do not have to include the hole in this boundary, so you will tell the system to ignore the holes. Choose the Ignore Holes option and turn it on. Select the top face of the island step as shown .
247
The boundary around the island step is defined.
Cutting the Blank Geometry and Pocket in One Operation Defining the Third Part Boundary The next part boundary is going to define the top of the island in the middle of the part. The Material Side option should still be set to Inside. The material will be retained on the inside of the boundary, preventing the island from being cut away. Leave the Ignore Holes option On. Select the top face of the island as shown.
The inside island boundary is defined.
248
Cutting the Blank Geometry and Pocket in One Operation Defining the Last Part Boundary The last part boundary is going to define the bottom of the pocket (as an island). The Material Side should still be set to Inside. Now you are ready to select the bottom face of the pocket. Select the bottom face of the pocket as shown.
All of the boundaries are defined for this operation. OK to return to the PLANAR_MILL dialog.
Cutting the Blank Geometry and Pocket in One Operation Displaying the Boundaries With the Part icon selected, choose Display from the Geometry section.
The five part boundaries are displayed.
249
Cutting the Blank Geometry and Pocket in One Operation Specifying the Floor Plane You are going to use the bottom of the part as the floor. This ensures that the tool will cut all of the blank material. With the Floor icon selected, choose Reselect.
OK the Reselect dialog. Select the very bottom face of the part.
The bottom face is defined as the floor. OK to return to the PLANAR_MILL dialog.
250
Cutting the Blank Geometry and Pocket in One Operation Specifying the Cut Depth You want to specify a Cut Depth for this operation. You are going to use Floor & Island Tops to generate one cut level at the floor plane and then generate a cleanup cut at the top of each island. Select Cut Depths.
Under Type, choose Floor & Island Tops.
OK to return to the PLANAR_MILL dialog.
Cutting the Blank Geometry and Pocket in One Operation Generating the Tool Path Generate the tool path. The first cut region of the tool path displays. Note the blank material that is defined. The tool will cut blank material to the floor plane.
251
OK as needed to continue generating the tool path. OK to complete the operation. Close the part file.
Planar Milling - Multi-Region In this lesson, you will learn how to create a multi-region Planar Milling operation.
Creating a Multi-Region Planar Mill Operation
252 You will develop a Planar Mill tool path that will cut many pockets (regions) with varying depths. You will cut one pocket, then edit the tool path and add more pockets.
Creating a Multi-Region Planar Mill Operation Opening the Part Open part file pln_pmr_1.prt from the pln subdirectory. The part has several pockets, one of which contains an island with steps and a pocket. Also note that one of the pockets has multi levels.
Choose Application
Manufacturing.
Creating a Multi-Region Planar Mill Operation Editing an Operation Double-click PMREGION in the Program Order view.
253
Creating a Multi-Region Planar Mill Operation Selecting the Part Boundaries The boundaries that you will use in this operation have been created for you (b1 through b6). Remember, in order to cut multiple pocket depths, you must specify the top of a pocket as Material Side Outside (creating a pocket boundary) and the bottom of the pocket as Material Side Inside (creating an island boundary). In review: Material Side Outside - A boundary with Material Side Outside is a pocket boundary. Material Side Inside - A boundary with Material Side Inside is an island boundary. With the Part icon selected, choose Select in the Geometry section.
Creating a Multi-Region Planar Mill Operation Defining the Top of the Pocket Set the Mode option to Boundary.
You want the tool to cut the inside of this closed boundary, so the material remaining should be outside. Set the Material Side to Outside/Right.
254
Key in b1 into the Name field and OK to accept it. The boundary b1 is highlighted on the screen.
Creating a Multi-Region Planar Mill Operation Defining the Bottom of the Pocket Set the Material Side to Inside/Left. Key in b2 into the Name field and OK to accept it. The boundary B2 is highlighted on the screen below B1.
255 You have now defined the top and bottom of the large pocket.
Creating a Multi-Region Planar Mill Operation Selecting the Remaining Boundaries Select the remaining boundaries b3 through b6 just as you did for b1 and b2. Use the following Material Side settings for each boundary: b3 . . . . . Outside/Right b4 . . . . . Inside/Left b5 . . . . . Inside/Left b6 . . . . . Inside/Left With boundaries b3 through b6 selected, your part should look similar to the part shown.
OK to return to the PLANAR-MILL dialog.
Creating a Multi-Region Planar Mill Operation Changing the Cut Depth Setting the Cut Depth Type to Levels at Island Tops will cause the tool to cut at the top of each island. You have defined the pocket bottom as an island, therefore, the tool will cut the pocket bottom at the proper depth. Choose Cut Depths.
256
Change User Defined to Levels at Island Tops.
The tool will cut to the tops of the islands. OK to return to the PLANAR-MILL dialog.
Creating a Multi-Region Planar Mill Operation Changing the Cut Order If you were to generate the tool path now, the tool would finish each level before engaging further down. You want to cut each pocket to full depth before moving on to the next pocket. Choose Cutting.
Set the Cut Order option to Depth First.
This option cuts each pocket to full depth and does not leave the pocket until reaching the bottom. OK to accept the cut parameters.
Creating a Multi-Region Planar Mill Operation Defining the Floor You are going to use the bottom of the part as the floor. Choose the Floor icon, then Reselect.
257
OK the Reselect dialog. Select the bottom face of the part.
OK to return to the PLANAR-MILL dialog.
Creating a Multi-Region Planar Mill Operation Generating the Tool Path Generate the tool path.
Each cut level displays as the tool path is generated. Continue to choose OK as necessary. The tool cuts to the bottom of the pocket.
258
The error message "Tool Cannot Fit into Level 3" will display. This is because the tool cannot reach the specified floor, which is below the bottoms of the pockets. OK the error message to continue. Reject the tool path and Refresh the graphics window.
Creating a Multi-Region Planar Mill Operation Cutting a Second Pocket You are going to add an additional pocket (a second cut region) to be cut in this operation as shown below.
This region contains a pocket within a pocket. The top boundary of the smaller pocket will define the lower boundary of the larger pocket.
Creating a Multi-Region Planar Mill Operation Editing the Part Geometry You are going to edit the part geometry by appending boundaries to the current set of boundaries.
259 Choose the Part icon, then Edit.
Creating a Multi-Region Planar Mill Operation Appending Boundaries Choose Append. Set the Mode option to Boundary. You are going to add boundaries b10, b13 and b14. You will set the Material Side for each boundary. Set Material Side to Outside/Right. Key in b10 into the Name field and OK to accept it. The boundary b10 is highlighted on the screen.
Key in b13 into the Name field and OK to accept it. Set Material Side to Inside/Left. Key in b14 into the Name field and OK to accept it. OK twice to return to the PLANAR-MILL dialog.
Creating a Multi-Region Planar Mill Operation Generating the Tool Path Generate the tool path. Each cut level displays as the tool path is generated.
260 Continue to choose OK as necessary. OK the warning. The tool path is generated. The tool cuts to the bottom of each pocket.
OK to complete the operation.
Creating a Multi-Region Planar Mill Operation Cutting the Remaining Two Pockets You will cut the remaining two pockets. You will need to append the additional boundaries ( b11 and b12 and b7, b8 and b9. See if you can do it by editing operation PMREGION_2 without further instruction. Double-click on operation PMREGION_2 in the Operation Navigator and Edit the boundaries listed above.
Append
Remember, in order to cut multiple pocket depths, you must specify the top of a pocket as Material Retained Outside (creating a pocket boundary) and the bottom of the pocket as Material Retained Inside (creating an island boundary). Top of Pocket=Outside/Right B7 Top of Pocket (island)=Outside/Right B8 Bottom of Pocket-Inside/Left B9
261
The pocket with the open end also requires a Closed Boundary Top of Pocket=Outside/Right B11 Bottom of Pocket=Inside/Left B12
Creating a Multi-Region Planar Mill Operation Generating the Tool Path When you have all the boundaries correctly specified, you are ready to generate the tool path. Generate the tool path. Turn the Display Cut Regions and Pause After Display options off. OK to generate the tool paths.
262
Creating a Multi-Region Planar Mill Operation Visualizing the Tool Path Choose the Verify icon
at the bottom of the dialog.
Choose the Dynamic tab. Choose Play Forward.
Cancel the tool path visualization.
Analysis Tools The Analysis Tools are used to visually inspect the cutting areas in the tool path.
263
Analysis Tools Analyzing Tool Paths Double-click on the PMREG_ANAL icon in the Operation Navigator.
Choose the Options icon at the bottom of the dialog. Choose Analysis Tools.
Analysis Tools Analyzing the Tool Path by Level Note that the number of levels in the tool path is displayed at the top of the dialog.
This dialog acts like a replay tool. It will only display the tool path at a specified level. Key in 4 in the Current Level field and press the Enter key. The tool movement at level 4 is replayed in the graphics window.
264
The Previous and Next arrows on the dialog select the tool path at the next level or the previous level. Choose the Previous or Next arrow. The tool path at that level is replayed. OK until you return to the PLANAR-MILL dialog. Cancel the PLANAR-MILL dialog.
Analysis Tools Generating the Tool Path Double-click on the PMREG_ANANL_2 icon in the Operation Navigator Generate the tool path.
Choose the Options icon. Choose Analysis Tools. The Analysis Tools dialog displays along with the cut region for the first cut. This dialog looks very different from the Analysis Path By Level dialog. Some of the options, such as Current Level and Edit Display, function in the same way.
265
Analysis Tools Analysis Tools Level Option Look at the top of the dialog and note the two settings, Region and Level.
The Level setting displays all of the offset shapes and regions at the current level. You can use the Previous and Next arrows to cycle through the different levels. This option is the same as the previous Analysis Tool. Choose Show Cut.
The cut motion for the specified level (level 1) is replayed.
Analysis Tools Displaying Blank Cut Shape Choose Blank Cut Shape.
266 Only the blank material offset shape displays.
If you use the arrows now, the system will cycle through only the Blank Shape Traces. Choose the Previous or Next several times to cycle through the Blank Cut Shape at each level.
Analysis Tools Displaying Part Shape Choose Part Shape.
You should see only part shapes displayed in the graphics window. If you cycle through the levels now, you will only see cut levels for the part displayed. Choose the arrow several times to cycle through the Part Shapes at each level. Key in 2 into the Current Level field and press Enter.
Analysis Tools Displaying Uncut Regions Choose Uncut Regions.
The Uncut Region at level 2 displays.
267
Analysis Tools Displaying Cut Regions Choose Cut Regions.
Analysis Tools Using the Cycle Option The Cycle option enables you to specify a subset of a specified shape. A drop down menu displays three options: All - displays all of the specified shapes within each level as you cycle from one level to the next. Shape - highlights each specified shape in sequence (only within the currently displayed level) as you select the arrows. Segment - highlights each segment of the displayed shapes in sequence (only within the currently displayed level) as you select the arrows. Set the Cycle option to Shape.
268
The display in the graphics window is changed.
The blank shape displays. Use the arrows to cycle through the different shapes at level 2, returning to the blank shape. Change the Cycle option to Segment. Use the arrows to cycle through the different segments of the blank shape. Change the Cycle option back to All.
Analysis Tools The Dump Level Option This option is only available when using the Level option and when Cycle is set to All. Dump Level allows you to write just the current level to a file so that problems occurring in that level can be analyzed by CAM Development.
Analysis Tools Analysis Tools Region Option The Region setting displays each cut region individually within the operation. Choose the Region option.
269
The cut regions are displayed in the graphic window. Although you no longer have control of the cut levels, the cut regions for level 2 are displayed. This is because you were at level 2 when you changed from Level to Region.
Use the Previous and Next arrows to cycle through the different Cut Regions. OK two times to return to the PLANAR-MILL dialog. Cancel the Analysis Tools dialog. Cancel the operation. Close the part file.
Face Milling Face Milling is a fixed axis milling method similar to Planar Milling, but designed specifically to rough and finish the planar faces of a part. It allows you to specify the face geometry simply by selecting the faces to be machined. It also allows you to define face geometry by selecting existing curves and edges or by specifying a sequence of points in much the same way as Planar Milling.
270
The tool axis is automatically defined as the normal of the first selected face boundary plane. Since Facing removes material in planar levels with respect to the tool axis, the normal of a face boundary plane must be parallel to the tool axis. If it is not, the face will be ignored during tool path generation. In this lesson you will create a Face Milling operation that finishes the faces of a part. You will also learn several ways to cut across open and closed voids and learn how to create mixed and manual cut patterns.
Creating a Simple Face Milling Operation You will create a simple Face Milling operation.
Creating a Simple Face Milling Operation Opening the Part Open part file pln_facing.prt from the pln subdirectory.
271
Choose Application
Manufacturing.
Creating a Simple Face Milling Operation Beginning the Operation Choose the Create Operation icon. Choose mill_planar as the Type. Choose FACE_MILLING as the subtype.
Specify the following parent groups.
OK to begin creating the operation.
Creating a Simple Face Milling Operation Displaying the Part Geometry Choose the Part icon and Display to verify the part geometry.
272
The part geometry has already been defined in the WORKPIECE parent group.
Refresh the graphics display.
Creating a Simple Face Milling Operation Defining the Faces You will define the faces to be machined. Choose the Face icon and Select.
With the Face Boundary icon chosen, select the six faces illustrated below.
273
Face boundaries are processed as blank boundaries. The center line of the tool cuts all the way to the boundary (where it does not gouge the part), which results in the material being removed along the edge of the face. OK to complete the selection. Choose Follow Periphery as the Cut Method.
Creating a Simple Face Milling Operation Generating the Tool Path Generate the tool path. Turn all of the Display Parameter options off and OK to continue.
Notice that the tool path does not avoid the clamps. You will need to define the clamps as check geometry.
Creating a Simple Face Milling Operation Defining Check Geometry You will define solid bodies as check geometry.
274 Choose the Check Body icon and Select.
Select the three solid bodies that represent clamps.
OK to complete the selection.
Creating a Simple Face Milling Operation Generating the Tool Path Generate the tool path. Turn off all of the Display Parameters and OK to continue.
Notice that the tool path now avoids the clamps. In addition, you can define multiple level cuts by specifying Blank Distance and Depth Per Cut. OK to complete the operation.
275
Creating a Simple Face Milling Operation Visualizing Material Removal You will use Verify Toolpath to graphically simulate material removal for the program. In the Program Order View of the Operation Navigator, choose PROGRAM. Choose the Verify Toolpath icon
in the toolbar.
Choose the Dynamic tab. Choose the Play Forward icon.
OK to complete the tool path visualization. Close the part file.
Cutting Across Closed Voids The cut pattern can be maintained or excluded when closed voids are encountered. This insures that the tool will cut across rather than around voids when Zig, Zig-Zag, or Zig with Contour is used. An area fully enclosed inside a single cut region that is empty or devoid of material is regarded as a closed void. An area along the periphery of a cut region that is empty or devoid of material is regarded as an open void. Cut patterns are not maintained across open voids. The cylindrical area illustrated below is an open void because it crosses cut regions.
276
Cutting Across Closed Voids Excluding Cut Pattern From Voids Open part file pln_facing_1.prt from the pln subdirectory. Choose Application
Manufacturing.
Double-click on the FACE_MILLING icon to edit the operation.
Choose Cutting. Notice that Across Voids is set to Follow. This option excludes the cut pattern from closed voids, causing the cut pattern to follow the shape of the cut region.
OK to accept the Cut Parameters. Replay the tool path. The cut pattern is excluded from the closed void.
277
Cutting Across Closed Voids Cutting Across Voids Choose Cutting. Set the Across Voids option to Cut.
This option maintains the cut pattern across closed voids at the cut feed rate. OK to accept the Cut Parameters. Generate the tool path.
278
Cutting Across Closed Voids Traversing Across Voids Choose Cutting. Set the Across Voids option to Traverse.
This option maintains the cut pattern across closed voids but uses the cut feed rate only while the tool is in contact with material. The traversal feed rate is used when the tool is not cutting material. Notice the Traverse Distance is set to zero. The Traverse Distance represents the minimum amount of empty space the tool must cut to employ a traversal feed rate inside a void. A Traverse Distance of zero ensures that a traversal feed rate will always be used when the tool is not cutting through material. OK to accept the Cut Parameters. Generate the tool path.
Cutting Across Closed Voids Editing the Blank Overhang Blank Overhang is the distance that the cutting tool travels beyond the edge of a face. By setting the Blank Overhang parameter to a value smaller than the cutter diameter, tool path movement is kept to a minimum.
279
Choose the Edit Display icon
under Tool Path.
Choose 2-D for the Tool Display and OK to accept it. Replay the tool path. Notice how the tool travels beyond the edge of the face the full diameter of the tool.
Choose Cutting. Key in 25 to define the Blank Overhang distance as a percentage of the tool diameter.
OK to accept the Blank Overhang. Generate the tool path.
280
Cutting Across Closed Voids Specifying the Tool Run-Off When using a Zig or Zig-Zag cut pattern, the Tool Run-Off parameter allows you to retract the tool completely off the part after each cutting pass. This is often desirable when finishing to achieve a quality finish.
Tool Run-Off
When finish milling using a Zig or Zig-Zag cut pattern, it is often desirable to retract the tool completely off the part after each cutting pass to achieve a quality surface finish. However, when roughing production parts, it is sometimes desirable to allow the tool to stay on the part after each cutting pass to minimize toolpath time The Tool Run-Off parameter satisfies both cases. Tool Run-Off is supported for Zig and ZigZag cut types in face milling, planar milling, and cavity milling operations and is only applied to operations which employ an Automatic Retract. When Tool Run-Off is On, the tool will automatically retract off the part after each cutting pass by a distance equal to the horizontal clearance. When Tool Run-Off is Off, no attempt is made to retract the tool off the part after each cutting pass. Depending upon the amount of the Blank Overhang, the tool may or may not remain on the part. The tool will always engage from the safe shape for a Zig or Zig-Zag cut. The tool will retract to the safe shape only if the Tool Run-Off option is On and and an Automatic Retract is employed by the operation.
281
Choose Method. Notice that Tool Run-Off is On.
Also notice that the horizontal clearance is set to 0.100.
The tool will retract off the part after each cutting pass by a distance equal to the horizontal clearance. You will increase the horizontal clearance so you can see the Tool Run-Off a little more clearly. Key in 0.30 in the Horizontal field and OK to accept it. Change to a Top view.
Cutting Across Closed Voids Generating the Tool Path Reject the previous tool path. Generate the tool path.
282
OK to complete the operation. Close the part file.
Creating Mixed and Manual Cut Patterns Face milling allows you to specify a different cut pattern for each region of an operation. In addition to automatic cut patterns (Zig-Zag, Zig, Zig with Contour, Follow Periphery, Follow Part, Profile), you can define manual cut patterns or exclude cut patterns completely. Manual cut patterns are defined interactively, allowing you to control tool movements individually. This is especially useful when you need to define a simplified tool path that is independent of the shape of the cut region. When using a large tool for example, a straight tool path across a complex shape is sometimes a more efficient way to machine the face as illustrated below.
283
Creating Mixed and Manual Cut Patterns Displaying the Face Boundaries You will open a part and display the face boundaries of an existing face milling operation. Open part file pln_facing_2.prt from the pln subdirectory. Choose Application
Manufacturing.
In the Program Order view of the Operation Navigator, double-click on the FACE_MILLING icon to edit the operation.
Choose the Face icon and Display.
Notice that three faces have been defined.
Creating Mixed and Manual Cut Patterns Specifying the Tool Path Display A Silhouette tool display will allow you to clearly see the area the tool cuts across.
284
Choose the Edit Display icon
under Tool Path.
Choose 2-D for the Tool Display and Silhouette for the Path display.
OK to accept the Display Options.
Creating Mixed and Manual Cut Patterns Defining Mixed Cut Methods The Mixed cut method allows you to specify a cut pattern for each region. Choose Mixed.
Choose Generate. The Mixed Cut Pattern dialog displays. The current cut level being processed and the region number at that level are displayed at the top of the dialog.
The order in which the regions are cut is determined by Region Sequencing. In this example, the Region Sequencing is set to Standard, so the regions will be cut in the order the faces were selected. The first cut region is displayed.
285
Turn on all three display parameters.
Creating Mixed and Manual Cut Patterns Specifying a Follow Periphery Cut Method You will specify a cut method for the first region. Choose Follow Periphery.
OK to accept the cut pattern and display the tool path.
OK to complete the cut pattern and display the next cut region.
286 Notice that the follow periphery cut pattern has been added to the list box.
The most efficient tool path for this next cut region is one that cuts in straight line segments where possible rather than following the exact shape of the region. A manual cut pattern will allow you to do this.
Creating Mixed and Manual Cut Patterns Specifying a Top View It is easier to define a manual cut pattern in a top view. MB3
Replace View
TOP.
Refresh the graphics display. You should be able to see the shape of the cut region clearly.
287
Creating Mixed and Manual Cut Patterns Defining a Manual Cut Pattern You will define a manual cut pattern to create an optimal tool path for this cut region. Choose Manual.
OK to begin defining the Manual cut pattern. The Create Manual Cut Pattern dialog contains options that allow you to interactively create specific tool motions for the current cut region and level. Most parameters that apply to automatic cut patterns (Cutter compensation, Engage/Retract parameters, Cutting parameters) do not apply to the Manual cut pattern.
Creating Mixed and Manual Cut Patterns Repositioning to a Center Point The Reposition To Point option is automatically selected, allowing you to define a transfer move from the previous cut region.
288
Choose Arc/Ellipse/Sphere Center as the Point Method.
Select the hole illustrated below to define the center as the reposition point.
Creating Mixed and Manual Cut Patterns Cutting to a Center Point The engage will be made to a center point on the face. Choose Move To Point.
Choose Engage as the Motion Type.
289 Select the small hole to define the center as the point the tool will cut to.
Creating Mixed and Manual Cut Patterns Cutting to a Point on the Cut Region Shape The next cutting move will cut in a straight line to a point on the cut region shape. Choose Move To/From Shape.
Choose Cursor Location as the Point Method.
Be sure Minimum Distance To Shape has been chosen.
These options allow you to create a point on the cut region shape close to where you indicate. Be sure Cut Region is specified as the shape to be selected.
290
Choose Cut as the Motion Type.
Indicate on or near the center of the cut region segment as illustrated below.
The indicated point projects at a minimum distance to the cut region shape where the system defines the point the tool will cut to. The face is cut with a simple linear move.
291
Creating Mixed and Manual Cut Patterns Cutting Along the Shape of the Cut Region The next several moves need to cut along the shape of the cut region. This will allow the tool to cut the face while avoiding the boss. Choose Move Along Shape.
Choose Minimum Distance To Vertex.
This option assures that the vertex of the cut region shape closest to where you indicate is defined as the point the tool will cut to. Indicate on or near the cut region vertex as illustrated below.
The tool moves along the shape in the wrong direction.
292
Choose the Reverse Direction icon.
The tool should now move along the shape in the opposite direction.
Select on or near the next cut region vertex as illustrated below.
293
Choose Minimum Distance To Shape.
Indicate on or near the center of the cut region segment as illustrated below.
Creating Mixed and Manual Cut Patterns Cutting to an End Point The next cutting move will be made to an end point. Choose Move To Point.
294
Choose End Point as the Point Method.
Select the end point of the arc as the next point the tool will cut to.
Creating Mixed and Manual Cut Patterns Cutting to a Center Point The last two cutting moves will be made to center points on the face. Choose Arc/Ellipse/Sphere Center as the Point Method.
Select the small hole to define the center as the next point the tool will cut to.
295
Select the small hole to define the center as the last point the tool will cut to.
OK to complete the manual cut pattern. Notice that the manual cut pattern has been added to the list box. Choose Format original view.
Layout
Refresh the graphics display.
Replace View
LAYOUT1 and OK to return to the
296
Creating Mixed and Manual Cut Patterns Excluding a Cut Region The next cut region displays at the center of the part. You will not cut this region.
Choose Omit as the Cut Method for this region.
OK to complete the mixed cut pattern. Replay the tool path.
Creating Mixed and Manual Cut Patterns Visualizing the Tool Path Choose the Verify
icon at the bottom of the dialog.
Slow down the Animation Speed to 8.
297 Choose the Play Forward icon.
Choose the Dynamic tab. Choose the Play Forward icon. Choose Offset from Part and key in 0.10 for the Offset.
OK to accept the blank material and begin the visualization. The system displays the dynamic material removal. Notice that the cut region specified as None was not cut.
OK to complete the tool path visualization.
298
Creating Mixed and Manual Cut Patterns Editing a Cut Pattern You can go back and edit any of the cut patterns. Reject the tool path. Choose the Edit Display icon
and turn on Pause After Display.
This will allow you to edit one cut region at a time. OK to accept the Display Options. Choose Generate. The Mixed Cut Pattern dialog displays along with the first cut region. OK to display the Follow Periphery cut pattern. OK to display the next cut region. OK again to display the Manual cut pattern. OK to display the last cut region. reg_3_lv_3_omit should be highlighted in the list box.
You will change the cut pattern for this region to Profile. Choose Profile.
OK to accept the cut pattern. OK to finish editing mixed cut pattern.
Creating Mixed and Manual Cut Patterns Visualizing the Tool Path Choose the Verify icon at the bottom of the dialog.
299 Choose the Dynamic tab. Choose the Play Forward icon. Choose Offset from Part and key in 0.10 for the Offset. OK to accept the blank material and begin the visualization. Material is now cut from every cut region.
OK to complete the tool path visualization. OK to complete the operation. Close the part file.
Cavity Milling Cavity Milling is designed to rough out large volumes of material from cavities and cores, especially those with tapered walls such as dies and molds. Cavity Milling is similar to Planar Milling in that it uses a fixed tool axis and removes the material in planar cut levels.
300
In this lesson you will create Cavity Milling operations that rough out cavities and cores.You will also learn how to use a faceted body to perform rest milling.
Machining the Body of the Bottle You will create an operation that roughs out a cavity.
Machining the Body of the Bottle Opening the Part Open part file pln_cavity_assy.prt from the pln subdirectory. This part file has features commonly found in many molds. The sides have a taper angle and the bottom has a curved face.
301
Choose Application
Manufacturing.
Machining the Body of the Bottle Defining the Workpiece Using Solids You will edit the WORKPIECE object to define the part and blank geometry. Later, you will use this object as a parent group for the operation.
Choose the Geometry View icon
in the toolbar.
Expand the MCS_MILL object and highlight WORKPIECE.
Choose MB3
Edit.
The MILL_GEOM dialog displays.
Machining the Body of the Bottle Defining the Material Type Before you select the part and blank geometry, you should define the type of material to cut. The material you are cutting has a very important effect in determining the cutter speeds and feeds. Choose Material: CARBON STEEL.
302 The Part Material listing displays in a Search Result dialog. Highlight MATO 00266 ALUMINUM and OK to accept it.
The part material has been changed to ALUMINUM.
Machining the Body of the Bottle Defining the Part Geometry With the Part icon chosen, choose Select
Select the body as the part geometry.
OK to accept the Part Geometry dialog.
Machining the Body of the Bottle Defining the Blank Geometry.
303 Choose the Blank icon and then Select.
Select the rectangular block as the Blank Geometry.
OK the Blank Geometry dialog. OK the MILL_GEOM dialog. The WORKPIECE geometry has been defined.
Machining the Body of the Bottle Beginning the Operation Choose the Create Operation icon Be sure Type is set to mill_contour. Choose the CAVITY_MILL icon.
Specify the following parent groups.
in the toolbar.
304
Enter RUF_BODY in the Name field. OK to begin creating the operation.
Machining the Body of the Bottle Defining the Cut Levels You will reduce the first cut range to the depth of the vertical cavity walls and then add an additional range with smaller cut levels for the curvature of the bottom of the cavity. Choose Cut Levels.
Zoom in on the corner of the part.
Machining the Body of the Bottle Defining the Level of the Bottom of the First Range The system initially assumes that the first cut range is from the top of the blank geometry to the bottom of the part geometry. The limits of this range are indicated by the large white plane symbols.
305
The range depth is currently indicated as 35.00 mm in the Range Depth field and on the slider bar.
You will raise the bottom of the range. Choose Generic Point.
Select the edge end point as illustrated below.
Use MB3
Refresh to clear the graphics window.
Choose Display to display the new cut range. The two large plane symbols display the reduced cut range. The smaller plane symbol indicates the first cut depth, which is set at 6.00 mm. Because the sides of the cavity have a small draft angle, a 6.00 mm depth of cut will provide adequate material removal.
306
Machining the Body of the Bottle Defining the Second Range You will append an additional cut range below the current range and set the depth per cut to a smaller value to provide for more material removal on the curved face. Choose Add Ranges.
You will reference the new range from the bottom of the currently highlighted range. Change the Reference option to Range Bottom.
Zoom in on the logo area. Choose Generic Point. Select the end point as illustrated below.
307
OK the Point Constructor dialog. MB3
Fit to display all the geometry in the graphics window.
Choose Display to display the new cut range. The new cut range is indicated by the large plane symbols beneath the first cut range.
Machining the Body of the Bottle Specifying the Depth per Cut You will change the depth per cut in the second range to 1.00 mm. This will remove more material from the curved faces by creating smaller steps. Choose Modify Ranges.
You need to modify the lowest range. It should be highlighted. If the lowest range is not highlighted in white, you can change the range you are modifying by choosing the Current Range arrows.
308
Selecting the up or down arrow will change the range being modified. Enter 1.00 in the Depth per Cut field and press Enter.
The graphics display indicates the new, smaller, depth per cut by displaying six plane symbols between the large range symbols.
OK the Cut Levels dialog. More About Cut Levels
The Cut Levels dialog allows you to adjust the planes of the cuts and the depths of the cuts. Some definitions are in order to clarify the terminology: A Range is a specified amount or depth of material within the cavity to be removed. You can specify up to 10 Ranges. A Cut Level is a specified depth of cut within a Range to be removed.
1) Use this area to add or modify the cut range. You can also specify the maximum depth per cut within the range.
309
2) Use this area to define where the range is measured from.
3) Use these arrow keys to select a defined range. 4) Use these icons to remove a defined range or reset any range modifications.
The dialog displays the exact depth of this range - both in the Range Depth field and at the end of the slider bar. You can use one or more ranges to cut the cavity. Assigning multiple ranges allows more control over the amount of material being removed within the cavity. For example, you may want to remove more material per cut in the upper portion of the cavity and smaller amounts of material towards the bottom of the cavity. Defining several ranges would accomplish this. Because the first range is defined for you, you must choose Modify in order to make any changes to the range. You must be certain the Modify Ranges icon is depressed for any changes to be applied.
By default, the Reference option is set to Top Level. This option determines where the Range Depth value you specify is referenced from. Notice the graphics area, several plane symbols are displayed. The system automatically determines the first range based on the highest and lowest points defined by the part and blank geometry. The top and bottom of the range are indicated by the two large plane symbols.
310
The smaller plane symbols indicate the depth per cut. Here is a summary of the Reference options: Top Level will reference the Range Depth value from the top of the first cut range. Range Top will reference the Range Depth value from the top of the currently highlighted range. Range Bottom will reference the Range Depth value from the bottom of the currently highlighted range. WCS Origin will reference the the Range Depth value from the origin of the WCS.
Machining the Body of the Bottle Setting the Feed Rates Tool motion speeds and feeds are set using the values stored in tables. Choose Feed Rates.
By default, only the Cut feed rate is defined at 250.000 mmpm. The feeds and speeds can be automatically calculated and set to values appropriate for your tool geometry and material and your part material by selecting Reset from Table.
311 Choose Reset from Table. An Error dialog displays. The Error displays because there is no data in the Feeds and Speeds data file for the combination of a ceramic tool and aluminum part material.You will change the tool material in the next step. OK the Error dialog. OK the Feeds and Speeds dialog.
Machining the Body of the Bottle Changing the Tool Material Choose the Groups tab. With the Tool option selected, choose Edit.
The Milling Tool-5 Parameters dialog displays. Change the Material to High Speed Steel (HSS).
OK the Milling Tool-5 Parameters dialog.
Machining the Body of the Bottle Setting the Feed Rates Choose the Main tab. Choose Feed Rates. Choose Reset from Table. The feeds and speeds are loaded into the appropriate fields.
312
OK the Feeds and Speeds dialog.
Machining the Body of the Bottle Generating the Tool Path Generate the tool path.
OK to generate the first level.
OK several more times to display the traces and tool paths at each level.
313 The last cut level is generated and displayed showing how the curved face of the bottom of the cavity has narrowed the tool path.
After the lowest cut level is generated, the Processor Error message "Tool cannot fit into level 8" displays. This message indicates that there is still material to be removed below the lowest level cut, but the tool cannot fit into the remaining volume. You must finish cutting this material with either a smaller tool or a different cutting method. OK the Warning dialog.
Machining the Body of the Bottle Visualizing Material Removal A shaded display of the material removal can help you to visualize the machining operation. Choose the Verify icon
at the bottom of the dialog.
Choose the Dynamic tab.
Choose the Play Forward icon at the bottom of the dialog. Notice that the large tool has not removed any material from the neck of the bottle.
314
Machining the Body of the Bottle Displaying Excess Material The Compare function displays areas where excess material remains due to large scallops and inaccessibility of the tool. This function is useful in determining how much material remains for subsequent operations to remove and for comparing the finished machined part to the modeled part. You can compare the remaining material with the part geometry. Choose Compare.
The white area indicates that further finishing is required to machine to the specified Outtol.
OK the Toolpath Visualization dialog. OK to complete the operation.
Machining the Neck of the Bottle
315
You will create a Cavity Mill operation that uses a small tool to rough out the neck of the bottle.
Machining the Neck of the Bottle Beginning the Operation Choose the Create Operation icon
in the toolbar.
Be sure Type is set to mill_contour. Choose the CAVITY_MILL icon.
Specify the following parent groups.
Enter RUF_NECK in the Name field and OK to begin creating the operation.
316
Machining the Neck of the Bottle Defining the Trim Boundary You will use an existing boundary to define the Trim boundary that will constrain the cut region to the neck of the bottle. Choose Format
Layer Settings in the menu bar.
Make Layer 4 Selectable. OK the Layer Settings dialog. A boundary displays surrounding the neck geometry of the bottle. You will use this boundary to define the Trim boundary.
Choose the More Tab. Choose Select under Boundary Geometry.
Choose Boundary as the Mode, Outside/Right as the Side Trimmed, and Trim as the Geometry Type.
317 These parameters will restrict the tool path to the inside of the inside of the selected boundary. Choose the boundary.
OK to accept the boundary.
Machining the Neck of the Bottle Defining the Cut Method Choose the Main tab. Set the Cut Method to Follow Periphery.
The follow periphery cut method creates cut patterns using only the outside part geometry.
Machining the Neck of the Bottle Defining Cut Levels Choose Cut Levels. Choose Generic Point. Choose the Quadrant Point icon. Select the bottom of the arc as illustrated below.
318
Enter 0.500 in the Depth per Cut field and Enter.
OK the Cut Levels dialog.
Machining the Neck of the Bottle Using Pre-Drill Engage Points Because the bulk of the material has already been removed from the body of the bottle, the tool can easily move to cut depth from the body area. You will define a pre-drill engage point to position the tool close to the neck to begin the cutting motion. Choose Points in the Control Geometry section. Choose Edit in the Pre-Drill Engage Points section.
If the depth field is left with the 0.00 default value, the Pre-Drill Engage Point will be applied to all cut levels. Choose Generic Point. Choose the Cursor Location icon. Indicate a point at the approximate screen position illustrated below.
319
OK the Point Constructor dialog. OK the Pre-Drill Engage Points dialog OK the Control Geometry dialog.
Machining the Neck of the Bottle Setting the Feeds and Speeds You need to reset the feed rates so that they are compatible with the new, smaller tool and the high speed steel tool material. Choose Feed Rates and Reset from Table. The recalculated speeds and feeds are displayed in their appropriate fields.
OK the Feeds and Speeds dialog.
320
Machining the Neck of the Bottle Generating the Tool Path Generate the tool path. Turn the Pause After Display option off. OK to continue generating the tool path. The path is generated. All of the engage motions are outside the material being cut.
OK to accept the operation and generated tool path.
Machining the Neck of the Bottle Visualizing Multiple Tool Paths. You will use Verify Toolpath to graphically simulate material removal for both operations. In the Program Order VIew of the Operation Navigator, highlight NC_PROGRAM.
Choose the Verify Toolpath icon
in the toolbar.
The Toolpath Visualization dialog displays. Choose the Dynamic tab and then Play Forward.
321
This cumulative display of the material removed is helpful in indicating areas requiring further machining. Choose Compare.
The white areas indicate the areas where further finishing is required to machine to the specified Outtol. OK the Toolpath Visualization dialog. Close the part file.
Machining a Core You will use Cavity Mill to rough out a core.
322
Machining a Core Opening the Part Open part file pln_cavity_2.prt from the pln subdirectory.
Choose Application
Manufacturing.
Machining a Core Choosing the Operation to Edit You are going to edit an existing Cavity Mill operation. Expand the WORKPIECE object in the Geometry View of the Operation Navigator. Double-click on the operation named BLNK_GEOM.
323
The CAVITY_MILL dialog displays. Some of the options that have been set for you are:
Machining a Core Looking at the Part Geometry With the Part icon chosen, choose Display. The part geometry highlights.
Machining a Core Defining the Blank Geometry Choose the Blank icon, then Select.
Select the white rectangular body that surrounds the part.
324
OK to accept the selection.
Machining a Core Defining the Cut Levels You are going to define Cut Levels by specifying Ranges and Cut Depths. Choose Cut Levels.
The current cut range is indicated by two plane symbols.
The blank geometry is a little more than .5 inches above the top of the part geometry. You will move the cut range to the top of the blank geometry and set the depth of each cut level to .25 inches.
Machining a Core
325
Removing the Current Range Choose the Remove Current Range icon to delete this range.
OK the Cut Levels dialog. Refresh the graphics window. Choose Cut Levels again.
Machining a Core Modifying the Range The current range is referenced from the top of the Blank geometry and extends to the top of the part geometry. You will extend the bottom of the range to a lower level so that it removes more of the blank material.
Choose the Modify Ranges icon.
Choose Generic Point. Select the end point of the edge illustrated below to define the bottom of the range.
326
The Range Depth field will read 2.50. The range will remain associative to this face. If the face is modified or deleted, the range is adjusted or deleted with it.
Machining a Core Modifying the Depth per Cut Key in 0.250 for the Depth per Cut and Apply.
Small plane symbols indicate the depth per cut for the current range.
Machining a Core Defining the Second Range
327 Choose the Add Ranges icon.
Slide the Range Depth pointer to 5.50.
Moving the slide bar to 5.50 sets the range bottom to the bottom of the Blank geometry. Key in 1.000 for the Depth per Cut and Apply.
The cut levels should look similar to those illustrated below.
OK to accept the cut levels.
Machining a Core Generating the Tool Path Generating this tool path may take a little longer than other tool paths you have generated due to the complexity of the part and the number of cut levels.
328 Generate the tool path. The first cut region and the Display Parameters dialog are displayed.
OK once to continue processing the tool path. The first cut level is generated. The tool removes .25 from the top of the blank material.
OK twice to generate the second cut level. The second cut level cuts to the top of the island. OK twice to generate the third cut level. The third level cuts around the islands.
329
Turn the Pause After Display option off. OK to finish processing the tool path. The tool path cuts around the islands to the bottom of the first range and then removes the blank material around the outside of the part.
Machining a Core Visualizing Material Removal for the Cavity Mill Operation MB3 Expand in the TFR-ISO view so that this is the only view that appears in the window. Choose the Verify icon at the bottom of the dialog. Choose the Dynamic tab. Choose the Play Forward icon.
The roughing operation leaves large scallops for the subsequent finishing operations to remove.
330 OK to complete the tool path visualization. OK to complete the operation. MB3
Expand so that all four views again appear in the window.
Refresh the graphics display. Next, you are going to remove blank material using an offset.
Machining a Core Making the Blank Geometry Invisible You are going to remove the modeled blank geometry from the display so you can later define blank geometry by specifying a blank distance. Choose Format
Layer Settings.
Select BLANK_GEOM_TOP in the list box and set it to Invisible.
OK to accept the layer settings. The blank material no longer displays.
Machining a Core
331
Choosing the Operation to Edit Double-click on the operation named BLNK_DIST.
Machining a Core Defining the Blank Distance You are going to define blank geometry uniformly to the entire part by specifying a blank distance. Choose Cutting. Key in 0.250 for the Blank Distance.
Also note that there is a Blank Stock setting as well. Blank Stock is the additional stock that is applied to blank geometry. OK to accept the cut parameters.
Machining a Core Generating the Tool Path Generate the tool path. The first cut regions are displayed. OK to continue processing the tool path. The tool cuts around the islands taking into consideration the Blank Distance. This is a very different tool path than the previous tool path you generated using the modeled blank geometry.
332
Turn the Pause After Display option off. OK to continue processing the tool path. OK in the Cavity-Mill dialog to complete the operation. Refresh the graphics display.
Machining a Core Using Blank Geometry to Isolate Areas You can use blank geometry to isolate and cut specific areas of the part. Choose Format
Layer Settings.
Select BLANK_ISOLATE_1 in the list box and set it to Selectable.
OK to accept the layer settings. A white block that you will use as blank material displays.
333
Machining a Core Choosing the Operation to Edit Double-click on the operation named BLNK_ISO.
Machining a Core Displaying the Part Geometry With the Part icon chosen, choose Display.
334 This time all of the faces have not been selected. You could have used all of the faces, but adding unnecessary part geometry will increase the time required for the tool path to generate. What is important is that the part geometry you wish to cut be contained within the blank material.
Machining a Core Defining the Blank Geometry Choose the Blank icon and then Select. Select the white rectangular block.
OK to accept the blank geometry.
Machining a Core Displaying the Cut Levels Choose Cut Levels in the Control Geometry section. The cut levels start at the top of the blank geometry and extend to the bottom of the blank geometry
OK to return to the CAVITY-MILL dialog.
Machining a Core Generating the Tool Path
335 Generate the tool path. The first cut region is displayed. OK once to continue processing the tool path. The tool cuts the top of the part within the blank geometry. OK twice to continue processing the tool path. The tool cuts around the island.
Turn the Pause After Display option off. OK to complete processing the tool path. In this operation, the tool begins machining each cut level in the middle of the region and cuts outward. Usually, you should start machining from the outside of the stock and cut inward. You can correct this by changing the pocket direction parameter. Reject the tool path.
Machining a Core Changing the Cut Direction You are going to change the cut direction so that the tool starts machining from the outside of the stock and cuts inward. Choose Cutting. Change the pocket direction to Inward.
336 OK to return to the CAVITY_MILL dialog.
Machining a Core Generating the Tool Path Generate the tool path. The first cut region displays. OK once to continue processing the tool path. The tool cuts from the outside in.
OK as necessary to complete the tool path. OK to complete the operation.
Machining a Core Using Blank Distance with Blank Geometry You can use modeled blank geometry and Blank Distance to machine parts which are more heavily stocked in some areas than others. The following figure illustrates rectangular blank geometry surrounding the left top side of the part. The remaining part area has a Blank Distance value of 0.1 specified because it was cast closer to size.
You will modify operation BLNK_ISO_DIST to generate a tool path with the stock defined as above.
337 Double-click on the operation named BLNK_ISO_DIST in the Operation Navigator.
Machining a Core Displaying the Part Geometry Choose Display from the Geometry section.
Machining a Core Defining the Blank Geometry You are going to define the blank geometry using the same rectangular block used in the operation you just generated. Choose the Blank icon, then Select in the Geometry section. Select the white rectangular block that surrounds the part and then OK to accept it.
Machining a Core Defining the Blank Distance Choose Cutting. Key in .25 for the Blank Distance.
338
OK to accept the cut parameters.
Machining a Core Specifying the Cut Levels Choose Cut Levels. You will define the cut range and levels to machine the top of the part. Choose Modify Ranges.
Choose Generic Point. Select the edge of the white block as illustrated below to define the bottom of the range.
Be sure 0.25 is displayed in the Depth per Cut field. Refresh the graphics display and choose Display. The cut levels display.
339
OK to return to the CAVITY_MILL dialog.
Machining a Core Generating the Tool Path Generate the tool path. Turn all of the Display Parameter options off.
OK to complete generating the tool path. OK to complete the operation. Close the part file.
Tolerant Machining and Undercut Handling Tolerant Machining is the preferred method for most milling operations. It is a reliable algorithm to find the correct machinable regions without gouging the part. In this case it will prevent the shank of the tool from rubbing against the part geometry by applying a horizontal clearance.
340
Tolerant Machining and Undercut Handling Opening the Part Open part file pln_cavity_3.prt from the pln subdirectory.
Choose Application
Manufacturing.
Tolerant Machining and Undercut Handling Choosing the Operation to Edit Expand the objects in the Geometry View of the Operation Navigator. Double-click the UNDERCUT_TOL icon to edit the operation.
Tolerant Machining and Undercut Handling Using Tolerant Machining
341 Tolerant Machining uses a reliable algorithm to find the correct machinable regions without gouging the part. In the following figure, the shank of the tool does not gouge the canted rib when using Tolerant Machining.
Unlike Undercut Handling, it does not apply a horizontal clearance to the tool shank. Choose Cutting. Notice that when Tolerant Machining is turned on, Undercut Handling is not available.
OK to accept the Cut Parameters.
Tolerant Machining and Undercut Handling Generating the Tool Path You will first generate the tool path with only Tolerant Machining turned on. Generate the tool path. Turn all of the Display Parameter options off. OK to complete the tool path. The tool does not collide with the canted wall of the pocket.
Tolerant Machining and Undercut Handling Turning Off Tolerant Machining and Undercut Handling
342 You will now turn off both Tolerant Machining and Undercut Handling and observe the behavior of the tool path. Choose Cutting. Note that Undercut Handling is grayed out. You can only turn off the Undercut Handling option after you have turned off the Tolerant Machining option. Turn the Tolerant Machining option off. Turn the Undercut Handling option off.
OK to accept the Cut Parameters.
Tolerant Machining and Undercut Handling Generating the Tool Path You will now generate the tool path with Tolerant Machining and Undercut Handling turned off. Generate the tool path. The shank of the tool collides with the wall..
Undercut Handling
When you use the Undercut Handling option the system applies the Horizontal Clearance (specified under Engage/Retract Method) to the shank of the tool (the portion above the flutes) unless the Horizontal Clearance is greater than the tool radius, in which case the tool radius is used. As the tool progresses deeper through the cut levels, the Horizontal Clearance will keep the shank from rubbing against the part geometry forming the undercut.
343 In this operation, the Horizontal Clearance uses the default of .100. The tool radius is .120. So the tool will be offset from the undercut face .100.
Tolerant Machining and Undercut Handling Using Undercut Handling Undercut Handling prevents the shank of the tool from rubbing against the part geometry by considering undercut geometry. The system applies the Horizontal Clearance (specified under Engage/Retract Method) to the shank of the tool to clear the undercut part geometry.
Undercut Handling applies only to non-tolerant machining (i.e., the Tolerant Machining option is toggled OFF).
Tolerant Machining and Undercut Handling Turning On Undercut Handling Choose Cutting. Turn the Undercut Handling option on.
OK to accept the Cut Parameters.
Tolerant Machining and Undercut Handling Generating the Tool Path You will now generate the tool path with only Undercut Handling turned on.
344 Generate the tool path. Notice that the tool is offset from the wall to avoid rubbing the shank of the tool on the wall.
Select OK to accept the tool path. OK to complete the operation. Close the part file.
Rest Milling Cavity Milling allows you to perform rest milling by creating an associative In-Process Workpiece (IPW) in an operation and using it as blank geometry in the next operation. It also allows you to display the previous IPW and the resultant IPW for each operation.
To use the IPW, operations must be in the correct program sequence in the MILL_GEOM or WORKPIECE geometry group. The tool path must be generated and accepted in all previous operations in the sequence before the IPW can be used in the next operation.
Rest Milling Opening the Part File The Initial IPW is defined as the Blank in the geometry parent group MILL_GEOM or WORKPIECE geometry parent group.
345 You will define the BLANK in the MILL_GEOM parent group, activate the use of the 3D IPW and generate the operation. You will use the subsequent IPW that was generated as the blank for the next operation. Open part file pln_rest_mill.prt from the pln subdirectory.
Choose Application
Manufacturing.
Display the Geometry View in the Operation Navigator and expand the objects.
Rest Milling Displaying the Part Geometry The part geometry has been defined in the WORKPIECE parent group. Double-click the WORKPIECE parent group.
With the Part icon highlighted, choose Display.
The part geometry highlights.
346
Rest Milling Defining the Blank Geometry You will define the blank geometry using a method that automatically creates a solid body enclosing the part geometry. Choose the Blank icon and Select.
Turn the Auto Block option on.
A solid body bounding the part geometry is created. The XM, YM, ZM fields allow you to modify the size of the body by specifying offsets from each face.
347
OK to accept the blank geometry with no additional offsets. OK to accept the MILL_GEOM dialog.
Rest Milling Creating a Roughing Operation You will create a roughing operation that uses the blank geometry you just defined.
Choose the Create Operation icon
from the toolbar.
Be sure the Type option is set to mill_contour and choose Cavity Mill.
Specify the following parent groups.
OK to begin creating the operation.
348
Rest Milling Generating the Tool Path Generate the Tool Path. Turn the three Display Parameter options off and OK to continue generating the tool path.
OK to complete the operation. Refresh the graphics display.
Rest Milling Creating a Semi-Finish Operation You will create a semi-finish operation that uses the IPW defined by the roughing operation as blank geometry. Choose the Create Operation icon from the toolbar. Be sure Cavity Mill is still chosen as the subtype. Specify the following parent groups.
OK to begin creating the operation.
349
Rest Milling Using the IPW as Blank Geometry in the Current Operation You will use the IPW generated by the roughing operation as the blank geometry in this operation. Choose Cutting from the CAVITY_MILL dialog. Turn the Use 3D IPW option on.
OK to accept the Cut Parameters dialog.
Rest Milling Displaying the Previous IPW The Previous IPW icon replaces the Blank icon at the top of the CAVITY_MILL dialog.
Choose the Previous IPW icon and Display. The system may require some processing time to display the faceted body. This IPW is the blank geometry that will be used by this operation.
350
Rest Milling Generating the Tool Path You will generate a tool path that semi-finishes the part. Generate the Tool Path. Turn the three Display Parameter options off and OK to continue generating the tool path.
Refresh the graphics display.
Rest Milling Displaying the Resulting IPW You will display the resulting IPW that will be passed on to the next operation. Choose the Display Resulting IPW icon.
The system may require some processing time to display the faceted body.
351
OK to complete the operation.
Rest Milling Creating a Finishing Operation You will create a finishing operation that uses the IPW defined by the semi-finish operation as blank geometry. Choose the Create Operation icon from the toolbar. Be sure Cavity Mill is still chosen as the subtype. Specify the following parent groups.
OK to begin creating the operation.
Rest Milling Using the IPW as Blank Geometry in the Current Operation You will use the IPW generated by the semi-finish operation as the blank geometry in this operation. Choose Cutting from the CAVITY_MILL dialog. Turn the Use 3D IPW option on.
352 OK to accept the Cut Parameters dialog. Key in 3.000 in the Depth Per Cut field.
Rest Milling Generating the Tool Path Generate the Tool Path. Turn the three Display Parameter options off and OK to continue generating the tool path.
Refresh the graphics display.
Rest Milling Displaying the Resulting IPW Choose the Display Resulting IPW icon at the bottom of the dialog. The system may require some processing time to display the faceted body.
OK to complete the operation.
353
Rest Milling Displaying the IPW Column in the Operation Navigator Click MB3 on the Operation Navigator background and choose Columns and Configure.
Turn the IPW option on.
OK to accept the Operation Navigator Properties dialog. The IPW column now displays in the Operation Navigator. The check marks indicate the operations that contain resulting IPW's.
354 If an new operation is inserted in the program sequence, if an operation is deleted, or if the operations are reordered, clock icons indicate that the resulting IPW's are out of date. This simply means that when generating the tool paths, the IPW's will need to be updated internally, requiring additional processing time. Remove the IPW column from the Operation Navigator. Close the part file.
Z-Level Milling Z-Level Milling is designed to profile a part at multiple cut levels using a fixed axis. It allows you to cut either the entire part or steep areas only. When the Steep Angle option is toggled on, only areas with a steepness greater than or equal to the specified Steep Angle are profiled. This allows you to profile areas left unmachined by the Area Milling Drive Method in Fixed Axis Surface Contouring.
In this lesson, you will profile the part at each cut level and then constrain the cut region using the silhouette or "shadow" of the part. You will then specify a Steep Angle to profile only the steep areas left unmachined by a previous Fixed Axis Surface Contouring operation. In addition, you will learn how to define a Cut Area and then further constrain the cut region using a trim boundary.
Profiling the Entire Part
355 You will use Z-Level Milling to profile the part. You will observe how the Trim By option can be used to profile the entire part at each cut level or to constrain the cut region by the silhouette or "shadow" of the part.
Profiling the Entire Part Opening the Part Open part file pln_zlevel_mill.prt from the pln subdirectory.
Choose Application
Manufacturing.
Profiling the Entire Part Defining the Part Geometry In the Geometry view of the Operation Navigator, expand the MCS_MILL object.
356 The WORKPIECE object does not yet define the part geometry and must be edited. Double-click on the WORKPIECE object.
This displays the MILL_GEOM dialog so you can define Part, Blank, and Check Geometry. Choose the Part icon and Select.
Select the body as the part geometry and OK to accept it.
OK in the MILL_GEOM dialog to complete the geometry definition. The WORKPIECE object defines the part geometry that will be inherited by the operations it contains.
Profiling the Entire Part Creating a Z-Level Profile Operation Choose the Create Operation icon. Change the Type to mill_contour. Choose ZLEVEL_PROFILE.
357
ZLEVEL_PROFILE and ZLEVEL_PROFILE_STEEP
You can choose either of the two subtypes outlined below to create a Zlevel Profile operation.
The ZLEVEL_PROFILE icon creates an operation with no Steep Angle, allowing the entire cut region to be profiled. The Steep angle option is turned off by default.
The ZLEVEL_PROFILE_STEEP icon creates an operation that allows only areas with a steepness greater than or equal to a specified Steep Angle to be profiled. The Steep angle option is turned on by default.
The system automatically names the operation ZLEVEL_PROFILE. Specify the following parent groups.
OK to begin creating the operation. Notice that the Select/Reselect option is blanked for defining part geometry. Part geometry is inherited from the WORKPIECE object.
358
Profiling the Entire Part Profiling the Entire Part The Trim By option can be set to None or Silhouette. None allows the tool to profile the entire part geometry by generating a trace at each cut level. Choose Cutting. Choose None as the Trim By option and OK.
Notice that the Steep Angle option is turned off.
The off condition allows the entire cut region to be profiled regardless of the steepness of the surface being cut.
Profiling the Entire Part Generating the Tool Path You will generate a tool path that profiles the entire part. Generate the tool path. Turn the Pause After Display option off and OK to continue generating the tool path.
The entire part is profiled at each cut level.
359
Profiling the Entire Part Profiling the Silhouette Now you will constrain the cut region using the silhouette or "shadow" of the part. Choose Cutting. When the Trim By option is set to Silhouette, the cut region is constrained by the silhouette or "shadow" of the part projected along the tool axis. The tool profiles outward until it reaches the silhouette of the part geometry where a single profiling cut is then generated along the outer edge.
Choose Silhouette as the Trim By option and OK.
Refresh the graphics display.
Profiling the Entire Part Generating the Tool Path You will generate a tool path that is trimmed by the silhouette of the part. Generate the tool path. Turn the Pause After Display option off and OK to continue generating the tool path. The tool path is generated with only a single pass at the silhouette.
360
OK to complete the operation. Close the part file.
Profiling Only Steep Areas An important feature of Z-Level Milling is the ability to specify a Steep Angle to distinguish steep from non-steep areas. This allows you to profile only the steep areas left unmachined by previous Fixed Axis Surface Contouring operations. When the Steep Angle option is turned on, only areas with a steepness greater than the specified Steep Angle are profiled. The steepness of the part at any given point is defined by the angle between the tool axis and the normal of the face.
361
Profiling Only Steep Areas Opening the Part Open part file pln_zlevel_mill_1.prt from the pln subdirectory.
Choose Application
Manufacturing.
In the Program Order view of the Operation Navigator, expand the PROGRAM object to display the two operations.
Notice that the ZLEVEL_PROFILE operation follows the CONTOUR_AREA operation in the program sequence. You will examine the CONTOUR_AREA operation first and then observe how the subsequent ZLEVEL_PROFILE operation profiles the unfinished steep areas.
Profiling Only Steep Areas Displaying the Part Geometry Double-click on the CONTOUR_AREA icon to edit the operation.
Notice that the Select/Reselect option is blanked, indicating that the part geometry is inherited from the WORKPIECE object.
362
Choose Display to highlight the part geometry. The part geometry is defined by a surface region.
Profiling Only Steep Areas Replaying the Tool Path Replay the tool path. This operation uses the Area Milling Drive Method to restrict the allowable steepness of the tool path. Notice that the very "steep" areas are not machined. This restriction is necessary when using a zig-zag cut pattern to prevent the tool from plunging directly down into the part material.
Profiling Only Steep Areas Examining the Steep Angle Choose Area Milling under Drive Method.
363
In the Area Milling Method dialog, notice that the Steep Containment is specified as Nonsteep and the Steep Angle is specified as 70 degrees. This allows only areas where the tool path is less than or equal to 70 degrees to be machined by this operation. The steepness of the part at any given point is defined by the angle between the tool axis and the normal of the face.
Cancel twice to exit the operation.
Profiling Only Steep Areas Specifying the Steep Angle in the Second Operation Now you will edit the ZLEVEL_PROFILE operation so that it profiles the steep areas left uncut by the CONTOUR_AREA operation. Double-click on ZLEVEL_PROFILE.
The ZLEVEL_PROFILE dialog displays. Turn the Steep Angle option on and key in 70.
364
This will allow only the areas with a steepness greater than or equal to 70 degrees to be profiled.
Profiling Only Steep Areas Generating the Tool Path Generate the tool path.
By comparing the tool paths, you will notice that the entire part is machined by the two operations. The CONTOUR_AREA operation zig-zags the areas where the steepness is less than or equal to 70 degrees. The ZLEVEL_PROFILE operation profiles the areas where the steepness is greater than or equal to 70 degrees.
OK to complete the operation. Close the part file.
365
Specifying the Cut Order Unlike Cavity Milling which orders cut traces by cut region, Z-Level Milling orders cut traces by shape. You may profile shapes by Depth First in which case one shape (an island, for example) is completely profiled before profiling the next shape as illustrated below, or you may profile shapes by Level First in which case all shapes are profiled at a particular level before cutting the next level.
Specifying the Cut Order Opening the Part Open part file pln_zlevel_mill_2.prt from the pln subdirectory. Choose Application
Manufacturing.
366
In the Geometry view of the Operation Navigator, expand the MCS_MILL object and the WORKPIECE object to display the ZLEVEL_PROFILE operation. Double-click on ZLEVEL_PROFILE to edit the operation.
Specifying the Cut Order Displaying the Part Geometry With the Part icon chosen, choose Display to highlight the part geometry.
The entire solid model highlights indicating that it has been defined as the part geometry.
367
Specifying the Cut Order Examining the Cut Order Notice that the Cut Order is currently set to Depth First. This causes the operation to completely finish profiling one shape (island in this example) before profiling the next shape.
Refresh the graphics display. Replay the tool path. The island on the left is completely profiled before profiling the island on the right.
368
Specifying the Cut Order Respecifying the Cut Order Change the Cut Order to Level First.
This option profiles all shapes (islands) at a given level before profiling the next level. Refresh the display.
Specifying the Cut Order Generating the Tool Path Choose Edit Display.
Turn the Pause After Display option on and OK the dialog. Generate the tool path. The first level cut on the left island displays.
OK the Display Parameters dialog. The first cut level on the right island displays.
369
OK as necessary to complete the tool path. Notice how the islands are cut alternately. OK the ZLEVEL_PROFILE dialog to complete the operation.
Specifying a Cut Area Unless otherwise specified, the system uses the entire defined part geometry (excluding areas not accessible by the tool) as the cut area. You can specify cut areas by selecting Surface Regions, Sheet Bodies, or Faces.
Specifying a Cut Area Specifying a Surface Region as the Cut Area Double-click on ZLEVEL_PROFILE.
370
The ZLEVEL_PROFILE dialog displays. Choose Cut Area, then Select.
In the Cut Area dialog, choose Features.
This will allow you to select surface regions (and only surface regions) to define the cut area. You may not mix features and geometry when defining a cut area. Select the surface region illustrated below and OK.
Specifying a Cut Area Generating the Tool Path Generate the tool path.
371 The Display Parameters dialog displays. Turn the Pause After Display option off and OK the dialog. The tool path is generated and restricted to the feature you selected.
Specifying a Trim Boundary A Trim boundary allows you to further constrain the cut regions. You may define the area of the cut regions to exclude from the operation by specifying the Trim Side as Inside or Outside. Trim boundaries are always closed and use an On condition.
372
Specifying a Trim Boundary Specifying a Trim Boundary Using Control Points Choose Trim, then Select.
In the Trim Boundary dialog, choose Outside as the Trim Side.
This will exclude all portions of the cut region falling outside of the trim boundary. Choose Point Boundary as the Filter Type and Control Point as the Point Method.
This will allow you to create the trim boundary by specifying a sequence of points. Specify the four control points in order as illustrated below and OK to accept them.
373 Choose Display (in the Geometry section of the dialog) to display the trim boundary.
Specifying a Trim Boundary Generating the Tool Path Generate the tool path. Turn off the Pause After Display option and OK the dialog. The tool path is generated within the trim boundary and restricted to the cut region you defined earlier.
Notice that the cutter retracts, traverses, and engages between each cut level. A more effecient cut pattern would be to allow the cutter to remain in contact with the part between cut levels. Refresh the graphics display.
374
Specifying a Cut Pattern for High Speed Machining Cut patterns for high speed machining must allow constant volume removal and eliminate burying the cutter into material. They must also provide a smooth transition from level to level as the cutter progresses downward or upward along the path, eliminating constant retracting, traversing, and engaging. To maximize volume removal, the tool should always be in contact with the part.
Specifying a Cut Pattern for High Speed Machining Specifying the Cut Pattern Choose Cutting. Set the Cut Direction option to Mixed and the Level to Level option to Direct on Part.
OK to accept the Cut Parameters.
Specifying a Cut Pattern for High Speed Machining Generating the Tool Path Generate the tool path. Turn off the Pause After Display option and OK the dialog.
375
Notice how the cutting tool engages the part, feeds down the wall of the part to get to the next level, and alternates the direction of cut from one level to the next. OK to complete the operation. Close the part file.
Specifying a Cut Pattern for High Speed Machining Another Example of High Speed Machining Open part file pln_zlevel_mill_4.prt from the pln subdirectory. Choose Application
Manufacturing.
Double-click on the ZLEVEL_PROFILE icon in the Operation Navigator to edit the operation.
Replay the tool path.
376 Choose Cutting. Set the Cut Direction option to Mixed and the Level to Level option to Direct on Part as you did before and OK to accept the cut parameters. Generate the tool path. Notice the reduction in engage, traverse, and retract moves.
OK to complete the operation. Close the part file.
Specifying a Merge Distance The Merge Distance option enables you to eliminate small discontinuities or unwanted gaps in the tool path by connecting disjointed cutting motions. The value you enter determines the distance the tool will span to connect the end points of cutting moves.
377
Specifying a Merge Distance Opening the Part Open part file pln_zlevel_mill_3.prt from the pln subdirectory.
Notice the two 4.0 mm slots cut into the part. The Merge Distance option determines whether the tool will retract or continue profiling when it reaches the slots.
Choose Application
Manufacturing.
Expand the objects in the Geometry view of the Operation Navigator.
Specifying a Merge Distance Specifying the Merge Distance Double-click on the ZLEVEL_PROFILE icon to edit the operation.
The ZLEVEL_PROFILE dialog displays. Notice that the Merge Distance is currently set to 3.0000.
378
Because this value is smaller than the width of the slots, the tool will not profile across the slots and will instead retract each time it encounters them. Replay the tool path.
Change the Merge Distance to 5.0000.
Now that the Merge Distance is greater than the width of the slots, the tool path will connect the disjointed cutting motions and cut across the slots.
Specifying a Merge Distance Generating the Tool Path Generate the tool path.
379
Notice that the tool does not retract, but instead cuts directly across the slots. OK to complete the operation. Close the part file.
Planar and Cavity Milling Project This English units part contains several cavities that are machined from a solid block of material. The completed machining program consists of six operations that rough, semi-finish, and finish the part. You will create three of the operations.
To complete this project, you should be familiar with the following operation subtypes. CONTOUR_AREA_NON-STEEP CONTOUR_ZIGZAG
380 CONTOUR_AREA_DIR_STEEP In addition, you should know how to use Verify Toolpath to graphically simulate material removal and compare the in-process workpiece to the part.
Functions Used to Machine the Part In this project you will: Create a ZLEVEL_FOLLOW_CAVITY operation to rough the part.
Create a ZLEVEL_PROFILE_STEEP operation to semi-finish the steep areas.
Create a FACE_MILLING operation that uses a manual cut pattern to finish the top face.
381
Use Verify Toolpath to graphically simulate material removal for the entire program.
Compare the in-process workpiece to the part by displaying the excess material.
Machining the Part
382 The completed program must cut the finished part from a solid block of material using a sequence of roughing, semi-finishing, and finishing operations while applying acceptable standard machining techniques.
Machining the Part Open the Part File Open part file pln_proj_1.prt from the pln subdirectory. Enter the Manufacturing Application. Fully expand the objects in the Program Order View of the Operation Navigator. Choose the Program Order View icon in the toolbar. In the Operation Navigator, click on the plus (+) sign next to the PROGRAM object. Replay the three operations. In the Operation Navigator, click on the PROGRAM icon and MB3
Replay.
These Fixed Axis Surface Contouring operations semi-finish and finish the part. You will create three more operations that rough out the initial material, semi-finish the non-steep areas, and finish the top face of the part, and then place them in the correct program sequence as illustrated below.
383
Machining the Part Creating a ZLEVEL_FOLLOW_CAVITY Operation You first need to create an operation that roughs out the initial material.
Begin a ZLEVEL_FOLLOW_CAVITY operation using the following parent groups: Choose the Create Operation icon. Choose mill_contour as the Type Choose the ZLEVEL_FOLLOW_CAVITY icon as the subtype. Specify the parent groups as indicated below.
OK to begin creating the operation.
Machining the Part Displaying the Part and Blank Geometry You need to visually verify the part and blank geometry the operation will use. Display the part geometry. Under Geometry, choose the Part icon and Display.
384
The part geometry is inherited from the WORKPIECE object. Refresh the graphics display. Display the blank geometry. Under Geometry, choose the Blank icon and Display.
The blank geometry is also inherited from the WORKPIECE object. Refresh the graphics display.
Machining the Part Specifying the Depth Per Cut and Range Depth You need to reduce the Depth Per Cut and specify the Range Depth. Specify a Depth Per Cut of 0.1500. Key in 0.1500 for the Depth Per Cut.
385
Specify the bottom of one of the cavities as the Range Depth. Under Control Geometry, choose Cut Levels. Select the bottom face of any one of the four cavities.
OK to accept the cut levels.
Machining the Part Generating the Tool Path You need to generate the tool path to see if the operation cuts the part correctly. Generate the tool path. Choose the Generate icon. Turn the Pause After Display option off. OK the Display Parameters dialog.
Notice that the tool path finishes each cut level by traversing from one region to the next before beginning the next cut level.
386
In this case, it would be more efficient to completely finish machining each region from top to bottom before traversing to the next region.
Machining the Part Specifying the Cut Order You need to specify a cut order that will machine the cavities more efficiently. Specify Depth First as the Cut Order. Choose Cutting. Choose Depth First as the Cut Order.
This option will cut each pocket to full depth, as encountered. OK to accept the cut parameters.
Machining the Part Generating the Tool Path You need to generate the tool path to see if the operation cuts the part correctly. Generate the tool path. Choose the Generate icon. Turn the Pause After Display option off. Turn the Display Cut Regions option off. OK the Display Parameters dialog.
387 Notice that the tool path completely machines each region from top to bottom before traversing to the next one.
OK to complete the operation. Notice that the operation is at the end of the program.
Machining the Part Reordering the Operations The operation you just created needs to be moved to the beginning of the program. Reorder the operations so that ZLEVEL_FOLLOW_CAVITY is at the beginning of the program. In the Program Order View, choose the CONTOUR_AREA_NON_STEEP, CONTOUR_AREA, and FLOWCUT_SINGLE operations. You will need to hold down the Ctrl key to choose all three operations. Choose MB3 Cut.
388
The operation you choose in the next step is the object below which the pasted operations will appear. Choose ZLEVEL_FOLLOW_CAVITY and MB3
Paste.
The operations should appear in the order illustrated below.
Machining the Part Creating a ZLEVEL_PROFILE_STEEP Operation You need to create an operation that semi-finishes the steep areas.
389
Begin a ZLEVEL_PROFILE_STEEP operation using the following parent groups: Choose the Create Operation icon. Choose mill_contour as the Type. Choose the ZLEVEL_PROFILE_STEEP icon as the subtype. Specify the parent groups as indicated below.
OK to begin creating the operation.
Machining the Part Displaying the Cut Area You need to visually verify the cut areas. Display the cut area geometry. Under Geometry, choose the Cut Area icon and Display.
390
Each cavity is a separate cut area. The cut area geometry is inherited from the Mill_AREA object. Refresh the graphics display.
Machining the Part Specifying the Steep Angle Specify a Steep Angle of 55.0000 degrees. Key in 55.0000 for the Steep Angle.
This will allow only the areas with a steepness greater than or equal to 55 degrees to be profiled.
Machining the Part Specifying the Depth Per Cut and Cut Levels You need to reduce the Depth Per Cut and specify the Range Depth. Specify a Depth Per Cut of 0.1000. Key in 0.1000 for the Depth Per Cut.
391
Machining the Part Verifying the Range Depth Verify that the Range Depth is the depth of the cavities. Under Control Geometry, choose Cut Levels.
The current Range Depth is defined by the depth of the Cut Area geometry and should be 1.0000.
OK to accept the cut levels.
Machining the Part Generating the Tool Path You need to generate the tool path to see if the operation cuts the part correctly. Generate the tool path. Choose the Generate icon. Turn all of the display parameters off. OK the Display Parameters dialog.
Notice that the tool path completely machines each region from top to bottom before traversing to the next one. Only the steep areas are machined.
392
OK to complete the operation. Notice that the operation is at the end of the program.
Machining the Part Reordering the Operations The operation you just created needs to be moved to a different position in the program. Move the ZLEVEL_PROFILE_STEEP operation to the third position in the program In the Program Order View, choose the ZLEVEL_PROFILE_STEEP operation. Choose MB3 Cut.
The operation you choose in the next step is the object below which the pasted operation will appear.
393 Choose CONTOUR_AREA_NON_STEEP and MB3
Paste.
The operations should appear in the order illustrated below.
Machining the Part Displaying Material Removal You need to visualize the tool path for the entire program and compare the in-process workpiece to the part. Use dynamic material removal to visualize the tool path for the entire program. In the Program Order View of the Operation Navigator, click on the PROGRAM icon. Choose the Verify Toolpath icon in the toolbar. Choose the Dynamic tab. Choose the Play Forward icon.
394
Compare the in-process workpiece to the part. Choose Compare in the Toolpath Visualization dialog.
Notice that large scallops remain on the top face of the part. Next, you will create a face milling operation that that uses a manual cut pattern to finish the top face. Cancel to dismiss the Toolpath Visualization dialog.
Machining the Part Creating a FACE_MILLING Operation You need to create an operation that uses a manual cut pattern to finish the top face of the part.
395
Begin a FACE_MILLING operation using the following parent groups: Choose the Create Operation icon. Choose mill_planar as the Type. Choose the FACE_MILLING icon as the subtype. Specify the parent groups as indicated below.
OK to begin creating the operation.
Machining the Part Specifying the Face Geometry You need to specify the face the operation will finish. Select the top of the part as the face to finish. Under Geometry, choose the Face icon and Select. Select the top face of the part. OK to accept the face geometry.
396
Machining the Part Specifying a Top View You need to change to a top view so you can see the manual cut pattern clearly. Replace the current view with a top view. MB3
Replace View
TOP.
Machining the Part Specifying the Tool Path Display You need to specify a 2-D silhouette tool path display so you can clearly see the area the tool cuts.
397 Specify a 2-D Tool display and a Silhouette Path Display. Choose the Edit Display icon under Tool Path. Choose 2-D for the Tool Display and Silhouette for the Path Display.
OK to accept the Display Options.
Machining the Part Specifying a Manual Cut Pattern You need to specify a manual cut pattern to cut along the top of the walls. Specify that you wish to begin defining a manual cut pattern. Choose Mixed as the Cut Method.
Choose the Generate icon. In the Mixed Cut Pattern dialog, be sure Manual is chosen as the Cut Method.
OK to begin defining the cut pattern.
The Create Manual Cut Pattern dialog should be displayed.
Machining the Part Repositioning to a Point Reposition the tool to a point in space just to the right of the corner of the part as illustrated below.
398 Be sure the Reposition to Point icon is chosen. Choose Cursor Location as the Point Method. Indicate a point in space to the right of the corner of the part.
Machining the Part Engaging to a Point Engage the tool to the corner of the part. Choose Move To Point.
Choose End Point as the Point Method. Choose Engage as the Motion Type.
Select the corner of the part as the engage point.
399
Machining the Part Cutting to a Sequence of Points Create four linear cuts along the periphery of the top face as illustrated below. Choose Cut as the Motion Type.
Select the four end points in order as illustrated below to define the sequence of linear cutting moves.
400
Machining the Part Repositioning to a Point Reposition the tool to a point in space just off to one side of the part as illustrated below. Choose Reposition To Point.
Choose Cursor Location as the Point Method. Indicate near the center of the side of the part.
Machining the Part Engaging to a Point Engage the tool to the center of the side of the part. Choose Move To Point. Choose Control Point as the Point Method. Choose Engage as the Motion Type. Select the center of the line as the engage point.
401
Machining the Part Cutting to a Point Cut across the center of the part to a point on the opposite side. Choose Cut as the Motion Type. Select the center of the line on the opposite side of the part.
Machining the Part Repositioning to a Point Reposition the tool to a point in space just off to one side of the part as illustrated below. Choose Reposition To Point.
402 Choose Cursor Location as the Point Method. Indicate near the center of the side of the part.
Machining the Part Engaging to a Point Engage the tool to the center of the side of the part. Choose Move To Point. Choose Control Point as the Point Method. Choose Engage as the Motion Type. Select the center of the line as the engage point.
403
Machining the Part Cutting to a Point Cut across the center of the part to a point on the opposite side. Choose Cut as the Motion Type. Select the center of the line on the opposite side of the part as illustrated below.
OK to complete the manual cut pattern.
Machining the Part Replaying the Tool Path Replace the current view with a TFR-ISO view. MB3
Replace View
Replay the tool path.
TFR-ISO.
404
OK to complete the operation.
Machining the Part Displaying Material Removal You need to visualize the tool path for the entire program and compare the in-process workpiece to the part. Use dynamic material removal to visualize the tool path for the entire program. In the Program Order View of the Operation Navigator, click on the PROGRAM icon. Choose the Verify Toolpath icon in the toolbar. Choose the Dynamic tab. Choose the Play Forward icon.
Compare the in-process workpiece to the part. Choose Compare in the Toolpath Visualization dialog.
Notice that the scallops have been removed from the top of the part.
405
Cancel to dismiss the Toolpath Visualization dialog. Close the part file.
406
SURFACE CONTOURING Area Milling Drive Method The Area Milling drive method generates a fixed axis surface contouring tool path by specifying a cut area and, if desired, adding steep containment and trim boundary constraints. Cut areas may be defined by selecting surface regions, sheet bodies, or faces. You can restrict cut areas based on the steepness of the tool path. By cutting non-steep areas and then profiling steep areas, you can avoid plunging the tool directly into the material along vertical walls.
Steep areas can be profiled with a subsequent Z-Level Milling operation or a Surface Contouring operation that uses a Directional Steep containment. The Area Milling drive method is similar to the Boundary drive method but has no drive geometry and uses a more robust and automated computation of collision-free containment. For these reasons, you should use the Area Milling drive method in place of the Boundary drive method whenever possible. In this lesson, you will create several fixed axis surface contouring operations using the Area Milling drive method. You will see how the Area Milling drive method works together with Z-Level Milling operations to machine both steep and non-steep areas of a cavity and a core. You will also learn to graphically simulate material removal using a shaded image and display areas where excess material remains.
Machining a Cavity
407 You will first examine a program that consists of three milling operations and observe how these three operations work together to machine the entire cavity.
Machining a Cavity Opening the Part Open part file srf_area_mill_1.prt from the srf subdirectory. Choose the Shaded icon
in the toolbar so you can clearly see the contoured surfaces.
Notice that the sides of the cavity are very steep (vertical or nearly vertical).
Choose the Visible Hidden Edges icon
to return to a wireframe display.
Machining a Cavity Entering the Manufacturing Application Choose Application
Manufacturing.
In the Geometry View of the Operation Navigator, choose Expand All expand the objects as illustrated below.
to fully
408
The operations inherit parameters from the MILL_GEOM and MILL_ORIENT parent groups.
Machining a Cavity Examining the MILL_GEOM Group The MILL_GEOM parent group defines the part geometry used by all three operations. Double-click on the MILL_GEOM icon.
Choose the Part icon and Display.
The part geometry highlights.
409 Refresh the graphics display. Cancel out of the MILL_GEOM dialog.
Machining a Cavity Replaying the Cavity Mill Tool Path Choose the Program Order View
icon in the toolbar.
The CAVITY_MILL operation first roughs out the cavity. The CONTOUR_AREA_NON_STEEP and ZLEVEL_PROFILE_STEEP operations then finish the cavity. Double-click on the CAVITY_MILL operation to display the CAVITY_MILL dialog.
Choose Replay.
Machining a Cavity Visualizing Material Removal for the Cavity Mill Operation The Verify option allows you to graphically simulate material removal using a shaded image. This function requires blank material to be defined. If it is not already defined in the Workpiece group or within the operation, it can be temporarily defined for display purposes when performing the tool path visualization.
410
Choose the Verify icon
at the bottom of the dialog.
Choose the Dynamic tab.
Choose the Play Forward icon. Be sure Auto Block is chosen as the Blank Type.
Auto Block creates a solid body bounding the part geometry with faces parallel to the WCS. Offsets can be added to each of the six faces by entering values in the dialog or by dragging the handles. OK to begin the tool path visualization.
The roughing operation leaves large scallops for the subsequent finishing operations to remove. OK to complete the tool path visualization. OK to complete the operation.
Machining a Cavity Replaying the Non-Steep Tool Path Double-click on the CONTOUR_AREA_NON_STEEP icon in the Operation Navigator
411 to display the operation dialog. Replay
the operation.
Notice that the tool does not cut all the way to the edge of the cavity. The Steep Containment parameters restrict the cut area, allowing the tool to cut from side to side but preventing it from cutting downward and plunging directly into the material.
Machining a Cavity Visualizing Material Removal for the Non-Steep Operation Choose the Verify
icon at the bottom of the dialog.
Choose the Dynamic tab. Choose the Play Forward icon. Be sure Auto Block is chosen as the Blank Type. OK to begin the tool path visualization.
OK to complete the tool path visualization. OK to complete the operation.
412
Machining a Cavity Replaying the Steep Tool Path Double-click on the ZLEVEL_PROFILE_STEEP operation.
Replay the operation. This operation profiles the steep areas left uncut by the surface contouring operation.
Machining a Cavity Visualizing Material Removal for the Steep Operation Choose the Verify icon at the bottom of the dialog. Choose the Dynamic tab. Choose the Play Forward icon. Be sure Auto Block is chosen as the Blank Type. OK to begin the tool path visualization.
413
Material removal is displayed for ZLEVEL_PROFILE_STEEP. OK to complete the tool path visualization. OK to complete the operation. Close the part file.
Cutting Non-Steep Areas You will create a fixed axis surface contouring operation that uses the Area Milling drive method to cut only the non-steep areas of a cavity.
Cutting Non-Steep Areas Opening the Part Open part file srf_area_mill_2.prt from the srf subdirectory. Choose Application
Manufacturing.
414
In the Geometry View of the Operation Navigator, expand the objects. This program contains a MILL_GEOM group that defines part and blank geometry and a CAVITY_MILL operation that roughs out the cavity.
Cutting Non-Steep Areas Creating the Operation Choose the Create Operation icon. Choose mill_contour as the Type. The Type determines the subtype icons that are available and the groups that are initially available to choose from in the dialog. You can use any one of the subtypes outlined below to create a fixed axis surface contouring operation. Choose CONTOUR_AREA_NON_STEEP as the subtype.
This subtype defines most of the operation parameters you will need to cut non-steep areas. The system automatically names the operation CONTOUR_AREA_NON_STEEP. Specify the following groups in the Create Operation dialog.
415
The operation will inherit the parameters defined by these parent groups. OK to begin creating the operation.
Cutting Non-Steep Areas Displaying the Part Geometry Notice that the Select/Reselect option is blanked for defining part geometry. Part geometry has already been defined and is inherited from the MILL_GEOM group. It can only be modified by editing the group.
Choose Display to highlight the part geometry. The part geometry is defined as the entire body. Refresh the display. Notice that the Drive Method defaults to Area Milling.
The CONTOUR_AREA_NON_STEEP subtype that you chose earlier determined this option as the default.
Cutting Non-Steep Areas Defining the Cut Area The cut area defines the area of the part the operation considers for cutting when generating the tool path. If you do not specify a cut area, the system uses the entire Part Geometry as the cut area.
416 Choose the Cut Area icon and Select.
The Selection Options should be set by default to Geometry and Faces.
Select the face defining the cavity as illustrated below.
OK to accept the face as the cut area.
Cutting Non-Steep Areas Specifying Non-Steep Containment The Non-Steep option enables you to generate only cuts that are less than or equal to the specified Steep Angle. This allows the tool to cut from side to side while preventing it from plunging into the material along the vertical walls. Choose Area Milling under Drive Method.
417
Notice that the Steep Containment parameters default to non-steep with a steep angle of 65.0000 degrees. The CONTOUR_AREA_NON_STEEP subtype you chose earlier determined these as the defaults. Key in 55 for the Steep Angle.
The operation will now cut only the areas where the steepness of the tool path is less than or equal to 55 degrees.
OK to accept the steep containment and return to the operation dialog.
Cutting Non-Steep Areas Generating the Tool Path You will generate the tool path and observe how the Cut Area and Steep Containment parameters influence the tool path. Generate the tool path. Only non-steep tool paths (those between 0-55 degrees) are generated.
418
Notice, however, that the operation also creates small zig-zag cuts along the edge of the cavity.
These small zig-zag cuts are non-steep tool paths that occur as a result of edge tracing. Edge tracing occurs when the tool "rolls over" the edge of the cut area. The steepness of these edge traces falls within the specified 0-55 degree Steep Angle as illustrated below.
Edge traces are generally undesirable and should be removed.
419
Cutting Non-Steep Areas Removing Edge Traces Choose Cutting. Turn Remove Edge Traces On.
OK to accept the cutting parameters.
Cutting Non-Steep Areas Generating the Tool Path You will generate the tool path and observe how the edge traces have been removed. Generate the new tool path.
OK to complete the operation. The CONTOUR_AREA_NON_STEEP operation now appears as the second operation in the Program Order View of the Operation Navigator.
The Program Order View determines the order in which operations will be executed on the machine tool.
420
Creating a Z-Level Profile Operation You will create a Z-Level Milling operation that profiles the steep areas left uncut by the previous Area Milling operation.
For additional information on creating Z-Level Milling operations, refer to the Z-Level Milling lesson in the Planar and Cavity Milling course.
Creating a Z-Level Profile Operation Creating the Operation Choose the Create Operation icon Choose ZLEVEL_PROFILE_STEEP
in the toolbar. as the subtype.
This subtype defines most of the operation parameters you will need to cut steep areas. The system automatically names the operation ZLEVEL_PROFILE_STEEP. Specify the following groups in the Create Operation dialog.
The operation will inherit the parameters defined in these groups. OK to begin creating the operation.
421
Creating a Z-Level Profile Operation Defining the Cut Area The cut area defines the area of the part the operation considers for cutting when generating the tool path. Choose the Cut Area icon and Select.
The Selection Options should be set by default to Geometry and Faces.
Select the three faces defining the cavity as illustrated below.
OK to accept the faces as the cut area.
Creating a Z-Level Profile Operation Defining the Steep Angle
422 The Steep Angle determines which portions of the Cut area will be machined based on the steepness of the area. Notice that the Steep Angle option has already been turned on. The ZLEVEL_PROFILE_STEEP subtype you chose earlier determined this as the default. Key in 55 for the Steep Angle.
This will allow only the areas with a steepness greater than or equal to 55 degrees to be profiled. In other words, all the steep areas left uncut by the previous Area Milling operation will now be profiled. Choose Cut Levels. Key in 0.0500 in the Depth per Cut field.
This determines the depth of each profile cut. OK to accept the cut levels.
Creating a Z-Level Profile Operation Generating the Tool Path You will generate the tool path and observe how only the steep areas are profiled. Generate the tool path. Turn off all of the Display Parameters options and OK.
OK to complete the operation.
423 The ZLEVEL_PROFILE_STEEP operation now appears as the third operation in the Program Order View of the Operation Navigator.
By comparing the Contour Area Non-Steep tool path and the Z-Level Profile Steep tool path, you can see that the two operations finish the entire cavity.
Using a Trim Boundary You will create a fixed axis surface contouring operation that uses a Trim boundary to constrain the cut area and define additional finishing passes within a specific area.
You will copy and paste an existing operation and then edit the parameters.
Using a Trim Boundary Copying an Existing Operation
424 This operation uses many of the same parameters as the existing CONTOUR_AREA_NON_STEEP operation. It will be easier to copy and modify the existing operation than to create a new operation. In the Program Order View of the Operation Navigator, highlight CONTOUR_AREA_NON_STEEP and MB3 Copy.
Highlight ZLEVEL_PROFILE_STEEP and MB3
Paste.
CONTOUR_AREA_NON_STEEP_COPY now appears as the last operation in the Program Order View.
Using a Trim Boundary Reselecting the Tool Double-click on CONTOUR_AREA_NON_STEEP_COPY to edit the operation.
First, you will change to a smaller tool. Choose the Groups tab.
425 With Tool:T2 chosen, choose Reselect.
Choose T3 in the Reselect Tool dialog and OK.
The dialog now displays T3 as the tool the operation will use. Choose the Main tab.
Using a Trim Boundary Editing the Steep Angle and Stepover Choose Area Milling under Drive method.
Key in 85 for the Steep Angle.
Key in 25 for the Stepover Percent.
Decreasing the stepover size will reduce the scallop height on the machined part. OK to accept the changes.
Using a Trim Boundary
426
Defining a Trim Boundary You will define a Trim boundary to constrain the cut area. To assist you in defining the boundary, you will display four points that are hidden on Layer 6. Choose Format
Layer Settings from the menu bar.
Highlight 6 in the Layer/Status list box and choose Selectable. OK to accept the layer settings. Four points should be displayed.
Choose the Trim icon
and Select.
The Trim Boundary dialog displays. Notice that Outside is specified as the Trim Side. This will exclude all areas of the cut region outside of the boundary. The tool path will only be created inside of the boundary. Choose the Point Boundary icon and Existing Point as the Point Method. Select the four points in order as illustrated below.
OK to complete the boundary.
427 Choose Display to verify that the boundary has been created correctly.
Trim boundaries are always Closed and always use an On condition.
Using a Trim Boundary Generating the Tool Path You will generate the tool path and observe how the Trim boundary constrains the cut area. Generate the tool path.
OK to complete the operation.
Using a Trim Boundary Visualizing Material Removal You will use Verify Toolpath to graphically simulate material removal for the entire program. In the Program Order View of the Operation Navigator, highlight NC_PROGRAM.
428
Choose the Verify Toolpath icon
on the Manufacturing Operations toolbar.
Choose the Dynamic tab. Choose Play Forward.
The material removed by each successive operation is displayed in a contrasting color. OK to complete the tool path visualization. Close the part file.
Using a Tool Holder The Area Milling and Flow Cut drive methods allow you to define a simple tool holder to ensure a collision free tool path. You will first replay a fixed contour operation that uses the Area Milling drive method to see how closely a tool without a holder cuts to the check geometry. Check geometry can be anything that you would want the tool to avoid. In this case, imagine it to be a clamp holding the part to be machined.
429
You will then create a tool with a holder and observe how the system alters the tool path to avoid collision between the tool holder and check geometry.
Using a Tool Holder Opening the Part File Open part file srf_area_mill_3.prt from the srf subdirectory. Choose Application
Manufacturing.
Display the Machine Tool View of the Operation Navigator and expand the objects.
Using a Tool Holder Replaying the Tool Path You will replay the fixed contour operation to see how closely the tool without a tool holder cuts to the check geometry.
430 In the Machine Tool View of the Operation Navigator, highlight the FIXED_CONTOUR operation.
Choose the Verify Toolpath icon
in the toolbar.
The Toolpath Visualization dialog displays with the Replay tab chosen. Choose the Play Forward icon. The operation uses a tool without a holder. Notice how closely the tool cuts to the check geometry.
OK to complete the tool path visualization.
Using a Tool Holder Creating the Tool You will create a tool with a holder.
Choose the Create Tool icon
.
Be sure mill_contour is specified as the Type. This is important because not all Types allow you to create a tool with a holder. Choose MILL_WITH_HOLDER as the subtype.
431
OK to begin defining the tool.
Using a Tool Holder Defining the Tool and the Holder You will specify parameters that define the tool and the holder. Fill in the values specified below to define the tool.
Fill in the values specified below to define the holder.
OK to accept the parameters and create the tool with the holder.
432
Using a Tool Holder Applying the Tool to the Operation You will now apply this tool to the operation. Double-click on FIXED_CONTOUR to edit the operation.
Choose Tool:MILL and Reselect.
Choose MILL_WITH_HOLDER in the Reselect Tool dialog and OK.
Using a Tool Holder Using the Holder With the Tool In order for the operation to recognize the holder, the Use Tool Holder option must be turned on. Choose Cutting. Check Safe Clearance defines an extended safety zone for check geometry which cannot be violated by the tool or the tool holder. Key in .01 for Check Safe Clearance.
433
Turn Use Tool Holder on.
OK to accept the Cutting Parameters and return to the FIXED_CONTOUR dialog.
Using a Tool Holder Generating the Tool Path You will generate the tool path and observe how the system alters the tool path to avoid collision between the tool holder and check geometry Generate the tool path.
The system has altered the tool path to avoid collision with the tool holder and the check geometry. Notice the Tool holder Collision Warning.
OK to dismiss the warning.
Using a Tool Holder Visualizing the Tool Holder Choose the Verify icon at the bottom of the dialog.
434 The Toolpath Visualization dialog displays with the Replay tab chosen. Choose the Play Forward icon.
OK to complete the tool path visualization. OK to complete the operation.
Using a Tool Holder Retrieving Tools From a Library The Retrieve Tool option allows you to retrieve tools from a library based on search criteria. Once retrieved, the tool groups appear in the Machine Tool View of the Operation Navigator and become available for selection when defining operations.
Choose the Create Tool icon Choose the Retrieve Tool icon
in the toolbar. and OK.
This displays the Library Class Selection dialog. Expand the Milling tools and choose End Mill (non indexable).
OK to accept the selection.
435
Using a Tool Holder Specifying Search Criteria The Search Criteria Dialog allows you to narrow down the library search by specifying parameters. Choose Count Matches.
Notice that the number "64" appears next to the option. This indicates there are sixty-four tools in the library that match the parameters you have specified so far. You can narrow the search even further by specifying exact numeric values or a range of values using <, >, <=, and >= signs. Key in .50 for the Diameter. Choose Count Matches. Notice that the number "7" now appears next to the option. You have narrowed the search to only those tools in the library with a diameter of .50. Choose Result Info. This displays an Information listing of all the tools matching the search criteria. It will allow you to determine which values (Flute Length and Corner Radius for example) can be specified to continue narrowing the list. Dismiss the Information window. Key in the following expressions.
The >1 means that the flute length should be greater than 1 inch long and the >=.05 means that the corner radius should be greater than or equal to 0.05. Choose Count Matches.
436 Notice that the number "3" now appears next to the option. You have narrowed the search to the only three tools in the library with a flute length greater than 1 and a corner radius greater than or equal to .05 . OK to accept the search criteria.
Using a Tool Holder Choosing Tools The Search Result listing allows you to choose the desired tool or tools. Each tool you choose will create a separate tool group. Choose the tools from the list indicated below. Use the left mouse button to choose a single tool. Use the left mouse button in combination with the Shift key to choose a range of tools. Use the left mouse button with the Ctrl key to selectively choose tools from the list. The Ctrl key also enables you to deselect.
OK to accept the tools. The tools retrieved from the library now appears in the Machine Tool View of the Operation Navigator and will be available for selection when defining operations.
Using a Tool Holder Changing the Tool You will drag and drop the operation so that it uses the library tool with a holder. In the Machine Tool View of the Operation Navigator, drag and drop the
437 FIXED_CONTOUR operation onto the UGTI0203_016 tool.
The operation now uses a library tool with a holder.
MB3
Generate to generate the tool path and OK to accept the tool path generation.
Using a Tool Holder Displaying the Tool Holder Assembly You will observe how you can graphically display a tool holder assembly when replaying a milling operation. Only tools retrieved from a library and containing a modeled assembly can display a tool holder assembly. If a part file defining the tool holder does not exist or cannot be loaded, then the Solid tool display option is used in place of the Assembly display. Choose the Verify Toolpath icon on the Manufacturing Operations toolbar. The Toolpath Visualization dialog displays with the Replay tab chosen. Choose Assembly for the Tool Display Option.
438 Zoom Out if necessary to see the tool holder. Choose the Play Forward icon.
OK to complete the tool path visualization. Close the part file.
Machining a Core You will create two fixed axis surface contouring operations that use the Area Milling drive method to machine a core. The first operation will use None as the Steep containment to mill the entire cut area. It will leave large scallops on the sides.
The second operation will use Directional Steep as the Steep Containment to cross cut only the steep areas and remove the large scallops left by the first operation.
439
Machining a Core Opening the Part Open part file srf_area_mill_4.prt from the srf subdirectory. Choose Application
Manufacturing.
In the Geometry View of the Operation Navigator, expand the objects as illustrated below.
The WORKPIECE group defines the part geometry that both operations will use.
Machining a Core Defining the Cut Area The cut area defines the area of the part the operation considers for cutting when generating the tool path. It may be specified in a geometry group and then inherited or it may be specified within individual operations. If you do not specify a cut area, the system cuts the entire Part Geometry. In this example, you will define the cut area in a geometry group so that subsequent operations can inherit the same set of cut area parameters.
Choose the Create Geometry icon. Choose mill_contour as the Type. Choose the MILL_AREA icon.
440 Choose WORKPIECE as the Parent Group.
OK to begin creating the geometry group. Choose the Cut Area icon and Select.
Turn the Features option on. Select the surface region as illustrated below.
OK to accept the cut area. OK to create the MILL_AREA geometry group.
More About Surface Regions
Surface Regions (Tools Prepare Geometry Surface Region) are CAM features that contain faces on a single solid body or sheet. The ability to select a single entity makes the specification of Part and Blank geometry very easy. Surface Regions are also easy to identify and select as features using the Model Navigation Tool. Surface Regions are associative to the solid. That is, when you modify the solid, the associated Surface Regions update automatically to match the solid.
441 Surface Regions are created by selecting faces of a body. All faces of a Surface Region Feature must be on the same body. Three methods of defining Surface Regions (Seed, All Faces, and Selected Faces) are available in the Surface Regions dialog box under Region Type. To summarize, the purpose of creating Surface Regions is to organize the areas to be machined, to make the selection of Part and Blank Geometry easier by enabling you to use the Surface Region selection method, and to establish associativity with bodies.
Machining the Entire Cut Area The first operation in this program will machine the entire cut area.
Machining the Entire Cut Area Beginning the Operation Choose the Create Operation icon. Choose mill_contour as the Type. Choose CONTOUR_ZIGZAG as the subtype.
This subtype defines most of the operation parameters you will need to mill the entire cut area. The system automatically names the operation CONTOUR_ZIGZAG.
442 Specify the following groups in the Create Operation dialog.
The operation will inherit the parameters defined by these groups. OK to begin creating the operation.
Machining the Entire Cut Area Displaying Part Geometry Choose the Part icon
and Display to highlight the part geometry.
The part geometry is defined by the entire body. This operation inherits the part geometry from the Workpiece group. Refresh the display.
Machining the Entire Cut Area Displaying Cut Area Choose the Cut Area icon
and Display to highlight the cut area.
443
This operation inherits the cut area from the Mill Area group you created. Refresh the display.
Machining the Entire Cut Area Specifying None as the Containment Specifying None as the Steep Containment imposes no steepness restrictions on the tool path and allows the operation to mill the entire cut area. Notice that the Drive Method defaults to Area Milling.
The CONTOUR_ZIGZAG subtype that you chose earlier determined this as the default. Choose Area Milling under Drive method.
Notice that the Steep Containment parameter defaults to None. The CONTOUR_ZIGZAG subtype you chose earlier determined this as the default.
444
Machining the Entire Cut Area Specifying the Cut Angle Choose User Defined as the Cut Angle.
The Cut Angle dialog displays. The Cut Angle determines the angle of rotation of the cutting pattern about the ZC axis with respect to the XC axis.
OK to accept 0.0000 degrees as the Cut angle. Choose Display Cut Direction. A vector displays indicating the cut angle direction of the zig-zag cutting moves. In this operation, the tool will zig-zag parallel to the XC axis.
The next operation in the program must have a cut direction defined at 90 degrees to this one in order to cross cut and remove the scallops remaining on the steep surfaces. OK to return to the CONTOUR_ZIGZAG dialog.
445
Machining the Entire Cut Area Generating the Tool Path You will generate the tool path and observe how the operation mills the entire cut area. Generate the tool path.
Machining the Entire Cut Area Visualizing the Scallops Choose the Verify icon at the bottom of the dialog. Choose the Dynamic tab. Choose the Play Forward option. Notice the large scallops left on the sides of the part.
You will use Directional Steep in the next section to remove these scallops. OK to complete the tool path visualization. OK to complete the operation.
446
Machining Steep Areas The second operation in this program will machine only the steep areas left by the first operation.
Machining Steep Areas Beginning the Operation Choose the Create Operation icon in the toolbar. Choose mill_contour as the Type. Choose CONTOUR_AREA_DIR_STEEP as the subtype.
This subtype defines most of the operation parameters you will need to mill only the steep areas. The system automatically names the operation CONTOUR_AREA_DIR_STEEP. Specify the following groups in the Create Operation dialog.
447 The operation will inherit the parameters defined by these groups. OK to begin creating the operation.
Machining Steep Areas Specifying Directional Steep as the Containment The Directional Steep option will cross cut only the steep areas and remove the scallops left behind by the first operation. Steep areas are determined relative to the cut direction. Choose Area Milling under Drive Method. Notice that the Steep Containment parameter defaults to Directional Steep. The CONTOUR_AREA_DIR_STEEP subtype you chose earlier determined this default. Choose Directional Steep as the Steep Containment.
Machining Steep Areas Specifying the Cut Angle Remember the Cut Angle for the previous operation was 0.000 degrees. This operation must cross cut the steep areas to remove the large scallops. Notice that the Cut Angle for this operation defaults to 90.0000 degrees.
OK to accept 90 degrees as the cut angle. The Area Milling Method dialog displays. Choose Display Cut Direction. A vector displays indicating the direction of the zig-zag cutting moves. In this operation, the tool will zig-zag parallel to the YC axis.
448
Machining Steep Areas Specifying the Steep Angle Key in 55 for the Steep Angle.
The operation will now cut only the areas where the steepness of the tool path is greater than 55 degrees.
OK to accept the parameters in the Area Milling Method dialog.
Machining Steep Areas Generating the Tool Path You will generate the tool path and observe how the operation machines only the steep areas.
449 Generate the tool path.
Notice that only the steep areas relative to the cut direction are machined. OK to complete the operation. By comparing the Area Milling operation that uses Steep Containment set to None with the operation that uses Steep Containment set to Directional Steep, you can see that the two operations finish the entire core.
Close the part file.
Controlling Scallop Height You will control the scallop height when using the Follow Periphery cut pattern to machine steep and non-steep areas.
450
By calculating the tool path directly on the part, scallop heights are consistent and both steep and non-steep surfaces can be effectively machined in the same operation.
Controlling Scallop Height Open the Part File Open part file srf_area_mill_7.prt from the srf subdirectory. Choose Application
Manufacturing.
Controlling Scallop Height Replaying the Tool Path You will replay the current Follow Periphery tool path and observe that the stepovers on the steep areas are very large. In the Program Order view of the Operation Navigator, choose the CONTOUR_FOLLOW operation and MB3 Replay. Currently, the drive path is calculated on the XC-YC plane at the base of the part and then projected upward onto the part surface. This results in large stepovers relative to the part surface on the steep areas.
451
Controlling Scallop Height Visualizing the Scallops You will display the scallops using dynamic material removal. Highlight CONTOUR_FOLLOW.
Choose the Verify Toolpath icon in the toolbar. Choose the Dynamic tab. Choose the Play Forward option. Notice the large scallops on the steep areas.
OK to complete the tool path visualization.
452
Controlling Scallop Height Controlling Scallop Height You will control the scallop height by calculating the tool path, including the stepovers, directly on the part. Double-click on the CONTOUR_FOLLOW operation icon to edit the operation.
Choose Area Milling.
The Apply option is currently set to On Plane. This causes the drive path to be calculated on XM-YM plane and then projected onto the part surface. The On Part option calculates the tool path directly on the part. Set the Apply option to On Part.
This option is only available for the Follow Periphery cut pattern. OK to accept it.
Controlling Scallop Height Generating the Tool Path You will generate the tool path and observe how the stepover is now consistent. Generate the tool path.
453
OK to complete the operation.
Controlling Scallop Height Visualizing the Scallops Use Verify Toolpath as you did before to display dynamic material removal.
Notice the scallop height is now consistent. OK to complete the tool path visualization. Close the part file.
Machining a Cavity You will create four fixed axis surface contouring operations that use the Area Milling drive method to semi-finish and finish a cavity. The program begins with a Cavity Mill operation, ZLEVEL_FOLLOW_CAVITY, that roughs out the cavity.
454
The first operation you create, CONTOUR_FOLLOW, will semi-finish the bottom of the cavity.
The second operation you create, CONTOUR_FOLLOW_1, will semi-finish the entire cavity.
The third operation you create, CONTOUR_ZIGZAG, will use None as the Steep Containment to finish the entire cavity.
The fourth operation you create, CONTOUR_AREA_DIR_STEEP, will use Directional Steep as the Steep Containment to cross cut only the steep areas and remove the scallops.
455
Machining a Cavity Opening the Part Open part file srf_area_mill_5.prt from the srf subdirectory. Choose Application
Manufacturing.
Machining a Cavity Examining the WORKPIECE Group The WORKPIECE group defines the part and blank geometry. Expand the objects in the Geometry View of the Operation Navigator. The ZLEVEL_FOLLOW_CAVITY operation inherits parameters from the WORKPIECE and MCS_MILL groups. Highlight the WORKPIECE group.
456
Choose the Display Object icon
in the toolbar.
The part and blank geometry highlight.
Refresh the graphics display.
Machining a Cavity Visualizing the Cavity Mill Operation You will use Verify Toolpath to graphically simulate material removal for the existing Cavity Mill operation. Highlight the ZLEVEL_FOLLOW_CAVITY operation.
Choose the Verify Toolpath icon. Choose the Dynamic tab. Choose the Play Forward icon.
457
OK to complete the tool path visualization.
Semi-Finishing the Bottom of the Cavity You will create a new operation and use the Area Mill Drive Method to semi-finish the bottom of the cavity.
Semi-Finishing the Bottom of the Cavity Beginning the Operation Choose the Create Operation icon. Choose mill_contour as the Type. Choose CONTOUR_FOLLOW as the subtype.
This subtype defines most of the operation parameters you will need to mill the cut area.
458 Specify the following groups in the Create Operation dialog.
The operation will inherit the parameters defined by these groups. OK to begin creating the operation.
Semi-Finishing the Bottom of the Cavity Defining the Cut Area The cut area defines the area of the part the operation considers for cutting when generating the tool path. For this operation, you will select the face at the bottom of the cavity. Choose the Cut Area icon and Select.
Select the face at the bottom of the cavity as illustrated below.
OK to accept the face.
459
Semi-Finishing the Bottom of the Cavity Specifying the Stepover This operation uses a fairly large tool to semi-finish the bottom of the cavity. You will need to decrease the stepover. Choose Area Milling under Drive method.
Key in 15.0 for the Stepover Percent.
OK to accept the stepover.
Semi-Finishing the Bottom of the Cavity Generating the Tool Path You will generate the tool path and observe how the operation machines the cut area at the bottom of the cavity. Generate the tool path.
Notice that the tool path does not cover the entire cut area. Part of the cut area is left uncut because the tool movement is limited by the sides of the cavity.
Choose the Edit Display icon under Tool Path and choose 3-D for the Tool Display.
460 OK to accept the tool display. Change to a Front view and Replay the tool path. The tool comes close to the sides of the cavity, but does not gouge the part. The operation machines as much of the cut area as possible without violating the part geometry.
The distance between the tool and the part is defined by the Part Stock in the MILL_SEMI_FINISH Method group. This is the material that is left for the finishing operations to remove. Change to a TFR-ISO view. OK to complete the operation.
Semi-Finishing the Entire Cavity This operation will use the Area Mill Drive Method to semi-finish the entire cavity. By using a smaller tool and a smaller stepover, large scallops will be removed and the entire bottom of the cavity will be semi-finished.
461
Semi-Finishing the Entire Cavity Beginning the Operation Choose the Create Operation icon in the toolbar. Choose mill_contour as the Type. Choose CONTOUR_FOLLOW as the subtype.
This subtype defines most of the operation parameters you will need. Specify the following groups in the Create Operation dialog.
OK to begin creating the operation.
Semi-Finishing the Entire Cavity Defining the Cut Area If you do not explicitly define the cut area in the operation or in a geometry group, the system uses the entire defined Part Geometry (excluding areas not accessible by the tool) as the cut area. In other words, the system uses the silhouette of the part as the cut area.
462 Cut Areas require additional processing time when generating a tool path. It is therefore a good idea to not define a cut area unless it is necessary. For this operation, you will not define the cut area.
Semi-Finishing the Entire Cavity Specifying the Stepover You will need to decrease the stepover to produce smaller scallops. Choose Area Milling under Drive method.
The Area Milling Method dialog displays. Key in 15.0 for the Stepover Percent.
OK to accept the stepover.
Semi-Finishing the Entire Cavity Generating the Tool Path You will generate the tool path and observe how the operation machines the entire cavity. Generate the tool path.
463
Notice that the tool rolls over the outer edge of the part. This occurs as a result of edge tracing. In this case, because a cut area was not defined, edge tracing cannot be removed by simply turning on the Remove Edge Traces option. Choose Cutting. Note that the Part Stock is set at 0.25 mm and the part tolerance is set at +/- 0.03. These values were determined when the MILL_SEMI_FINISH method was chosen.
Turn the Remove Edge Traces option on and OK to accept it. Generate the tool path. The edge traces remain. In cases like this where edge tracing occurs because a cut area has not been specified, you must use a Trim boundary to remove the edge tracing. OK to complete the operation.
Semi-Finishing the Entire Cavity Defining a Trim Boundary You will define a Trim boundary in a Mill Area geometry group. By doing this, you will define the boundary just once and then apply it to as many operations as needed.
Choose the Create Geometry icon.
464 Choose mill_contour as the Type. Choose the MILL_AREA icon and WORKPIECE as the Parent group.
OK to begin creating the geometry group. Choose the Trim icon and Select.
ChooseOutside as the Trim Side. This will insure that the tool path is created inside of the boundary and will exclude all areas outside of the boundary. With the Face Boundary icon
chosen, select the bottom face of the part.
OK to accept the boundary. OK to create the MILL_AREA geometry group. This geometry group contains the Trim boundary and can be used as a parent to as many operations as needed.
465
Semi-Finishing the Entire Cavity Applying the Trim Boundary You will now make the MILL_AREA geometry group a parent of the CONTOUR_FOLLOW_1 operation so that the Trim boundary is applied to the operation. In the Geometry view of the Operation Navigator, double-click on the CONTOUR_FOLLOW_1 to display the CONTOUR_FOLLOW dialog.
Choose the Geometry tab. Turn the Geometry option on and choose Reselect.
Choose MILL_AREA in the Reselect Geometry dialog and OK. OK to complete the operation. The Geometry view of the Operation Navigator now shows the MILL_AREA group as a parent of the CONTOUR_FOLLOW_1 operation.
This operation will now inherit the parameters defined in the MCS_MILL, WORKPIECE, and the MILL_AREA groups.
466
Semi-Finishing the Entire Cavity Generating the Tool Path You will generate the tool path and observe how the operation no longer generates edge tracing. In the Operation Navigator, highlight CONTOUR_FOLLOW_1 and MB3
Generate
Notice that the tool path no longer rolls over the outer edge of the part. The remaining operations you create will also require the Trim boundary defined in the MILL_AREA group. OK the tool path Generation dialog.
Finishing the Entire Cavity This operation will use the Area Mill Drive Method to finish the entire cavity with a zig-zag cut pattern.
467
Finishing the Entire Cavity Beginning the Operation Choose the Create Operation icon. Choose CONTOUR_ZIGZAG as the subtype.
Specify the following groups in the Create Operation dialog.
OK to begin creating the operation. Choose Area Milling under Drive method. Notice that the Steep Containment parameter defaults to None. The CONTOUR_ZIGZAG subtype you chose earlier determined this option as the default.
Finishing the Entire Cavity Specifying the Cut Angle
468 The Cut Angle determines the angle of rotation of the cutting pattern about the ZC axis with respect to the XC axis. Choose User Defined as the Cut Angle.
OK to accept 0.0000 degrees as the Cut angle. Choose Display Cut Direction. A vector displays indicating the direction of the zig-zag cutting moves. In this operation, the tool will zig-zag parallel to the XC axis.
The next operation must have a cut direction defined at 90 degrees to this one in order to remove the scallops left on the steep surfaces.
Finishing the Entire Cavity Specifying the Stepover You will need to decrease the stepover to produce smaller scallops. Key in 10.0 for the Stepover Percent.
OK to return to the CONTOUR_ZIGZAG dialog.
Finishing the Entire Cavity Generating the Tool Path
469 You will generate the tool path and observe how the operation finishes the entire cavity. Generate the tool path.
OK to complete the operation.
Finishing the Steep Areas This operation will use Directional Steep as the Steep Containment to cross cut only the steep areas and remove the scallops.
Finishing the Steep Areas Beginning the Operation Choose the Create Operation icon in the toolbar.
470 Choose CONTOUR_AREA_DIR_STEEP as the subtype.
Specify the following groups in the Create Operation dialog.
OK to begin creating the operation.
Finishing the Steep Areas Specifying Directional Steep as the Containment The Directional Steep option will allow you to cross cut only the steep areas. Steep areas are determined in relation to the cut direction. Choose Area Milling under Drive Method. Notice that the Steep Containment defaults to Directional Steep. Choose Directional Steep as the Steep Containment.
Remember that the Cut Angle for the previous operation was 0.000 degrees. This operation must cross cut the steep areas to remove the large scallops. Notice that the Cut Angle defaults to 90.0000 degrees.
471 OK to accept the cut angle.
Finishing the Steep Areas Specifying the Steep Angle Key in 60 degrees for the Steep Angle.
The operation will only cut areas where the steepness of the tool path is greater than 60 degrees.
Finishing the Steep Areas Specifying the Stepover You will need to decrease the stepover to produce smaller scallops. Key in 10.0 for the Stepover Percent.
OK to accept the parameters in the Area Milling Method dialog.
472
Finishing the Steep Areas Generating the Tool Path You will generate the tool path and observe how the operation finishes the steep areas Generate the tool path.
OK to complete the operation.
Finishing the Steep Areas Visualizing the Tool Paths You will use Verify Toolpath to graphically simulate material removal for the entire program. In the Program Order View of the Operation Navigator, highlight PROGRAM.
This chooses all of the operations in the program. Choose the Verify Toolpath icon in the toolbar Choose the Dynamic tab. Choose the Play Forward option.
473
The material removed by each successive operation displays in a contrasting color.
Finishing the Steep Areas Comparing to the Original Model You can compare the machined part to the original model. White areas, if any, indicate the areas where further finishing is required to machine to the specified Outtol. Choose Compare.
OK to dismiss the Toolpath Visualization dialog. Close the part file.
Displaying Excess Material The Show Excess function allows you to display areas where excess material remains due to large scallops and inaccessibility of the tool. This function is useful in determining how much material remains for subsequent operations to remove and for comparing the finished machined part to the modeled part.
474
You will first use the Show 3D option to create a faceted model of the uncut material that remains after generating a specific operation or sequence of operations. You will then use the Show Excess option to compare the faceted model to the specified Excess Material. Excess Material is an offset value that defines the allowable material measured from the part. Areas of the faceted model that exceed this offset are graphically displayed as excess material when you choose Show Excess.
Displaying Excess Material Opening the Part Open part file srf_area_mill_6.prt from the srf subdirectory. Choose Application
Manufacturing.
Choose the Shaded icon
to display the part as a shaded solid.
Displaying Excess Material Changing Object Color Preference You should display the faceted model in a color that contrasts the part. Choose Preferences
Object from the menu bar.
Choose Orange (or a similar color) and OK to accept it.
OK to accept the Object Preferences.
475
Displaying Excess Material Creating a Roughing Faceted Model You will use a roughing operation to create a faceted model representing the uncut material. In the Program Order View, highlight the ZLEVEL_FOLLOW_CAVITY icon.
Choose the Verify Toolpath icon in the toolbar. Choose the Static tab.
Choose Create to create the faceted model. The faceted model displays in orange and represents graphically the uncut material that remains after generating the ZLEVEL_FOLLOW_CAVITY operation.
The faceted model was created from a roughing operation that uses a 0.1200 mm Outtol and a 1.0000 mm Part Stock. Therefore, any uncut material within a 1.1200 mm offset of the part is allowed by the operation. Any uncut material beyond the 1.1200 mm offset is excess material. Choose Delete to remove the currently displayed faceted model.
Displaying Excess Material Displaying Excess Material
476
In the Toolpath Visualization dialog, choose Excess and key in 1.1200 for the Excess Material.
Choose Create. The excess material graphically represents the uncut material outside of the specified 1.1200 mm Excess Material offset. This is the material that must be removed by subsequent operations in the program.
The color of the Excess Material is determined under Preferences Visualize in the menu bar.
Manufacturing
The thickness of the excess material can determine whether or not the subsequent operations are appropriate. If it is too thick, additional roughing operations may need to be added. Choose Delete to remove the displayed excess material.
Displaying Excess Material Determining Excess Material Thickness You can get an idea of the thickness of the excess material by increasing the specified Excess Material value. Any excess material that continues to display is thicker than the specified increase. Key in 1.5200 for the Excess Material.
477
This increases the Excess Material value by 0.4000 mm. Choose Create.
Excess material continues to display, although there is now less of it. The displayed excess material is thicker than 0.4000 mm. Choose Delete to remove the currently displayed excess material. OK to complete the tool path visualization.
Displaying Excess Material Creating a Finishing Faceted Model You will use the two finishing operations to create a faceted model representing the finished machined part. You will then compare the finished machined part to the modeled part to determine whether or not the finish meets the design specifications. Choose Preferences
Object from the menu bar.
Choose Red (or a similar color) and OK to accept it. This is the color in which the faceted model will display. OK to accept the Object Preferences. In the Program Order View of the Operation Navigator, highlight CONTOUR_ZIGZAG and CONTOUR_AREA_DIR_STEEP. You will need to use the Ctrl key to select the second operation.
478
Choose the Verify Toolpath icon in the toolbar. Choose the Static tab. Choose Create to create the faceted model. The faceted model displays in red. It graphically represents the uncut material that remains after finishing the part.
The finishing operations use a 0.0300 mm Outtol and a 0.0300 mm Intol. Any uncut material within 0.0300 mm offset of the part is allowed by the program. Any uncut material outside of the 0.0300 mm offset is excess material. Choose Delete to remove the currently displayed faceted model.
Displaying Excess Material Displaying Excess Material In the Toolpath Visualization dialog, choose Excess and key in 0.0300 for the Excess Material.
Choose Create.
479
Notice that there is quite a bit of excess material remaining on the finished part. You can reduce the amount of excess material by reducing the stepover to create smaller scallops and also by changing the part Intol and Outtol smaller values. Making these values smaller will increase the size of the calculated tool path and also increase the time required for its calculation. Choose Delete to remove the currently displayed excess material. OK to complete the tool path visualization.
Displaying Excess Material Modifying the Operations You will decrease the stepover in the two operations to finish the part more accurately. In the Program Order View of the Operation Navigator, double-click on the CONTOUR_ZIGZAG icon.
Choose Area Milling under Drive Method.
480 Key in 10.0 for the Stepover Percent.
OK to accept the change. Generate the tool path. OK to complete the operation. Repeat these steps for the CONTOUR_AREA_DIR_STEEP operation.
Displaying Excess Material Creating a Finishing Faceted Model You will create a new faceted model representing the machined part with the smaller finishing stepovers. In the Program Order View of the Operation Navigator, highlight CONTOUR_ZIGZAG and CONTOUR_AREA_DIR_STEEP.
Choose the Verify Toolpath icon in the toolbar. Choose the Static tab. Choose Create to create the faceted model. The faceted model displays in red.
Choose Delete to remove the currently displayed faceted model.
481
Displaying Excess Material Displaying Excess Material In the Toolpath Visualization dialog, choose Excess and key in 0.0300 for the Excess Material.
This accounts for the Outtol in the finishing operations. Choose Create.
Notice that there is less excess material remaining on the finished part. OK to complete the tool path visualization. Close the part file.
Flow Cut Drive Method The Flow Cut drive method generates fixed axis surface contouring tool paths that machine concave corners and valleys formed by part surfaces. The system determines where to apply
482 flow cutting based on bi-tangency contact points and the angle between part surfaces. You can create single pass or multiple pass operations.
The resulting tool path is optimized in such a way that the tool remains in contact with the part as much as possible and minimizes non-cutting moves. The Flow Cut drive method, like the Area Milling drive method, allows you to define a simple tool holder to ensure a collision free tool path. It is recommended that only Ball Nose tools be used in flow cut operations. Unsatisfactory results in the tool path can occur if Bull Nose or Flat Nose tools are used. In this lesson, you will create Single Pass, Multiple Pass, and Reference Tool Flow Cut operations.
Machining a Cavity In this section, you will examine the geometry groups and the sequence of operations. You will observe how the rough, semi-finish, and finish operations inherit parameters and work in sequence to machine the entire cavity.
Machining a Cavity Opening the Part
483
Open part file srf_flow_cut_1.prt from the srf subdirectory. Notice the concave corners and valleys formed between part surfaces. These are the areas the system will recognize when determining flow cuts.
Choose the Invisible Hidden Edges icon Choose Application
to display a wireframe.
Manufacturing.
Machining a Cavity Examining the WORKPIECE Group The WORKPIECE group defines the part geometry used by all of the operations. In the Geometry View of the Operation Navigator, fully expand the objects and doubleclick on the WORKPIECE icon to edit the group.
Choose the Part icon and Display.
484 The part geometry highlights.
Cancel out of the MILL_GEOM dialog.
Machining a Cavity Examining the MILL_AREA Group The MILL_AREA group defines the cut area used by the CONTOUR_AREA_NON_STEEP, CONTOUR_FOLLOW, ZLEVEL_PROFILE_STEEP, and FLOWCUT_SINGLE operations. Double-click on the MILL_AREA icon to edit the group.
Choose the Cut Area icon and Display.
The cut area geometry highlights.
485
Cancel out of the MILL_AREA dialog.
Machining a Cavity Visualizing Material Removal for the Program You will graphically simulate material removal for the program. In the Program Order View of the Operation Navigator, fully expand the objects. Notice the sequence of operations. The ZLEVEL_FOLLOW_CAVITY operation first roughs out the cavity. The CONTOUR_AREA_NON_STEEP and ZLEVEL_PROFILE_STEEP operations then semi-finish the cavity. The CONTOUR_FOLLOW and FLOWCUT_SINGLE operations finish the cavity. Highlight the PROGRAM group.
Choose the Verify Toolpath icon
in the toolbar.
Choose the Dynamic tab. Choose the Play Forward icon. The material removed by each successive operation is displayed in a contrasting color.
486
In the following section, you will create a Single Pass Flow Cut operation similar to the one in this program. OK to complete the tool path visualization. Close the part file.
Creating a Single Pass Flow Cut Operation You will create a Single Pass Flow Cut operation that finishes the concave corners and valleys formed by the part surfaces.
Creating a Single Pass Flow Cut Operation Opening the Part Open part file srf_flow_cut_2.prt from the srf subdirectory. Choose Application
Manufacturing.
487
Creating a Single Pass Flow Cut Operation Beginning the Operation Choose the Create Operation icon. Choose mill_contour as the Type. The Type determines the subtype icons that are available and the groups that are initially available to choose from in the dialog. You can use any one of the subtypes outlined below to create a flow cut operation. Choose FLOWCUT_SINGLE as the subtype.
This subtype defines most of the operation parameters you will need to create a Single Pass Flow Cut operation. The system automatically names the operation FLOWCUT_SINGLE. Specify the following groups in the Create Operation dialog.
488 The operation will inherit the parameters defined by these groups. OK to begin creating the operation.
Creating a Single Pass Flow Cut Operation Displaying the Cut Area Choose the Cut Area icon and Display.
Notice that the Select/Reselect option is blanked for defining the cut area. The cut area cannot be defined within the operation because it is inherited from the MILL_AREA group.
The cut area has been defined as all the interior faces of the cavity. Refresh the display.
Creating a Single Pass Flow Cut Operation Generating the Tool Path You will observe how the operation generates the tool path along corners and valleys formed between part surfaces. Generate the tool path.
489
Creating a Single Pass Flow Cut Operation Removing Short Tool Path Segments Minimum Cut Length enables you to eliminate short cutting moves that may occur in isolated areas of the part. You will eliminate the short cutting moves that occur at the intersection of the fillets.
Choose the More tab. Key in 0.8000 for the Min. Cut Length.
490
Cutting moves shorter than 0.8000 will not be generated. Choose the Main tab. Reject the previous tool path and Generate a new one.
Creating a Single Pass Flow Cut Operation Restricting the Maximum Concavity Maximum Concavity enables you to determine where flow cuts are created based on the angle of concave corners and valleys formed by part surfaces. Flow cuts are created where the angle between surfaces is less than or equal to the specified Maximum Concavity angle. The Maximum Concavity is currently specified as 179.0000 degrees. Because of this, the tool does not cut across the top of the part where the angle between surfaces is very flat. The angle between the surfaces in this area exceeds 179.000 degrees, so the tool retracts.
491
Watch what happens when you restrict the Maximum Concavity. Choose the More tab. Key in 100 for the Maximum Concavity.
Choose the Main tab. Reject the previous tool path and Generate a new one.
Notice that some of the flow cuts have been eliminated. The angles formed between part surfaces in these areas exceeds the Maximum Concavity of 100.0000 degrees. The areas of the cylindrical intersections that have a concavity less that 120 are not cut because the length of the cut is less than 0.80.
Creating a Single Pass Flow Cut Operation Increasing the Maximum Concavity
492
You will now increase the Maximum Concavity so that the tool cuts as much of the flat area on the top of the part as possible. The value you enter must be positive and must be less than or equal to 179.0000 degrees. Key in 179 for the Maximum Concavity.
Choose the Main tab. Reject the previous tool path and Generate a new one. Flow cuts are created where the angles formed between adjacent part surfaces are less than or equal to the 179.000 degrees.
A closer look reveals that the tool path still does not cut all the way across the top of the part. This is an area where the angle between part surfaces is very large (between 179 and 180 degrees) and is nearly flat.
You cannot specify a Maximum Concavity greater than 179.0000 degrees. You can, however, increase the Hookup Distance to eliminate unwanted gaps in the tool path.
493
Creating a Single Pass Flow Cut Operation Eliminating Unwanted Gaps in the Tool Path Hookup Distance enables you to eliminate small discontinuities or unwanted gaps in the tool path. These discontinuities occur where the tool retracts from the part and are sometimes caused by gaps between surfaces or variations in the angle of concavity that exceed the specified Maximum Concavity angle. The value you enter determines the distance the tool will span to connect the end points of cutting moves. The system will connect the two ends by linearly extending the two paths and will not gouge the part. Choose the More tab. Key in 0.2500 for the Hookup Distance.
Choose the Main tab. Reject the previous tool path and Generate a new one.
The tool no longer retracts and now continues cutting across the top of the part.
Creating a Single Pass Flow Cut Operation Flow Cutting Along the Fillets As stated earlier, the system determines where to apply flow cutting based on bi-tangency contact points. To generate a flow cut, the tool must contact two part surfaces at two distinct points. Single pass flow cutting will not occur in areas where the curvature of the surface is larger than the corner radius of the tool as illustrated below. It will occur, however, in areas where the curvature of the surface is equal to or less than the corner radius of the tool, allowing bi-tangency contact points.
494
In your part, the fillet that surrounds the cavity on three sides has a radius of 0.5000 inch. The tool you have been using (MILL_2) has a diameter of only 0.2000 inch. This is why flow cutting has not occurred along the fillet. You will change to a larger tool and observe how flow cutting is generated along the fillets as a result bi-tangency contact points between two surfaces. Choose the Groups tab. Choose Tool: MILL_2 and Reselect.
Choose MILL_3 in the Reselect Tool dialog and OK. MILL_3 is a 1.0000 inch diameter ball end mill. Because this tool has the same radius as the fillet, it contacts the surfaces on both sides of the fillet. Choose the Main tab. Reject the previous tool path and Generate a new one. Notice that flow cutting now occurs along the fillets.
495
OK to complete the operation. Close the part file.
Creating a Multiple Pass Flow Cut Operation You will create a Multiple Pass Flow Cut operation to finish the concave corners and valleys formed by the part surfaces.
Creating a Multiple Pass Flow Cut Operation Opening the Part Open part file srf_flow_cut_2.prt from the srf subdirectory again. This is the same part you used for creating the single pass operation.
496
Choose Application
Manufacturing.
Creating a Multiple Pass Flow Cut Operation Beginning the Operation Choose the Create Operation icon in the CAM Create toolbar. Choose mill_contour as the Type. Choose FLOWCUT_MULTIPLE as the subtype.
This subtype defines most of the operation parameters you will need to create a Multiple Pass Flow Cut operation. The system automatically names the operation FLOWCUT_MULTIPLE. Specify the following groups in the Create Operation dialog.
The operation will inherit the parameters defined by these groups. OK to begin creating the operation.
497
Creating a Multiple Pass Flow Cut Operation Generating the Tool Path You will use the default operation parameters to generate the multiple pass tool path. Generate the tool path.
You will now make some changes to improve the tool path.
Creating a Multiple Pass Flow Cut Operation Removing Short Tool Path Segments You will eliminate the short cutting moves at the intersections of the fillets as you did previously for the single pass operation.
498
Choose the More tab. Key in 0.8000 for the Minimum Cut Length.
Choose the Main tab
Creating a Multiple Pass Flow Cut Operation Specifying the Cut Sequence Sequencing enables you to determine the order in which the multiple Zig or Zig-Zag cut passes are executed. Inside-Out causes the cutter to start at the center pass and move toward one of the outside passes. The tool then moves back to the center cut and works its way toward the other side.
Outside-In does just the opposite.
499
Unidirection causes the cutter to move from one outside cut to the other, traversing through the center.
Be sure Inside-Out is specified for the Sequencing.
Creating a Multiple Pass Flow Cut Operation Specifying the Number of Offsets Number of Offsets enables you to determine the number of passes to generate on each side of the center flow cut. Key in 4 for the Number of Offsets.
Creating a Multiple Pass Flow Cut Operation Specifying the Cut Direction While a Mixed cut direction will provide the least amount of tool motion, it is frequently desirable to cut from high to low. Cutting from High to Low tends to keep the tool forced into the tool holder.
500 Choose the More tab. Set the Cut Direction to High to Low.
Choose the Main tab.
Creating a Multiple Pass Flow Cut Operation Generating the Tool Path You will generate the tool path and observe how the short cutting moves have been eliminated. Reject the previous tool path and Generate a new one.
Notice that the short cutting moves at the intersections of the fillets have been eliminated. OK to complete the operation.
Creating a Multiple Pass Flow Cut Operation Visualizing Material Removal for the Program You will graphically simulate material removal for the program. In the Program Order view of the Operation Navigator, highlight PROGRAM.
501
Choose the Verify Toolpath icon on the CAM toolbar. Choose the Dynamic tab. Choose the Play Forward option.
OK to complete the tool path visualization. Close the part file.
Creating a Reference Tool Flow Cut Operation You will create a Reference Tool Flow Cut operation that uses multiple passes to finish the concave corners and valleys formed by the part surfaces.
Reference Tool Diameter enables you to specify the width of the finishing cut region based on the diameter of the roughing (reference) tool. The reference tool is typically the tool used to previously rough out the area. The system calculates the bi-tangency contact points from the
502 specified Reference Tool Diameter and then uses these points to define the cut region for the finishing operation. 1. 2. 3. 4.
Reference Tool Diameter Finishing Tool Bi-Tangency Contact Pts. of Reference Tool Cut Region Defined by Contact Pts. of Reference Tool
Because the reference tool determines the bi-tangency contact points rather than the actual cutting tool, this type of flow cut operation can finish large fillets using multiple passes of a small tool.
Creating a Reference Tool Flow Cut Operation Opening the Part Open part file srf_flow_cut_3.prt from the srf subdirectory.
Choose Application
Manufacturing.
Creating a Reference Tool Flow Cut Operation Beginning the Operation Choose the Create Operation icon in the toolbar.
503 Choose mill_contour as the Type. Choose FLOWCUT_REF_TOOL as the subtype.
This subtype defines most of the operation parameters you will need to create a Reference Tool Flow Cut operation. The system automatically names the operation FLOWCUT_REF_TOOL. Specify the following groups in the Create Operation dialog.
The operation will inherit the parameters defined by these groups. OK to begin creating the operation.
Creating a Reference Tool Flow Cut Operation Removing Short Tool Path Segments You will eliminate the short cutting moves that occur at the intersection of the fillets as you did for the single and multiple pass operations. Choose the More tab. Key in 0.8000 for the Minimum Cut Length.
Choose the Main tab.
Creating a Reference Tool Flow Cut Operation
504
Specifying the Reference Tool Diameter The system calculates the bi-tangency contact points from the specified Reference Tool Diameter and then uses these points to define the cut region for the finishing operation. You must key in a diameter for the reference tool that is larger than that of the current tool in use. The current tool in use (MILL_2) has a diameter of 0.2000. Key in 1.0 for the Reference Tool Diameter. You might need to scroll down in the dialog to see this option.
Because the reference tool has the same radius as the fillet (.5000), it contacts the surfaces on each side of the fillet, establishing the necessary bi-tangency contact points. Overlap Distance enables you to extend the width of the area defined by the Reference Tool Diameter along the tangent surfaces.
Creating a Reference Tool Flow Cut Operation Generating the Tool Path You will generate the tool path and observe how the concave corners, valleys, and fillets are finished with multiple passes. Generate the tool path.
OK to complete the operation.
Creating a Reference Tool Flow Cut Operation Visualizing Material Removal for the Program
505
You will graphically simulate material removal for the program. Highlight the PROGRAM group.
Choose the Verify Toolpath icon in the toolbar. Choose the Dynamic tab. Choose the Play Forward option.
OK to complete the tool path visualization. Close the part file.
Radial Cut Drive Method The Radial Cut drive method generates a fixed axis surface contouring tool path normal to and along a boundary.
506
Radial cuts allow hand finishing of concave corners and valleys across scallops rather than along scallops. It is often used as a follow-up to flow cutting. In this lesson, you will create a fixed axis surface contouring operation that uses the Radial Cut drive method to finish the concave corner the part.
Creating a Radial Cut Operation You will create a fixed axis surface contouring operation that uses the Radial Cut drive method. You will then Animate the program to graphically simulate material removal.
Creating a Radial Cut Operation
507
Opening the Part Open part file srf_radial_1.prt from the srf subdirectory.
Choose Application
Manufacturing.
Creating a Radial Cut Operation Beginning the Operation Choose the Create Operation icon
in the toolbar.
Choose mill_contour as the Type. The Type determines the subtype icons that are available and the groups that are initially available to choose from in the dialog. Choose FIXED_CONTOUR as the subtype.
Specify the following groups in the Create Operation dialog.
508 The WORKPIECE geometry group defines the part geometry and the blank geometry. Blank geometry is required by the Verify function to graphically simulate material removal. The operation will inherit the parameters defined by these groups. OK to begin creating the operation.
Creating a Radial Cut Operation Defining the Drive Method The Radial Cut drive method allows you to define a tool path normal to and along a boundary. Choose Radial Cut under Drive method.
A Warning dialog is displayed, cautioning you that previously defined drive parameters will be deleted. OK the warning.
Creating a Radial Cut Operation Defining the Drive Geometry Drive geometry allows you to define the boundaries along which the tool will zig or zig-zag. Choose Select under Drive Geometry. Choose Open as the Type.
Select the five edges in sequence as illustrated below.
509
Creating a Radial Cut Operation Specifying a Tool Diameter Percent Stepover Stepover allows you to specify the distances between successive cutting passes. The stepover is a straight line distance measured either at the widest point between successive passes (A-B) or at the boundary intersection (C-D), depending on the Stepover method used.
The % of Tool option allows you to define the stepover in terms of a percentage the effective tool diameter. This distance is measured at the boundary (between points C and D). Turn the Stepover option on. % of Tool should already be specified as the Stepover. Key in 20 for the Percent.
OK to complete the drive geometry. A single temporary boundary is created.
510
If multiple boundaries are defined, a lift is applied allowing the tool to traverse from one boundary to the next. OK to complete the Radial Cut drive method.
Creating a Radial Cut Operation Generating the Tool Path You will generate the tool path and observe how the tool path zig-zags along the boundary. Generate the tool path.
Notice how far apart the stepovers are at the corners. You may control this by specifying a maximum stepover value.
511
Creating a Radial Cut Operation Specifying a Maximum Stepover The Maximum option requires you to key in a value defining the Maximum allowable distance between Stepovers. This value is applied at the widest point of the cut pass (between points A and B).
Choose Radial Cut under Drive method. Choose Maximum as the Stepover.
Key in .05 for the Value.
OK to complete the Radial Cut Drive Method.
Creating a Radial Cut Operation Generating the Tool Path You will generate the tool path and observe how the modified Stepover effects the tool path. Generate the tool path.
512
Notice how the tool path crosses over itself at the corners and how it cuts all the way to the outside edge of the part. This can be corrected by adjusting the Bandwidth.
Creating a Radial Cut Operation Modifying the Bandwidth Bandwidth defines the total width of the machined area measured in the plane of the boundary. The bandwidth is the sum of the Material Side and Opposite Side offset values. 1. Band Width 2. Opposite Side 3. Material Side
Choose Radial Cut under Drive Method.
513 Key in .25 for Material Side and .74 for Opposite Side.
OK to complete the Radial Cut Drive Method.
Creating a Radial Cut Operation Generating the Tool Path You will generate the tool path and observe how the modified Bandwidth effects the tool path. Generate the tool path.
The tool path no longer crosses over itself at the corners and no longer cuts all the way to the outside edge of the part. OK to complete the operation.
Creating a Radial Cut Operation Visualizing Material Removal for the Program You will graphically simulate material removal for the program.
514 In the Program Order View of the Operation Navigator, highlight the PROGRAM icon.
This chooses all of the operations in the program. Choose the Verify Toolpath icon in the toolbar. Choose the Dynamic tab. Choose the Play Forward icon.
The material removed by each successive operation is displayed in a contrasting color. OK to complete the tool path visualization. Close the part file.
515
Curve/Point Drive Method The Curve/Point drive method generates a fixed axis surface contouring tool path that follows selected points and curves. This drive method is sometimes used for engraving on contoured surfaces.
The drive path is generated from points and curves and projected onto the part surfaces where the tool path is created. The curves may be open or closed, contiguous or noncontiguous, planar or nonplanar. In this lesson, you will create a fixed axis surface contouring operation that uses the Curve/Point drive method.
Creating a Curve/Point Operation You will create a fixed axis surface contouring operation that uses the Curve/Point drive method to engrave the number "1471" on the part. You will then animate the program to graphically simulate material removal.
516
Creating a Curve/Point Operation Opening the Part Open part file srf_curve_1.prt from the srf subdirectory. Choose Application
Manufacturing.
Creating a Curve/Point Operation Beginning the Operation Choose the Create Operation icon
in the toolbar.
Choose mill_contour as the Type. The Type determines the subtype icons that are available and the groups that are initially available to choose from in the dialog. Choose FIXED_CONTOUR as the subtype.
Specify the following groups in the Create Operation dialog.
517
The WORKPIECE geometry group defines the part geometry and the blank geometry. Blank geometry is required by the Verify function to graphically simulate material removal. The operation will inherit the parameters defined by these groups. Key in engrave for the operation name.
OK to begin creating the operation.
Creating a Curve/Point Operation Defining the Drive Method The Curve/Point drive method allows you to define a tool path that follows curves projected onto contoured surfaces. Choose Curve/Point under Drive method.
OK the warning. The Curve/Point Drive Method dialog displays.
Creating a Curve/Point Operation Defining the Drive Geometry The Drive Geometry options allow you to select and edit points and curves that will be used to define the tool path. They also allow you to specify parameters such as feed rates, lifts, and cut direction. Drive geometry is projected onto part surfaces along the projection vector. 1. Drive Curves
518 2. Projection Direction 3. Tool Path 4. Part Surface
Choose Select under Drive Geometry. The order in which the curves are selected determines the sequence in which they are cut. The proximity in which each curve is selected determines the cut direction. The selected end of the curve defines the start point of the cut for that curve. 1. Selected End of Curve 2. Cut Direction of Tool
Creating a Curve/Point Operation Selecting the First Curve The tool should retract at the end of the first curve (the first "1" in 1471) and engage at beginning of the second curve. Turn the Local Lift at End option on.
Select the first curve at the upper end as illustrated below.
519
A vector indicates the cut direction.
Creating a Curve/Point Operation Selecting the Second Curve The tool should not retract at the end of the second curve, but should cut continuously to the end of the third curve. Turn the Local Lift at End option off.
Select the second curve at the upper end so the cut direction vector displays as illustrated below. You may choose Back at any time to deselect the curves one at a time if you make a mistake.
520
Creating a Curve/Point Operation Selecting the Third Curve The tool should retract at the end of the third curve and engage at beginning of the fourth curve. Turn the Local Lift at End option on.
Select the third curve so the vector displays as illustrated below.
Creating a Curve/Point Operation Selecting the Fourth Thru Seventh Curves The tool should retract at the end of the fourth curve and engage at beginning of the fifth curve. Local Lift at End should remain turned on. Select the fourth curve so the vector displays as illustrated below.
521
The tool should not retract at the end of the fifth curve, but should cut continuously to the end of the sixth curve. Turn the Local Lift at End option off. Select the fifth curve so the vector displays as illustrated below.
Turn the Local Lift at End option on and select the sixth and seventh curves.
Creating a Curve/Point Operation Selecting the Last Four Curves The tool should cut the last four curves continuously.
522 Turn the Local Lift at End option off and select curves eight through eleven at the positions indicated below so they are cut in a counterclockwise direction.
OK to complete the selections.
Creating a Curve/Point Operation Defining the Projection Vector The projection vector determines how the drive path projects from the drive geometry to the part surface. Choose Display Drive Path.
Choose Tool Axis for the Projection Vector.
OK to complete the Curve/Point drive method.
523
Creating a Curve/Point Operation Specifying a Negative Part Stock A negative stock allows you to cut below the part surface, creating a groove.
Choose Cutting. Key in -.035 for the Part Stock.
This value is the same as the radius of the tool. OK to accept the Part Stock
Defining Non-Cutting Moves Non-Cutting moves allow you to specify movements that position the tool before, after, and between cutting moves.
524
This section describes the non-cutting moves that apply to this particular operation. Refer to the non-cutting moves lesson at the end of this course for a complete discussion.
Defining Non-Cutting Moves Defining Non-Cutting Moves Choose Non-Cutting.
You will first define non-cutting moves for engages. You will then define non-cutting moves for retracts by specifying that they will use the same non-cutting moves as defined for engages.
Defining Non-Cutting Moves Defining Engages Choose the Engage icon.
525 The Case options determine whether the motion parameters will apply to all engages or only to specific types of engages. By specifying Default as the Case, all types of engages will use the same motion parameters. Be sure the Case is specified as Default.
The Status option determines the available motion parameters. For this operation, all engages will move a specified distance to the part along the tool axis. Be sure the Status is specified as Manual.
The Distance option determines the length of the engage. Turn the Distance option on and key in 0.25 .
The Movement options determine the shape of the engage. Choose Linear for the Movement.
The Direction options determine the orientation of the engage. Choose Tool Axis for the direction.
Here is how you would read the Non-Cutting Moves dialog; "Unless otherwise specified, all engages will move .25 inches in a linear direction defined by the orientation of the current tool axis".
526 Next, you will define retracts by specifying that they will use the same motion parameters as defined for engages.
Defining Non-Cutting Moves Defining Retracts Choose the Retract icon.
Notice that the Case is set to Default and the Status is set to Use Engage. All retracts (by default) will use the same parameters as defined for engages. In other words, all retracts (by default) will move from the part to the clearance plane in a linear path along the tool axis.
Defining Non-Cutting Moves Defining Departures and Approaches In this example, Approach and Departure moves are not necessary. Choose the Departure icon.
Choose None for the Departure Status.
Choose the Approach icon.
527
Choose None for the Approach Status. OK to accept the Non-Cutting Moves.
Defining Non-Cutting Moves Generating the Tool Path You will generate the tool path and observe how the tool path follows the drive geometry and incorporates the specified local lifts. Generate the tool path.
OK to complete the operation.
Defining Non-Cutting Moves Blanking the Drive Geometry You will blank the drive geometry so you can clearly observe the dynamic material removal. In the tool bar, choose Edit
Blank
Blank.
Set the Rectangle/Polygon Method to Inside and drag a rectangle around the drive geometry.
528
OK to accept the selection and blank the drive geometry.
Defining Non-Cutting Moves Visualizing Material Removal for the Program You will graphically simulate material removal for the program. In the Program Order View of the Operation Navigator, highlight the PROGRAM icon.
This chooses all of the operations in the program. Choose the Verify Toolpath icon Choose the Dynamic tab. Choose the Play Forward icon.
in the toolbar.
529
The material removed by each successive operation is displayed in a contrasting color. OK to complete the tool path visualization. Close the part file.
Spiral Drive Method The Spiral drive method generates a fixed axis surface contouring tool path that spirals outward from a specified center point.
Unlike other drive methods which require an abrupt change in direction to Stepover to the next cutting pass, the Spiral drive method Stepovers are a smooth, constant transition outward. Because this drive method maintains a constant cutting speed and smooth motion, it is useful for high speed machining applications.
530 In this lesson, you will create a fixed axis surface contouring operation that uses the Spiral drive method to finish the part. You will then Animate the operation to graphically simulate material removal.
Creating a Spiral Drive Operation You will create a fixed axis surface contouring operation that uses the Spiral drive method to finish the part. You will then Animate to graphically simulate material removal.
Creating a Spiral Drive Operation Beginning the Operation Open part file srf_spiral_1.prt from the srf subdirectory. Choose Application
Manufacturing.
Choose the Create Operation icon
in the toolbar.
Choose mill_contour as the Type. The Type determines the subtype icons that are available and the groups that are initially available to choose from in the dialog. Choose FIXED_CONTOUR as the subtype.
531
Specify the following groups in the Create Operation dialog.
The WORKPIECE geometry group defines the blank geometry required by the Verify function to graphically simulate material removal. The operation will inherit the parameters defined by these groups. Key in spiral for the operation name.
OK to begin creating the operation.
Creating a Spiral Drive Operation Defining Part Geometry The WORKPIECE group does not currently define the part geometry. You will define the part geometry within the operation. Choose the Part icon
and Select.
Select the body as illustrated below.
532
OK to accept the body as the part geometry.
Creating a Spiral Drive Operation Defining the Drive Method The Spiral drive method allows you to define a tool path that spirals outward from a specified center point. Choose Spiral under Drive method.
OK the warning. The Spiral Drive Method dialog is displayed.
Creating a Spiral Drive Operation Defining the Center Point The center point defines the center of the spiral and it is where the tool begins cutting. If you do not specify a center point, the system uses 0,0,0 of the Absolute Coordinate System. If the center point is not directly on the part surface, the point follows the projection vector to the part surface. Choose Select under Spiral Center Point. Choose the Arc/Ellipse/Sphere Center icon. Select the arc on top of the part as illustrated below.
533
Creating a Spiral Drive Operation Defining the Stepover Stepover allows you to specify the distances between successive cut passes.
Spiral drive method stepovers are a smooth, constant transition outward and do not require an abrupt change of direction. Tool Diameter allows you to define the stepover in terms of a percentage of the effective tool diameter. Choose Tool Diameter as the Stepover.
Key in 20 for the Percent.
534
Creating a Spiral Drive Operation Defining the Maximum Spiral Radius Maximum Spiral Radius allows you to limit the area to be machined. This constraint reduces processing time by limiting the number of drive points created. The radius is measured in the plane normal to the projection vector. 1. Maximum Spiral Radius 2. Part Surface
Key in 8.25 for the Max(imum) Spiral Radius.
This value is the same as the radius of the part.
Creating a Spiral Drive Operation Defining the Projection Vector The projection vector determines how the drive path projects from the plane of the center point to the part surface. The drive path you are using is much more dense than the one shown below.
535
Choose Specify Vector.
The Vector Constructor dialog displays and the current projection vector displays on the part. OK to accept this projection vector. OK to complete the Spiral drive method.
Creating a Spiral Drive Operation Generating the Tool Path You will generate the tool path and observe how the tool path spirals outward from a specified center point. Generate the tool path.
536
OK to complete the operation.
Creating a Spiral Drive Operation Visualizing Material Removal for the Operation You will graphically simulate material removal for the operation. In the Program Order View of the Operation Navigator, highlight the SPIRAL operation.
Choose the Verify Toolpath icon Choose the Dynamic tab. Choose the Play Forward icon.
in the toolbar.
537 OK to complete the tool path visualization. Close the part file.
Surface Area Drive Method The Surface Area drive method creates a wide variety of fixed and variable tool axis operations. Variable axis operations generate tool paths that can follow the contours of very complex surfaces by providing control of both the tool axis and the projection vector.
The Surface Area drive method creates an array of drive points on the drive surface and then projects them to the part surface along a specified projection vector. The tool path is created as the tool moves across the part surface from one contact point to the next. A tool path may also be created directly on the drive surface when there is no part geometry defined. In this lesson, you will create variable axis surface contouring operations using the Surface Area drive method and a variety of tool axis controls.
Examining a Program You will first examine a program consisting of operations that rough and semi-finish a part. You will then add a variable axis surface contouring operation that finishes the contoured surfaces.
538
Examining a Program Opening the Part Open part file srf_srf_area_1.prt from the srf subdirectory.
Choose the Wireframe icon
to return to a wireframe display.
Examining a Program Entering the Manufacturing Application Choose Application
Manufacturing.
In the Geometry View of the Operation Navigator, fully expand the objects as illustrated below.
539
These operations rough and semi-finish the part. They inherit parameters from the MCS and WORKPIECE groups.
Examining a Program Examining the Workpiece Group The WORKPIECE group defines the part geometry. Highlight WORKPIECE.
Choose the Display Object icon. The part geometry highlights.
Refresh the graphics display.
Examining a Program
540
Animating the Program You will animate the program to display material removal for the roughing and semi-finishing operations. In the Program Order View of the Operation Navigator, highlight PROGRAM.
This chooses all of the operations in the program. Choose the Verify Toolpath icon
in the toolbar.
Choose the Dynamic tab. Choose the Play Forward icon. Temporary blank geometry must be defined for the system to display dynamic material removal. Auto Block creates a solid body aligned with the MCS and enclosing the part geometry. Offset from Part defines blank geometry based on a specified offset distance.
OK to accept Auto Block and the default values of 0.0000.
541
OK to complete the tool path visualization.
Away From Line Tool Axis You will create a variable axis surface contouring operation that uses the Surface Area drive method and the Away From Line tool axis to finish the contoured surfaces. Away From Line defines a tool axis that diverges away from a focal line, allowing the axis to follow the general convex shape of the part geometry while not undulating excessively.
Away From Line Tool Axis Beginning the Operation Choose the Create Operation icon. Choose mill_multi-axis as the Type. The Type determines the subtype icons that are available and the groups that are initially available to choose from in the dialog. Choose VARIABLE_CONTOUR as the subtype.
542
This option is the most generic of the multi-axis subtypes and will allow you to create a wide variety of operations. The system automatically names the operation VARIABLE_CONTOUR. Specify the following groups in the Create Operation dialog.
The operation will inherit the parameters defined by these groups. OK to begin creating the operation.
Away From Line Tool Axis Defining Part Geometry This operation does not inherit part geometry from the WORKPIECE group. You will define the part geometry within the operation. Choose the Part icon
and Select.
Choose Features as the Selection Option.
Select the Surface Region as illustrated below.
543
More About Surface Regions
Surface Regions (Tools Prepare Geometry Surface Region) are CAM features that contain faces on a single solid body or sheet. The ability to select a single entity makes the specification of Part and Blank geometry very easy. Surface Regions are also easy to identify and select as features using the Model Navigation Tool. Surface Regions are associative to the solid. That is, when you modify the solid, the associated Surface Regions update automatically to match the solid. Surface Regions are created by selecting faces of a body. All faces of a Surface Region Feature must be on the same body. Three methods of defining Surface Regions (Seed, All Faces, and Selected Faces) are available in the Surface Regions dialog box under Region Type. To summarize, the purpose of creating Surface Regions is to organize the areas to be machined, to make the selection of Part and Blank Geometry easier by enabling you to use the Surface Region selection method, and to establish associativity with bodies. OK to accept the surface region as the part geometry.
Away From Line Tool Axis Defining Check Geometry Check geometry will prevent the tool from gouging the planar face. Choose the Check icon
and Select.
544 Choose Faces as the Filter Method.
Select the planar face as illustrated below.
OK to accept the face as the check geometry.
Away From Line Tool Axis When Gouging Check Geometry The When Gouging option allows you to specify how the system will respond when the tool gouges Check geometry during cutting moves. Choose Cutting. Choose Skip for When Gouging.
Warning causes the system to issue only a warning message and does not alter the tool path
545 Skip causes the tool to omit the tool positions which gouge the Check Geometry. Retract causes the tool to avoid gouging the Check Geometry by using the Check Engage and Retract parameters defined in Non-Cutting moves. Check Safe Clearance defines an extended safety zone for check geometry which cannot be violated by the tool or the tool holder.
Be sure a value of 0.1000 is specified for Check Safe Clearance. OK to accept the Cutting Parameters.
Away From Line Tool Axis Defining the Drive Method The Surface Area drive method allows you to define a variable tool axis. Choose Surface Area under Drive Method.
OK the warning. The Surface Drive Method dialog displays.
Away From Line Tool Axis Defining the Drive Geometry You will select the bottom face of the part as the drive geometry. This is the face on which the array of drive points will be created. Choose Select under Drive Geometry.
546 Select the planar face on the bottom of the part.
OK to accept the drive geometry. Two vectors display, one defining the default drive direction and other defining the Material Side of the drive geometry.
When machining part surfaces as in this example, the Projection Vector (which you have not yet defined) determines which side of the surface the tool contacts and the Material Side vector has no effect.
Away From Line Tool Axis Defining the Cut Direction Cut Direction allows you to specify the direction of the first cut and the quadrant where the first cut will begin.
547 Choose Cut Direction. Select the vector illustrated below.
The Surface Drive Method dialog displays.
Away From Line Tool Axis Defining the Stepover Stepover controls the distance between successive Cut Passes. Choose Scallop as the Stepover.
Scallop Height is the maximum allowable height measured normal to the Drive Surface.
548
Key in 0.0100 for the Scallop Height.
Choose Display Drive Path to verify that drive points and a zig-zag drive path are defined on the drive geometry.
Refresh the graphics display. More About Stepover
Stepover controls the distance between successive Cut Passes. You may specify the Stepover in terms of the scallop size or the total number of Stepovers. The Stepover options vary depending on the Cut Type used.
549
Scallop allows you to specify the maximum allowable size of Scallops by specifying values for height, horizontal, and vertical distances. This method is useful for good Scallop Height Control when the Drive Surface is also used as the Part Surface. The system limits the size of the stepover to roughly less than two-thirds of the tool diameter regardless of what you specify as the scallop size. Scallop Height is the maximum allowable height measured normal to the Drive Surface. Horizontal Limit allows you to restrict the distance a tool may move in a direction normal to the Projection Vector. This option helps you avoid leaving wide ridges on near vertical surfaces by limiting the horizontal distance of the Stepover. Vertical Limit allows you to restrict the distance a tool may move in a direction parallel to the Projection Vector. This option helps you avoid leaving wide ridges on near vertical surfaces by limiting the vertical distance of the Stepover. Horizontal Limit and Vertical Limit may be used together, separately, or not at all. If the values are set to zero, then they are not used. Number allows you to specify the total number of Stepovers for the Tool Path. If the Cut Type you select is Follow Pocket, enter the Number of Stepovers for the First Direction (i.e., cut direction) and for the Second Direction (i.e., Stepover direction).
Away From Line Tool Axis Defining the Projection Vector The projection vector determines how the drive points project to the part geometry and the side of the part geometry the tool contacts. Choose Specify Vector under Projection Vector.
550
The Vector Constructor dialog is displayed. OK to accept the default I,J,K values of 0,0,-1. A vector pointing in the negative ZM direction displays.
Drive points always project from the drive geometry to the part geometry. The angle of the vector determines the path along which the drive points project. For this part, the drive points project upward from the drive geometry (bottom face of the part) to the part geometry along the ZM axis. The positive vs. negative direction of the arrowhead does not matter. The side of the part geometry the tool contacts is determined by the direction of the projection vector. The tool always positions to the part geometry on the side the Projection Vector approaches. For this part, the arrowhead must point downward (as it currently does) so that the tool approaches and positions on the part geometry from the top.
More About Projection Vector
Projection Vector enables you to define how the Drive Points project to the Part Surface, and the side of the Part Surface the tool contacts. The Drive Points project along the Projection Vector to the Part Surface. Sometimes, as illustrated below, Drive Point project in the opposite direction of the Projection Vector (but still along the vector axis) as they move from the Drive Surface to the Part Surface. The direction of the Projection Vector determines the side of the Part Surface the tool contacts. The tool always positions to the Part Surface from the side the Projection Vector
551 approaches. In the following figure, drive point p1 projects to the Part Surface in the opposite direction of the Projection Vector to create p2. 1. Projection Vector 2. Part Surface 3. Drive Surface
The types of Projection Vectors available depend upon the Drive Method. The Projection Vector option is common to all Drive Methods except Flow Cut. The following figure illustrates another example of how the Drive Points project to the Part Surface. In this example, the Projection Vector is defined as Fixed. The vector is parallel to the ZM axis at any given point on the Part Surface. To reach the Part Surface, the Drive Points must project from the Boundary Plane in the same direction as the Projection Vector arrowhead. 1. 2. 3. 4.
Drive Boundary Projection Vector Part Surface Drive Path Projection
The direction of the Projection Vector determines the side of the Part Surfaces the tool contacts. 1. Projection Vector 2. Part Surface
552 3. Drive Surface 4. Tool Side of Part Surface
The following figures illustrate how the direction of the Projection Vector determines which side of the Part Surfaces the tool contacts. In each figure, the tool contacts the same Part Surface (inside the cylinder), but the contact side differs depending on the direction of the Projection Vector. The Projection Vector illustrated below, Towards Line, yields undesirable results. The tool follows the direction of the Projection Vector and approaches the Part Surface from the outside of the cylinder and gouges the part. 1. 2. 3. 4.
Part Surface Drive Surface Projection Vector Tool Gouges Part
The Projection Vector illustrated below, Away From Line, yields the desired results. The tool follows the direction of the Projection Vector and approaches the Part Surface from the inside of the cylinder and does not gouge the part. 1. 2. 3. 4.
Part Surface Drive Surface Projection Vector Tool Does Not Gouge Part
553
When using Away From Point or Away From Line as the Projection vector, the minimum distance from the Part Surface to the vector focal point or line must be greater than the radius of the tool as illustrated below. The tool end must be allowed to position to the projection vector focal point or anywhere along the projection vector focal line without gouging the Part Surface. 1. 2. 3. 4. 5. 6.
Tool Path Part Surface Drive Surface Distance Greater than Tool Radius Projection Vector Away from Line Projection Vector Focal Line
If the tool gouges the Part Surface when the tool end is positioned at the focal point or anywhere along the focal line as illustrated below, the system cannot guarantee a good tool path. 1. 2. 3. 4. 5. 6.
Gouge Part Surface Drive Surface Distance Less than Tool Radius Projection Vector Away from Line Projection Vector Focal Line
554
Away From Line Tool Axis Defining the Away From Line Tool Axis The Tool Axis is a vector that points away from the tip of the tool and toward the tool holder.
A variable tool axis constantly changes orientation as it moves along the tool path. The method you use to control the orientation of the tool axis depends to a large extent on the shape of the part you are machining. For this part, a fixed tool axis would cause the tool to plunge straight down along the vertical sides.
By contrast, a tool axis that is normal to the part surface would cause excessive tool undulations.
555
This part requires a tool axis that follows the general convex shape of the part geometry while not undulating excessively. Away From Line defines a variable tool axis that diverges away from a focal line. The tool axis hinges on the line as it travels along the length and remains normal to the line.
Choose Away From Line under Tool Axis. You might need to scroll up in the dialog to see this option.
The Line Definition dialog is displayed. Choose Two Points. Choose the Control Point icon. Select the two control points illustrated below.
556
OK to accept the line definition. OK to complete the Surface Area drive method.
Away From Line Tool Axis Generating the Tool Path You will generate the tool path and then replay it to observe how the tool axis follows the general convex shape of the part while preventing excessive tool undulations. Generate the tool path.
Choose the Shaded icon surfaces. Choose the Verify icon
in the toolbar so you can clearly see the contoured part
at the bottom of the dialog.
The Toolpath Visualization dialog displays with the Replay tab chosen.
557 Choose the Play Forward icon.
OK to complete the tool path visualization. OK to complete the operation. Close the part file.
Normal to Drive Tool Axis You will create a variable axis surface contouring operation that uses the Surface Area drive method and the Normal to Drive tool axis to finish the contoured part surfaces. Normal to Drive defines a tool axis perpendicular to the drive surface, allowing the axis to follow the general convex shape of the part geometry while not undulating excessively.
Normal to Drive Tool Axis Opening the Part Open part file srf_srf_area_2.prt from the srf subdirectory.
558 This part is the same as the one used in the previous section with the addition of a surface that will be used as drive geometry. Choose Application
Manufacturing.
Normal to Drive Tool Axis Beginning the Operation Choose the Create Operation icon in the toolbar. In the Create Operation dialog, choose mill_multi-axis as the Type. Choose VARIABLE_CONTOUR as the subtype. The system automatically names the operation VARIABLE_CONTOUR. Specify the following groups in the Create Operation dialog.
The operation will inherit the parameters defined by these groups. OK to begin creating the operation.
Normal to Drive Tool Axis Defining Part Geometry This operation does not inherit part geometry from the WORKPIECE group. You will define the part geometry within the operation.
559
Choose the Part icon
and Select.
Choose Features as the Selection Option. Select the Surface Region as illustrated below.
OK to accept the surface region as the part geometry. The VARIABLE_CONTOUR dialog displays.
Normal to Drive Tool Axis Defining the Drive Method The Surface Area drive method allows you to define a variable tool axis. Choose Surface Area under Drive method.
OK the warning.
Normal to Drive Tool Axis Defining the Drive Geometry
560 The drive geometry will define the drive points and will control the tool axis. Choose Select under Drive Geometry. Select the curved surface above the part.
OK to accept the drive geometry. Two vectors display, one defining the default drive direction and other defining the Material Side of the drive geometry.
Normal to Drive Tool Axis Defining the Projection Vector Projection Vector determines how the drive points project to the part geometry and the side of the part surface the tool contacts.
561 Choose Normal to Drive under Projection Vector. Normal to Drive allows you to define the projection vector relative to the drive surface normals. The side of the part geometry the tool contacts is determined by the direction of the projection vector. The tool always positions to the part geometry on the side of the part geometry the projection vector approaches. For this part, the projection vector must point inward toward the part geometry as illustrated below for the tool to position correctly.
When using Normal to Drive, the projection vector is calculated as the inverse of the material side vector. This means that the projection vector currently points outward away from the part geometry and not inward as it should. Refresh the graphics display to remove the vectors. Choose Flip Material. This reverses the direction of the material side vector.
The projection vector, calculated as the inverse of the material side vector, now points inward toward the part geometry as it should. The tool will therefore position to the part geometry along the projection vector.
562
Normal to Drive Tool Axis Defining the Cut Direction Cut Direction allows you to specify the direction of the first cut and the quadrant where the first cut will begin. Choose Cut Direction. A set of vectors is displayed, showing all possible vectors tangent to the drive surface edges. Choose the vector illustrated below.
The Surface Drive Method dialog displays.
Normal to Drive Tool Axis Defining the Stepover Stepover controls the distance between successive Cut Passes. Choose Number as the Stepover.
Number of Steps defines the total number of stepovers for the tool path.
563 Key in 50 for the Number of Steps.
Choose Display Drive Path to verify that drive points and a zig-zag drive path are defined on the drive geometry.
Refresh the graphics display.
Normal to Drive Tool Axis Defining the Normal to Drive Tool Axis This part requires a tool axis that follows the general convex shape of the part geometry while not undulating excessively. Normal to Drive defines a variable tool axis perpendicular to the drive surface at each the drive point. 1. Tool Axis 2. Drive Surface 3. Part Surface
564 Choose Normal to Drive under Tool Axis.
OK to complete the Surface Area drive method.
Normal to Drive Tool Axis Generating the Tool Path You will generate the tool path and observe how the tool axis follows the drive geometry. Generate the tool path.
Choose the Shaded icon in the toolbar so you can clearly see the contoured part surfaces. Choose the Verify icon at the bottom of the dialog. The Toolpath Visualization dialog displays with the Replay tab chosen. If the drive geometry does not appear translucent as illustrated below, choose Preferences Visualization Visual (tab) and turn on Translucency. Choose the Play Forward icon.
565
It is difficult to tell by looking at the tool path whether or not the tool gouges the part. Defining check geometry can help. OK to complete the tool path visualization.
Normal to Drive Tool Axis Defining Check Geometry Check Geometry can be defined and warnings generated if the tool violates the check geometry. Choose the Check icon
and Select.
Choose Faces as the Filter Method.
Select the planar face as illustrated below.
566
OK to accept the face as the check geometry.
Normal to Drive Tool Axis When Gouging Check Geometry The When Gouging option allows you to specify how the system will respond when the tool gouges check geometry during cutting moves. Choose Cutting. Choose Warning for When Gouging. Warning causes the system to issue only a warning message and does not alter the tool path. OK to accept the Cutting Parameters. Generate the tool path. When the tool path is complete, the following message displays warning you that the check geometry is violated by the tool.
OK to dismiss the message. If you wish, you may specify Skip for the When Gouging option to omit the tool positions that gouge the check geometry and then regenerate the tool path. OK to complete the operation. Close the part file.
567
Normal to Drive Tool Axis You will create a variable axis surface contouring operation that uses the Surface Area drive method and the Normal to Drive tool axis to finish the contoured surface while avoiding the blades.
Normal to Drive defines a tool axis perpendicular to the drive geometry. In this operation, you will define only the drive geometry. You will not define part geometry. As a result, the tool path will be created directly on the drive geometry and definition of a projection vector will not be necessary.
Normal to Drive Tool Axis Opening the Part Open part file srf_srf_area_3.prt from the srf subdirectory. Choose Application
Manufacturing.
Normal to Drive Tool Axis Beginning the Operation
568 Choose the Create Operation icon in the toolbar. In the Create Operation dialog, choose mill_multi-axis as the Type. Choose VARIABLE_CONTOUR as the subtype. The system automatically names the operation VARIABLE_CONTOUR. Specify the following groups in the Create Operation dialog.
The operation will inherit the parameters defined by these groups. OK to begin creating the operation.
Normal to Drive Tool Axis Defining the Drive Method ChooseSurface Area under Drive Method.
OK the warning. The Surface Drive Method dialog displays.
Normal to Drive Tool Axis Defining the Drive Geometry You will define the drive geometry by selecting a single drive surface. Choose Select under Drive Geometry.
569 Select the face illustrated below.
OK to complete the drive geometry. Two vectors display; one defining the default drive direction and other defining the material side of the drive geometry. Rotate the view so you can see these arrows clearly. 1. Drive Direction 2. Material Side
The material side vector determines the side the tool will contact when cutting directly on the drive surface. This vector should point towards the material to be removed (away from the part). It currently points away from the material to be removed and must be reversed. Choose Flip Material. This reverses the direction of the material side vector.
570
Refresh the graphics display and then MB3
Restore to change back to a TFR-ISO view.
Normal to Drive Tool Axis Defining the Cut Direction Cut Direction allows you to specify the direction of the first cut and the quadrant where the first cut will begin. Choose Cut Direction.
Choose the vector illustrated below.
Normal to Drive Tool Axis Defining the Stepover Stepover controls the distance between successive cut passes.
571 Choose Scallop as the Stepover.
Scallop Height is the maximum allowable height measured normal to the Drive Surface. Key in 0.0100 for the Scallop Height.
Choose Display Drive Path to verify that drive points and a zig-zag drive path are defined on the drive geometry.
Refresh the graphics display.
Normal to Drive Tool Axis Defining the Normal to Drive Tool Axis This part requires a tool axis that follows the contour of the drive geometry. Normal to Drive defines a variable tool axis perpendicular to the drive surface at each drive point.
572
Choose Normal to Drive under Tool Axis.
Normal to Drive Tool Axis When Gouging Drive Surfaces The When Gouging option allows you to specify how the system will respond when the tool gouges drive surfaces during cutting moves. These options apply only when you are cutting directly on drive surfaces and not when you are cutting on part surfaces. When Gouging also appears in the Cutting Parameters dialog. In that dialog, the options determine how the system responds when the tool gouges check geometry. Warning causes the system to issue only a warning message and does not alter the tool path Skip causes the system to alter the tool path by removing only the drive points that cause the gouging to occur. Retract causes the tool to avoid gouging the Drive Surface by using the parameters defined in Non-Cutting Moves. Choose Skip for When Gouging.
573
OK to complete the Surface Area drive method. More About When Gouging Drive Surfaces
The When Gouging option allows you to specify how the system will respond when the tool gouges the Drive Surface during cutting moves. These options only apply when you are cutting to Drive Surfaces and not when you are cutting to Part Surfaces. None causes the system to ignore Drive Surface gouging. It will generate the same unaltered tool path as the Warning option, but will not issue a warning message to the tool path or CLSF.
Skip causes the system to alter the tool path by removing only the Drive Points that cause gouging to occur. The result is a straight tool movement from the last position before gouging to the first position which is no longer gouging. When generating tool paths directly from Drive Surface, the tool does not violate the Drive Surface at convex corners, and does not gouge concave regions when using Skip as illustrated below.
In some cases where the drive surface is smoothly concave, the Skip option may not clean up the tool path as well as illustrated in the concave corner case above. Retract causes the tool to avoid gouging the Drive Surface by using the parameters defined in Non-Cutting Moves.
Normal to Drive Tool Axis Defining Check Geometry
574 Check geometry will prevent the tool from gouging the blades. You will define the check geometry by selecting the three faces on each blade. Choose the Check icon
and Select.
The Check Geometry dialog displays. Choose Faces as the Filter Method.
Select the three faces that define the first blade as illustrated below.
Select the three faces that define the second blade as illustrated below.
OK to accept the faces as check geometry.
575 The Variable Contour dialog displays.
Normal to Drive Tool Axis When Gouging Check Geometry The When Gouging option allows you to specify how the system will respond when the tool gouges check geometry during cutting moves. Choose Cutting. Choose Retract for When Gouging.
Retract causes the tool to avoid gouging the check geometry by using the Check, Engage, and Retract parameters defined in Non-Cutting moves. Check Safe Clearance defines an extended safety zone for check geometry which cannot be violated by the tool or the tool holder.
Be sure a value of 0.1000 is specified for Check Safe Clearance. OK to accept the Cutting Parameters.
Normal to Drive Tool Axis Defining Non-Cutting Moves Non-Cutting moves allow you to specify movements that position the tool before, after, and between cutting moves.
576 This section describes the non-cutting moves that apply to this particular operation. Refer to the non-cutting moves lesson at the end of this course for a complete discussion. Choose Non-Cutting.
You will first define non-cutting moves for engages. You will then define non-cutting moves for retracts by specifying that they will use the same non-cutting moves as defined for engages.
Normal to Drive Tool Axis Defining Engages Choose the Engage icon.
The Case options determine whether the motion parameters will apply to all engages or only to specific types of engages. By specifying Default as the Case, all types of engages will use the same motion parameters. Be sure the Case is specified as Default. The Status option determines the available motion parameters. For this operation, all engages will move a specified distance to the part along the tool axis. Choose Manual for the Status.
The Distance option determines the length of the engage. Turn the Distance option on and key in 1.5.
577
The Movement options determine the shape of the engage. Choose Linear for the Movement.
The Direction options determine the orientation of the engage. Choose Tool Axis for the direction.
Here is how you would read the Non-Cutting Moves dialog; "Unless otherwise specified, all engages will move 1.5 inches in a linear direction defined by the orientation of the current tool axis". Next, you will define retracts by specifying that they will use the same motion parameters as defined for engages.
Normal to Drive Tool Axis Defining Retracts Choose the Retract icon.
Notice that the Case is set to Default and the Status is set to Use Engage. All retracts (by default) will use the same parameters as defined for engages. In other words, all retracts (by default) will move from the part to the clearance plane in a linear path along the tool axis. OK to accept the Non-Cutting Moves.
Normal to Drive Tool Axis
578
Generating the Tool Path You will generate the tool path and observe how the tool axis follows the contours of the drive geometry while avoiding the check geometry. Generate the tool path.
Choose the Shaded icon in the toolbar so you can clearly see the contoured part surfaces. Choose the Verify icon at the bottom of the dialog. The Toolpath Visualization dialog displays with the Replay tab chosen. Choose the Play Forward icon.
OK to complete the tool path visualization. OK to complete the operation. Close the part file.
Swarf Drive Tool Axis You will create two variable axis surface contouring operations that uses the Surface Area drive method and the Swarf Drive tool axis to finish the blades.
579 You will create the first operation by specifying all the necessary parameters to finish the first blade.
You will create the second operation by copying the first operation and then respecifying the drive geometry to finish the second blade. Swarf Drive defines a tool axis that follows the swarf rulings of drive surfaces. The side of the tool cuts along the drive surfaces and the tip of the tool cuts along the part surfaces.
Swarf Drive Tool Axis Opening the Part Open part file srf_srf_area_4.prt from the srf subdirectory. Choose Application
Manufacturing.
Swarf Drive Tool Axis Beginning the Operation Choose the Create Operation icon in the toolbar. In the Create Operation dialog, choose mill_multi-axis as the Type. Choose VARIABLE_CONTOUR as the subtype.
580 Specify the following groups in the Create Operation dialog.
The operation will inherit the parameters defined by these groups. Key in swarf for the operation name.
OK to begin creating the operation.
Swarf Drive Tool Axis Defining the Drive Method Choose Surface Area under Drive Method.
OK the warning. The Surface Drive Method dialog displays.
Swarf Drive Tool Axis Defining the Drive Geometry You will define the drive geometry by selecting the three faces on the first blade. Choose Select under Drive Geometry. The Drive Geometry dialog displays. Select the three faces that define the blade in order as illustrated below.
581 Drive surfaces must be selected in order and must be edge-to-edge.
OK to complete the drive geometry. Two vectors display; one defining the material side of the drive geometry and other defining the default drive direction.
The material side vector determines the side the tool will contact when cutting directly on the drive surface. This vector should point towards the material to be removed (away from the part) as it currently does. The currently displayed drive direction vector will cause the tool to cut along the drive surfaces in the direction indicated below.
582
Refresh the graphics display.
Swarf Drive Tool Axis Defining the Swarf Drive Tool Axis This part requires a tool axis that cuts along the sides of the blades. Swarf Drive defines a variable tool axis that allows the side of the tool to cut along the drive surfaces by following the swarf rulings. The tip of the tool cuts along the part surfaces. 1. Part Surface 2. Drive Surface 3. Swarf Ruling Direction
Choose Swarf Drive under Tool Axis.
583
Four directional vectors appear relative to the first drive surface you selected. The vector you select defines the swarf ruling direction that the tool axis will follow. The vector you select should point toward the tool holder. Rotate the view so you can see these vectors clearly. Choose the vector illustrated below.
Refresh the graphics display and change back to a TFR-ISO view.
Swarf Drive Tool Axis Defining the Projection Vector The projection vector determines how the drive points project to the part geometry. Choose Tool Axis under Projection Vector.
584
Swarf Drive Tool Axis Defining the Stepover The cut type (Zig-Zag, Zig, Follow Pocket, etc.) has no effect on the Swarf Drive tool axis. To produce a single pass, the number of stepovers must be set to zero. If the number of stepovers is greater than zero, the system will produce multiple passes. Choose Number as the Stepover. Key in 0 for the Number of Steps.
Swarf Drive Tool Axis When Gouging Drive Surfaces The When Gouging option allows you to specify how the system will respond when the tool gouges drive surfaces during cutting moves. When Gouging also appears in the Cutting Parameters dialog. In that dialog, the options determine how the system responds when the tool gouges check geometry. Skip causes the system to alter the tool path by removing only the drive points that cause the gouging to occur. Choose Skip for When Gouging.
OK to complete the Surface Area drive method. More About When Gouging Driving Surfaces
The When Gouging option allows you to specify how the system will respond when the tool gouges the Drive Surface during cutting moves. These options only apply when you are cutting to Drive Surfaces and not when you are cutting to Part Surfaces.
585 None causes the system to ignore Drive Surface gouging. It will generate the same unaltered tool path as the Warning option, but will not issue a warning message to the tool path or CLSF.
Skip causes the system to alter the tool path by removing only the Drive Points that cause gouging to occur. The result is a straight tool movement from the last position before gouging to the first position which is no longer gouging. When generating tool paths directly from Drive Surface, the tool does not violate the Drive Surface at convex corners, and does not gouge concave regions when using Skip as illustrated below.
In some cases where the drive surface is smoothly concave, the Skip option may not clean up the tool path as well as illustrated in the concave corner case above. Retract causes the tool to avoid gouging the Drive Surface by using the parameters defined in Non-Cutting Moves.
Swarf Drive Tool Axis Defining Part Geometry The part geometry guides the tip of the tool. Choose the Part icon
and Select.
Choose Faces as the Filter Method. Select the face as illustrated below.
586
OK to accept the face as the part geometry.
Swarf Drive Tool Axis Generating the Tool Path You will generate the tool path and observe how the SWARF operation finishes the first blade. Generate the tool path.
Choose the Shaded icon in the toolbar so you can clearly see the contoured part surfaces. Choose the Verify icon at the bottom of the dialog. Choose the Play Forward icon.
587
OK to complete the tool path visualization. OK to complete the operation. Choose the Wireframe icon to return to a wireframe display.
Swarf Drive Tool Axis Copying the Operation You will finish the second blade by copying the existing SWARF operation and respecifying the drive geometry. This will be easier than creating a new operation. In the Program Order View of the Operation Navigator, highlight the SWARF operation and MB3 Copy.
MB3
Paste to copy the operation.
SWARF_COPY now appears as the last operation in the Program Order View.
588
Swarf Drive Tool Axis Editing the Drive Geometry You will respecify the drive geometry so that this operation machines the second blade. Double-click on the SWARF_COPY icon to edit the operation. Choose Surface Area under Drive Method. You will define the drive geometry by selecting the three faces on the second blade. Choose Reselect under Drive Geometry. OK the warning Select the three faces that define the second blade as illustrated below. Drive surfaces must be selected in order and must be edge-to-edge.
OK to complete the drive geometry. The Surface Drive Method dialog displays. OK to complete the Surface Area drive method.
Swarf Drive Tool Axis Generating the Tool Path You will generate the tool path and observe how the SWARF_COPY operation finishes the second blade.
589 Generate the tool path.
Choose the Shaded icon in the toolbar so you can clearly see the contoured part surfaces. Choose the Verify icon at the bottom of the dialog. The Toolpath Visualization dialog displays with the Replay tab chosen. Choose the Play Forward icon.
OK to complete the tool path visualization. OK to complete the operation. Close the part file.
Instancing an Operation Instancing allows you to make multiple copies of the tool path while maintaining a link to the original operation. Editing one instance automatically updates all instances.
590 This is especially useful when the part has not been fully modeled and uses a callout to specify that certain features are repeated.
Instancing an Operation Opening the Part You will create five instances of an operation that finishes one of the blades. Open part file srf_srf_area_5.prt from the srf subdirectory.
Choose Application
Manufacturing.
Instancing an Operation Replaying the Tool Path You will replay the tool path and observe how the SWARF operation finishes the blade.
591 In the Program Order View of the Operation Navigator, highlight the SWARF operation and MB3 Replay.
Instancing an Operation Creating Instances You will create five instances of the operation by rotating it about the centerline in 60 degree increments. In the Program Order View of the Operation Navigator, highlight the SWARF operation icon and MB3 Object Transform. Choose Rotate About Line. Choose Existing Line. Select the centerline of the part.
Key in 60 for the Angle and OK to accept it. Choose Multiple Instances. Key in 5 for the Number and OK to accept it.
592 The instances display temporarily for visual verification.
Choose Accept to complete the instances. Notice that five additional operations named "Instance" are created.
Each instance is linked to the original operation. Unlike copies, modifying any instance will automatically update all associated instances.
Instancing an Operation Editing an Instance You will edit one of the instances and observe how all five associated instances automatically update. Double-click on the SWARF_INSTANCE_2 icon to edit the operation. A warning displays informing you that all associated instances will be edited. OK the warning.
593 Choose Method:MILL_FINISH and Reselect.
Set the Method option to MILL_SEMI_FINISH and OK. OK to complete the operation. Notice that all of the instances as well as the original operation have been edited and must now be regenerated.
Instancing an Operation Generating the Tool Path You will generate the sequence of operations and then visualize the tool paths. Highlight the Program icon and MB3
Generate.
OK for each operation. Choose the Shaded icon in the toolbar. Choose the Verify Toolpath icon in the toolbar. The Toolpath Visualization dialog displays with the Replay tab chosen. Choose the Play Forward icon.
594
OK to complete the tool path visualization. Close the part file.
Normal to Part Tool Axis You will create a variable axis surface contouring operation that uses the Surface Area drive method and the Normal to Part tool axis to finish the contoured surfaces. Normal to Part defines a tool axis that is normal to the part geometry.
Normal to Part Tool Axis Opening the Part Open part file srf_srf_area_6.prt from the srf subdirectory.
595
Choose Application
Manufacturing.
Normal to Part Tool Axis Beginning the Operation Choose the Create Operation icon in the toolbar. In the Create Operation dialog, choose mill_multi-axis as the Type. Choose VARIABLE_CONTOUR as the subtype. The system automatically names the operation VARIABLE_CONTOUR. Specify the following groups in the Create Operation dialog.
The operation will inherit the parameters defined by these groups. OK to begin creating the operation.
Normal to Part Tool Axis Defining Part Geometry This operation inherits the part geometry from the WORKPIECE group. Choose the Part icon
and Display.
Part surfaces (unlike drive surfaces) do not need to be arranged in an orderly grid of rows and columns.
596
Normal to Part Tool Axis Defining the Drive Method The Surface Area drive method allows you to define a variable tool axis. Choose Surface Area under Drive method.
OK the warning.
Normal to Part Tool Axis Defining the Drive Geometry Drive geometry defines the drive points that are projected to the part surfaces. Choose Select under Drive Geometry. Select the bottom face of the part.
597
OK to accept the drive geometry. Two vectors display, one defining the default drive direction and other defining the material side of the drive geometry.
The material side vector determines which side of the surface the tool contacts only when machining directly on drive surfaces. When machining on part surfaces as in this example, the projection vector (not the material side vector) determines the side of the surface the tool contacts. The material side vector therefore has no effect on this operation.
Normal to Part Tool Axis Defining the Projection Vector Projection Vector determines how the drive points project to the part geometry and the side of the part geometry the tool contacts.
598 Choose Specify Vector under Projection Vector.
The side of the part geometry the tool contacts is determined by the direction of the projection vector. The tool always positions to the part geometry on the side that the projection vector approaches. For this part, the projection vector must point in a downward direction so that the tool positions to the part geometry from the top. Be sure that the I,J,K values in the Vector Constructor dialog are 0,0,-1.
Drive points always project along the vector to the part geometry. In this case, the points project along the vertical vector but up from the bottom of the part in the opposite direction of the arrowhead. OK to accept the projection vector.
Normal to Part Tool Axis Defining the Cut Direction Cut Direction allows you to specify the direction of the first cut and the quadrant where the first cut will begin. Choose Cut Direction. Choose the vector illustrated below.
599
Refresh the graphics display.
Normal to Part Tool Axis Defining the Stepover Stepover controls the distance between successive Cut Passes. Choose Scallop as the Stepover.
Scallop Height is the maximum allowable height measured normal to the Drive Surface. Be sure the Scallop Height is 0.0050. Choose Display Drive Path to verify that drive points and a zig-zag drive path are defined on the drive geometry.
600
Refresh the graphics display.
Normal to Part Tool Axis Defining the Normal to Part Tool Axis Normal to Part defines a tool axis perpendicular to the part surfaces, allowing the axis to follow the contours of the part geometry.
Choose Normal to Part under Tool Axis.
OK to complete the Surface Drive Method.
601
Normal to Part Tool Axis Generating the Tool Path You will generate the tool path and observe how the tool axis follows the contours of the part geometry. Generate the tool path.
Choose the Shaded icon in the toolbar so you can clearly see the contoured part surfaces. Choose the Verify icon at the bottom of the dialog. The Toolpath Visualization dialog displays with the Replay tab chosen. Choose the Play Forward icon.
OK to complete the tool path visualization. OK to complete the operation. Close the part file.
602
Relative to Part Tool Axis You will define a Relative to Part tool axis by editing a Variable Contour operation containing a Normal to Part tool axis. Relative to Part defines a tool axis leaning forward or backward, or tilting to the right or left of an otherwise normal tool axis relative to the part surfaces. The Lead angle leans the tool forward or backward relative to the cut direction.
Open part file srf_srf_area_7.prt from the srf subdirectory. Choose Application
Manufacturing.
Relative to Part Tool Axis Editing the Operation In the Program Order View of the Operation Navigator, double-click on the VARIABLE_CONTOUR icon to edit the operation.
This operation uses Normal to Part as the tool axis and is similar to the operation you created in the previous section.
Relative to Part Tool Axis Defining the Relative to Part Tool Axis Relative To Part defines a tool axis leaning forward or backward, or tilting to the right or left of an otherwise normal tool axis relative to the part surfaces.
603 Lead Angle defines the angle of the tool forward or backward along the tool path. Tilt Angle defines the angle of the tool side to side. 1. 2. 3. 4.
Negative Tilt Positive Tilt Lead (positive) Lag (negative)
Choose Relative to Part under Tool Axis.
Relative to Part Tool Axis Defining the Lead A positive lead angle leans the tool forward from the normal axis orientation based on the direction of the tool path. A negative lead angle (lag) leans the tool backward based on the direction of the tool path. The minimum and maximum lead values define how far the tool can deviate from the specified lead angle. 1. 20 Degree Lead (forward angle) 2. Max Lead (25 degrees) 3. Min Lead (15 degrees)
604
Key in the following values for Lead, Minimum Lead, and Maximum Lead.
Leave the Tilt values set to zero for now. OK to accept the values.
Relative to Part Tool Axis Generating the Tool Path You will generate the tool path and observe how the Relative to Part tool axis maintains the specified lead angle. Generate the tool path.
605
Relative to Part Tool Axis Visualizing the Tool Path Reorient to a Front view (MB3
Orient View
Front).
Choose the Shaded icon in the toolbar so you can clearly see the contoured part surfaces. Choose the Verify icon at the bottom of the dialog. The Toolpath Visualization dialog displays with the Replay tab chosen. Choose the Play Forward icon. A positive lead angle leans the tool forward based on the direction of the cutting pass. This is why the lead flips direction as the tool alternates between zig and zag cuts.
OK to complete the tool path visualization. OK to complete the operation. Close the part file.
4-Axis Normal to Part Tool Axis You will define a 4-Axis Normal to Part tool axis by editing a Variable Contour operation containing a Normal to Part tool axis. 4-Axis Normal to Part defines a tool axis that uses a rotation angle and a rotation axis. The rotation angle allows the tool to rotate about the rotation axis while remaining normal to the
606 axis. Unlike a lead angle, a rotation angle leans the tool to the same side of the normal tool axis regardless of the zig or zag cut direction. 1. Rotation Angle 2. Tilt
Open part file srf_srf_area_7.prt from the srf subdirectory. Choose Application
Manufacturing.
4-Axis Normal to Part Tool Axis Editing the Operation In the Program Order View of the Operation Navigator, double-click on the VARIABLE_CONTOUR icon to edit the operation.
This operation uses Normal to Part as the tool axis. You will change this to a 4-Axis Normal to Part tool axis.
4-Axis Normal to Part Tool Axis Defining the 4-Axis Normal to Part Tool Axis 4-Axis Normal to Part defines a tool axis that uses a rotation angle and a rotation axis. In the left view illustrated below, the rotation angle causes the tool axis to lean to the right of the normal tool axis in both the zig and zag moves. The tool moves within parallel planes normal to the rotation axis. 1. Part Surface Normal 2. Rotation Angle
607 3. Plane Normal to Rotation Axis 4. Axis Parallel to Plane
Choose 4-Axis Normal to Part under Tool Axis.
The 4-Axis Normal to Part dialog displays. Key in 15 degrees for the Rotation Angle. Choose 2 Points for the Rotation Axis.
Select line end points 1 and 2 as illustrated below to define the Rotation Axis.
608
The Rotation Axis vector displays. OK to accept the tool axis definition.
4-Axis Normal to Part Tool Axis Generating the Tool Path You will generate the tool path and observe the 4-Axis Normal to Part tool axis. Generate the tool path.
4-Axis Normal to Part Tool Axis Visualizing the Tool Path Reorient to a Front view (MB3
Orient View
Front).
Choose the Shaded icon in the toolbar so you can clearly see the contoured part surfaces. Choose the Verify icon at the bottom of the dialog.
609 The Toolpath Visualization dialog displays with the Replay tab chosen. Choose the Play Forward icon. The tool consistently leans to the right (by 15 degrees) of a tool axis that is otherwise normal to the part surface during both zig and zag moves.
Change to a Right view. Choose the Shaded icon in the toolbar so you can clearly see the contoured part surfaces. Choose the Play Backward icon. The tool moves within parallel planes normal to the rotation axis.
OK to complete the tool path visualization. OK to complete the operation. Close the part file.
610
4-Axis Relative to Part Tool Axis You will define a 4-Axis Relative to Part tool axis by editing a Variable Contour operation containing a 4-Axis Normal to Part tool axis. 4-Axis Relative to Part works in much the same way as 4-Axis Normal to Part. In addition, you may define a lead and a tilt angle allowing the tool axis to lean forward or backward or tilt to the right or left of an otherwise 4-Axis Normal to Part tool axis. 1. 2. 3. 4. 5.
Part Surface Normal Positive Lead Angle Rotation Angle Plane Normal to Rotation Axis Axis Parallel to Plane. Tilt of 0 Degrees
Open part file srf_srf_area_8.prt from the srf subdirectory. Choose Application
Manufacturing.
4-Axis Relative to Part Tool Axis Editing the Operation In the Program Order View of the Operation Navigator, double-click on the VARIABLE_CONTOUR icon to edit the operation.
611
This operation uses 4-Axis Normal to Part as the tool axis. You will change this to a 4-Axis Relative to Part tool axis.
4-Axis Relative to Part Tool Axis Defining the 4-Axis Relative to Part Tool Axis 4-Axis Relative to Part defines a tool axis that uses a lead, tilt, rotation angle, and rotation axis. A positive lead leans the tool forward from the normal tool axis based on the direction of the tool path. The rotation angle leans the tool forward or back in relation to the lead angle. It always leans to the same side of the lead angle and is not dependent on the cut direction. 1. Part Surface Normal 2. Positive Lead Angle 3. Rotation Angle
The rotation axis defines the plane that the tilt is referenced from. A tilt angle defines the angle of the tool axis from side to side and is referenced from the plane normal to the rotation axis. A positive value tilts the tool to the right as you look in the direction of cut. A negative value tilts the tool to the left. 1. Plane Normal to Rotation Axis 2. Rotation Axis 3. Axis Parallel to Plane. Tilt of 0 Degrees
612
Choose 4-Axis Relative to Part under Tool Axis.
The 4-Axis Relative to Part dialog displays. The Rotation Angle and Rotation Axis are retained from the 4-Axis Normal to Part tool axis. Key in 5.0 degrees for the Lead.
Leave the Tilt set to 0.0000. OK to accept the tool axis definition.
4-Axis Relative to Part Tool Axis Generating the Tool Path Generate the tool path.
613
4-Axis Relative to Part Tool Axis Visualizing the Tool Path Reorient to a Front view (MB3
Orient View
Front).
Choose the Verify icon at the bottom of the dialog. Choose the Play Forward icon. The rotation angle consistently remains 15 degrees to the right of the lead. The lead reverses 5 degrees to either side of the normal tool axis depending on the zig or zag cut direction. 1. Lead 2. Rotation Angle
Change to a Right view. Choose the Play Backward icon. The tool moves within parallel planes normal to the rotation axis (zero degree tilt).
614
OK to complete the tool path visualization. OK to complete the operation. Close the part file.
Interpolate Tool Axis You will create a variable axis surface contouring operation that uses the Surface Area drive method and the Interpolate tool axis to finish the contoured surfaces. Interpolate controls the tool axis at specific points by allowing you to add, delete, and edit tool axis vectors.
615 In this operation, you will define only the drive geometry. You will not define part geometry. As a result, the tool path will be created directly on the drive geometry and definition of a projection vector will not be necessary.
Interpolate Tool Axis Opening the Part Open part file srf_srf_area_9.prt from the srf subdirectory.
Choose Application
Manufacturing.
Interpolate Tool Axis Beginning the Operation Choose the Create Operation icon
in the toolbar.
In the Create Operation dialog, choose mill_multi-axis as the Type. Choose VARIABLE_CONTOUR as the subtype. The system automatically names the operation VARIABLE_CONTOUR. Specify the following groups in the Create Operation dialog.
The operation will inherit the parameters defined by these groups.
616 OK to begin creating the operation.
Interpolate Tool Axis Defining the Drive Method The Surface Area drive method allows you to define a variable tool axis and to cut directly on the drive geometry. Choose Surface Area under Drive Method.
OK the warning. The Surface Drive Method dialog displays.
Interpolate Tool Axis Defining the Drive Geometry You will define the drive geometry by selecting an array of faces. Choose Select under Drive Geometry. The Drive Geometry dialog displays. When selecting more than one face, the faces must be arranged in an orderly grid of rows and columns.
617 Faces must be selected in an orderly sequence. They may not be selected randomly. The sequence in which you select the first adjacent faces defines a row. When you finish selecting the first row, you must specify that you wish to begin selecting the second row. Each subsequent row must then contain the same number of adjacent faces.
Interpolate Tool Axis Selecting the First Row Select the first face as illustrated below.
Select the second face. You may need to rotate the model.
618
Select the third and fourth faces.
You must now specify that you wish to begin the next row.
Interpolate Tool Axis Selecting the Second Row Choose Select Next Row.
619 By choosing this option, you have specified that every row will contain four faces. You will no longer need to choose Select Next Row when beginning a new row. Select the fifth through eighth faces.
Interpolate Tool Axis Selecting the Remaining Faces Select the ninth through twelfth faces.
Continue selecting faces in the same orderly sequence until all twenty-eight faces have been selected.
620 OK to complete the drive geometry. The Surface Drive Method dialog displays.
Interpolate Tool Axis Defining the Material Side Two vectors display; one defining the default drive direction and other defining the Material Side of the drive geometry.
The material side vector determines which side the tool contacts when cutting on the drive surfaces. The material side vector should point towards the material to be removed (away from the part) as illustrated above. If it does not, Flip Material can be used to reverse the direction. Choose Display under Drive Geometry to verify that the drive geometry has been correctly defined.
621
Refresh the graphics display.
Interpolate Tool Axis Defining the Cut Direction Cut Direction allows you to specify the direction of the first cut and the quadrant where the first cut will begin. Choose Cut Direction. Choose the vector illustrated below.
622
Interpolate Tool Axis Defining the Stepover Stepover controls the distance between successive Cut Passes. Choose Scallop as the Stepover.
Scallop Height is the maximum allowable height measured normal to the Drive Surface. Key in 0.01 for the Scallop Height.
Choose Display Drive Path to verify that drive points and a zig-zag drive path are defined on the drive geometry.
623
Refresh the graphics display.
Interpolate Tool Axis Defining the Interpolate Tool Axis This part requires a tool axis that follows the general shape of the drive surfaces while avoiding excessive tool axis change. Interpolate controls the tool axis at specific points using vectors. It allows you to control excessive change of the tool axis caused by very complex drive or part geometry without requiring the construction of additional tool axis control geometry (ex: points, lines, vectors, smoother drive surface).
You may define as many vectors extending from specified positions on the drive geometry as needed to create a smooth tool axis movement. The more vectors you specify, the more control you have over the tool axis.
624 Choose Interpolate under Tool Axis.
An array of default tool axis vectors displays. These vectors are normal to the drive surfaces and define the current Interpolate tool axis. Using all of these vectors would cause excessive change in the tool axis.
You may remove, add, and edit vectors to achieve the necessary tool axis control. To edit or remove a vector, you must first highlight the desired vector by using the Previous or Next arrow options or by selecting the desired vector directly from the screen and then choose Edit or Remove. Display refreshes the screen and updates the currently defined vectors for visual reference.
Interpolate Tool Axis Removing Tool Axis Vectors You will remove the vectors that cause unnecessary tool axis change.
625 Choose the Next arrow until the vector illustrated below highlights.
Choose Remove to delete the highlighted vector. The next vector in the sequence highlights.
Choose Remove to delete the highlighted vector.
626 Continue using Next and choosing Remove to delete vectors until only the vectors illustrated below remain. remember, you can choose Display at any time to update the currently defined vectors for visual reference.
OK to complete the Interpolated tool axis. OK to complete the Surface Area drive method.
Interpolate Tool Axis Generating the Tool Path You will generate the tool path and observe how the tool axis follows the vectors. Choose the Edit Display icon under Toolpath and choose 3-D for the Tool Display. Key in 40 for the Frequency. OK to accept the tool display. Generate the tool path.
627
Interpolate Tool Axis Visualizing the Tool Path Reorient to a Front view (MB3
Orient View
Front).
Choose the Verify icon at the bottom of the dialog. The Toolpath Visualization dialog displays with the Replay tab chosen. Choose the Play Forward icon.
The tool axis rotates 180 degrees as the tool zig-zags from one side of the part to the other. You can reduce the change in the tool axis by editing the tool axis vectors. OK to complete the tool path visualization.
628
Interpolate Tool Axis Editing Tool Axis Vectors You will edit the vectors so that there is less change in the tool axis as the tool zig-zags from one side of the part to the other. Change to a TFR-ISO view. To aid you in editing the vectors, you will display two lines that are currently hidden on Layer 3 and use them to edit the vectors. Choose Format
Layer Settings from the menu bar.
The Layer Settings dialog is displayed. Highlight 3 in the Layer/Status list box and choose Selectable. OK to accept the layer settings. Two yellow angled lines display. Choose Interpolate under Tool Axis. Use the Next arrow icon to highlight the vector illustrated below.
Choose Edit under Data Point to modify the highlighted vector. Choose the Inferred Vector icon.
629 Choose the upper end of the angled line as illustrated below.
A temporary vector displays at the end of the line. OK to complete editing the vector. The edited vector is highlighted.
630 Choose Display to refresh the screen. The currently defined tool axis vectors are displayed. Continue using Previous or Next, choosing Edit, choosing the Inferred Vector icon, and selecting the top end of the appropriate angled line to edit the remaining five vectors at the bottom of the part.
Choose Display to refresh the screen.
OK to complete the Interpolated tool axis.
631
Interpolate Tool Axis Generating the Tool Path You will generate the tool path and observe how the tool axis follows the edited vectors Reorient to a Front view (MB3
Orient View
Front).
Reject the previous tool path. Generate the tool path.
Interpolate Tool Axis Visualizing the Tool Path Choose the Verify icon at the bottom of the dialog. The Toolpath Visualization dialog displays with the Replay tab chosen. Choose the Play Forward icon.
632
The tool axis rotates 180 degrees as the tool zig-zags from one side of the part to the other. You can reduce the change in the tool axis by editing the tool axis vectors. OK to complete the tool path visualization. OK to complete the operation. Close the part file.
Toward Point Tool Axis You will create a variable axis surface contouring operation that uses the Surface Area drive method and the Toward Point tool axis to finish the vertical walls of a cavity. Toward Point defines a tool axis that converges toward a focal point, allowing the tool to cut with the tip in a confined space.
633
In this operation, you will define only the drive geometry. You will not define part geometry. As a result, the tool path will be created directly on the drive geometry and definition of a projection vector will not be necessary.
Toward Point Tool Axis Opening the Part Open part file srf_srf_area_10.prt from the srf subdirectory.
Choose Application
Manufacturing.
634
Toward Point Tool Axis Creating the Operation Choose the Create Operation icon in the toolbar. In the Create Operation dialog, choose mill_multi-axis as the Type. Choose VARIABLE_CONTOUR as the subtype. The system automatically names the operation VARIABLE_CONTOUR. Specify the following groups in the Create Operation dialog.
The operation will inherit the parameters defined by these groups. OK to begin creating the operation.
Toward Point Tool Axis Defining the Drive Method The Surface Area drive method allows you to define a variable tool axis and to cut directly on the drive geometry. Choose Surface Area under Drive Method.
OK the warning. The Surface Drive Method dialog displays.
635
Toward Point Tool Axis Defining the Drive Geometry You will define the drive geometry by selecting an array of surfaces as you did when defining the Interpolate tool axis. Choose Select under Drive Geometry. When selecting more than one drive surface, the surfaces must be selected by row in an orderly sequence. Select the first surface as illustrated below.
Select the second and third surfaces.
636
Toward Point Tool Axis Selecting the Second Row
You must now specify that you wish to begin the next row. Choose Select Next Row. By choosing this option, you have specified that you will begin a new row and that every row will contain three surfaces. Select the fourth, fifth, and sixth surfaces.
637
Toward Point Tool Axis Selecting the Third Row Select the seventh through ninth surfaces.
Toward Point Tool Axis Selecting the Remaining Surfaces Continue selecting drive surfaces in the same orderly sequence until all twenty-four
638 surfaces have been selected. You may need to rotate the model.
OK to complete the drive geometry. The Surface Drive Method dialog displays. Choose Display under Drive Geometry to verify that the drive geometry has been correctly defined.
Toward Point Tool Axis Defining the Material Side Two vectors display; one defining the default drive direction and other defining the Material Side of the drive geometry.
639
The material side vector determines which side the tool contacts when cutting on the drive surfaces. The material side vector should point towards the material to be removed (away from the part) as illustrated above. If it does not, Flip Material can be used to reverse the direction. Refresh the graphics display.
Toward Point Tool Axis Defining the Cut Direction Cut Direction allows you to specify the direction of the first cut and the quadrant where the first cut will begin. Choose Cut Direction. Choose the vector illustrated below.
640
Toward Point Tool Axis Defining the Cut Type A Zig cut type will allow the tool to cut the cavity in one direction. Choose Zig for the Cut Type.
Toward Point Tool Axis Defining the Stepover Stepover controls the distance between successive Cut Passes. Choose Scallop as the Stepover.
Scallop Height is the maximum allowable height measured normal to the Drive Surface. Key in 0.10 for the Scallop Height. Choose Display Drive Path to verify that drive points and zig drive path are defined on the drive geometry.
641
Refresh the graphics display.
Toward Point Tool Axis Defining the Toward Point Tool Axis This part requires a tool axis that can reach into the cavity and cut along the vertical walls with the tip of the tool. Toward Point defines a tool axis that converges at a focal point.
Choose Toward Point under Tool Axis.
Select the point above the part.
642
The Surface Drive Method dialog displays.
Toward Point Tool Axis When Gouging Drive Surfaces The When Gouging option allows you to specify how the system will respond when the tool gouges drive surfaces during cutting moves. These options apply only when you are cutting directly on drive surfaces and not when you are cutting on part surfaces. When Gouging also appears in the Cutting Parameters dialog. In that dialog, the options determine how the system responds when the tool gouges check geometry. Skip causes the system to alter the tool path by removing only the drive points that cause the gouging to occur. Choose Skip for When Gouging.
OK to complete the Surface Area drive method. More About When Gouging Driving Surfaces
The When Gouging option allows you to specify how the system will respond when the tool gouges the Drive Surface during cutting moves. These options only apply when you are cutting to Drive Surfaces and not when you are cutting to Part Surfaces.
643 None causes the system to ignore Drive Surface gouging. It will generate the same unaltered tool path as the Warning option, but will not issue a warning message to the tool path or CLSF.
Skip causes the system to alter the tool path by removing only the Drive Points that cause gouging to occur. The result is a straight tool movement from the last position before gouging to the first position which is no longer gouging. When generating tool paths directly from Drive Surface, the tool does not violate the Drive Surface at convex corners, and does not gouge concave regions when using Skip as illustrated below.
In some cases where the drive surface is smoothly concave, the Skip option may not clean up the tool path as well as illustrated in the concave corner case above. Retract causes the tool to avoid gouging the Drive Surface by using the parameters defined in Non-Cutting Moves.
Toward Point Tool Axis Generating the Tool Path You will generate the tool path and observe how the tool finishes the sides of the cavity. Generate the tool path.
644
Choose the Shaded icon in the toolbar so you can clearly see the contoured part surfaces. Choose the Verify icon at the bottom of the dialog. The Toolpath Visualization dialog displays with the Replay tab chosen. Choose the Play Forward icon.
OK to complete the tool path visualization. OK to complete the operation. Close the part file.
645
Away From Point Tool Axis You will create a variable axis surface contouring operation that uses the Surface Area drive method and the Away From Point tool axis to finish the sides of a core. Away From Point defines a tool axis that diverges away from a focal point, allowing the tool to cut the vertical walls with the tip.
In this operation, you will define only the drive geometry. You will not define part geometry. As a result, the tool path will be created directly on the drive geometry and definition of a projection vector will not be necessary.
Away From Point Tool Axis Opening the Part Open part file srf_srf_area_11.prt from the srf subdirectory.
646 Choose Application
Manufacturing.
Away From Point Tool Axis Creating the Operation Choose the Create Operation icon in the toolbar. In the Create Operation dialog, choose mill_multi-axis as the Type. Choose VARIABLE_CONTOUR as the subtype. The system automatically names the operation VARIABLE_CONTOUR. Specify the following groups in the Create Operation dialog.
The operation will inherit the parameters defined by these groups. OK to begin creating the operation.
Away From Point Tool Axis Defining the Drive Method The Surface Area drive method allows you to define a variable tool axis and to cut directly on the drive geometry. Choose Surface Area under Drive Method.
OK the warning.
647 The Surface Drive Method dialog displays.
Away From Point Tool Axis Defining the Drive Geometry You will define the drive geometry by selecting a single drive surface. Choose Select under Drive Geometry. The Drive Geometry dialog displays. Select the surface as illustrated below.
OK to complete the drive geometry. The Surface Drive Method dialog displays. Two vectors display; one defining the default drive direction and other defining the Material Side of the drive geometry. The material side vector determines which side the tool contacts when cutting on the drive surfaces. The material side vector should point towards the material to be removed (away from the part) as illustrated below. If it does not, Flip Material can be used to reverse the direction.
648
Away From Point Tool Axis Defining the Cut Direction Cut Direction allows you to specify the direction of the first cut and the quadrant where the first cut will begin. Choose Cut Direction. Choose the vector illustrated below.
Away From Point Tool Axis Defining the Cut Type A Zig cut type will allow the tool to continually cut around the core in one direction. Choose Zig for the Cut Type.
649
Away From Point Tool Axis Defining the Stepover Stepover controls the distance between successive Cut Passes. Choose Scallop as the Stepover. Scallop Heights the maximum allowable height measured normal to the Drive Surface. Be sure the Scallop Height is 0.0050. Choose Display Drive Path to verify that drive points and a zig-zag drive path are defined on the drive geometry.
Refresh the graphics display.
Away From Point Tool Axis Defining the Away From Point Tool Axis This part requires a tool axis that can finish the vertical sides of a core with the tip of the tool. Away From Point defines a tool axis that diverges away from a focal point.
650
Choose Away from Point under Tool Axis.
Select the point below the part.
The Surface Drive Method dialog displays. OK to complete the Surface Area drive method.
Away From Point Tool Axis Defining the Check Geometry Check geometry will prevent the tool from gouging the planar face. Choose the Check icon
and Select.
Choose Faces as the Filter Method.
651
Select the planar face as illustrated below.
OK to accept the face as the check geometry. The VARIABLE_CONTOUR dialog displays.
Away From Point Tool Axis When Gouging Check Geometry The When Gouging option allows you to specify how the system will respond when the tool gouges check geometry during cutting moves. Choose Cutting. Choose Skip for When Gouging. Skip causes the tool to omit the tool positions which gouge the check geometry. Check Safe Clearance defines an extended safety zone for check geometry which cannot be violated by the tool or the tool holder.
652
Key in 0.05 for the Check Safe Clearance. OK to accept the Cutting Parameters.
Away From Point Tool Axis Generating the Tool Path You will generate the tool path and observe how the tool finishes the sides of the core. Generate the tool path.
Choose the Shaded icon in the toolbar so you can clearly see the contoured part surfaces. Choose the Verify icon at the bottom of the dialog. The Toolpath Visualization dialog displays with the Replay tab chosen. Choose the Play Forward icon.
653
OK to complete the tool path visualization. OK to complete the operation. Close the part file.
Surface Contouring Projects These two projects require you to finish a core and a cavity. You will create programs consisting of Surface Contouring operations that machine the parts using standard machining techniques. You will then check each program by dynamically displaying material removal and comparing the finished machined part to the original model.
654
Using Area Mill to Machine a Core This metric part is a core machined from a solid block of material. The completed machining program consists of six operations that rough, semi-finish, and finish the part. You will create the last four operations using the Area Mill drive method to semi-finish and finish the part.
To complete this project, you should be familiar with the following types of operations. CONTOUR_AREA_NON-STEEP CONTOUR_ZIGZAG CONTOUR_AREA_DIR_STEEP In addition, you should know how to create a Mill Area parent group and how to define a Trim Boundary and a Cut Area. You will also Animate the tool path and use Show Excess to graphically display the excess material left by the roughing operations.
655
Using Area Mill to Machine a Core Functions Used to Machine the Part In this project you will: Create a CONTOUR_AREA_NON_STEEP operation to semi-finish the part.
Create a MILL_AREA parent group containing a Trim Boundary.
Apply the MILL_AREA geometry group as a parent to the CONTOUR_AREA_NON_STEEP operation to eliminate edge tracing.
656 Create a CONTOUR_ZIGZAG operation using the MILL_AREA geometry group to finish the part.
Create a CONTOUR_AREA_DIR_STEEP operation that finishes only the steep areas.
Create a CONTOUR_ZIGZAG operation using a Cut Area to finish the core with a very small stepover.
Use Verify Toolpath to graphically simulate material removal for the entire program.
657
Compare the finished machined part to the original model.
Using Area Mill to Machine a Core Design Intent The completed program must cut the finished part from a solid block of material using a sequence of roughing, semi-finishing, and finishing operations while applying acceptable standard machining techniques.
Using Area Mill to Machine a Core Open the Part File
658 Open part file srf_proj_1.prt from the srf subdirectory. Enter the Manufacturing Application.
Fully expand the objects in the Geometry View of the Operation Navigator. Choose the Geometry View icon in the Toolbar. In the Operation Navigator, select the plus (+) signs next to the MCS_MILL and WORKPIECE groups. Replay the two operations. In the Operation Navigator, highlight the WORKPIECE icon and MB3
Replay.
These two Z-Level Milling operations perform the initial rough cuts. You will create four Fixed Axis Surface Contouring operations that use the Area Mill drive method to semi-finish and finish the part.
Using Area Mill to Machine a Core Creating a Contour Area Non-Steep Semi-Finish Operation You need to create an operation that semi-finishes only the non-steep areas.
659
Create a CONTOUR_AREA_NON_STEEP operation using the following parent groups: Choose the Create Operation icon. Choose mill_contour as the Type Choose the CONTOUR_AREA_NON_STEEP icon as the subtype. Specify the parent groups as indicated below.
OK to begin creating the operation. Specify a Steep Angle of 35 degrees and a Stepover of 25 percent of the tool diameter. Under Drive Method, choose Area Milling. Key in 35.0000 for the Steep Angle and 25.0000 for the Stepover Percent. OK to accept the parameters. Generate the tool path. Notice the edge tracing.
660 OK to complete the operation.
Using Area Mill to Machine a Core Defining a Trim Boundary You need to remove the edge tracing. In this case, you will define a Trim boundary in a geometry group.
Create a MILL_AREA geometry group using WORKPIECE as the parent. Choose the Create Geometry icon. Choose the MILL_AREA icon. Choose WORKPIECE as the Parent group. OK to begin creating the Group. Define a trim boundary on the bottom face of the part. Choose the Trim icon and Select. Turn on the Outside option. Select the bottom face of the part. OK to complete the trim boundary. OK to complete the MILL_AREA geometry group. The MILL_AREA geometry group should now appear in the Geometry View of the Operation Navigator.
661
Using Area Mill to Machine a Core Applying the Trim Boundary You need to apply the geometry group to the operation so that the edge tracing is removed. Edit the CONTOUR_AREA_NON_STEEP operation so that MILL_AREA is specified as the parent geometry group. In the Operation Navigator, double-click on the CONTOUR_AREA_NON_STEEP icon to display the operation parameters dialog. Choose the Groups tab. Turn on the Geometry:WORKPIECE option. Choose Reselect. Choose MILL_AREA in the Reselect Geometry dialog. OK to accept the change. OK to complete editing the operation.
The MILL_AREA geometry group should appear as a parent of the CONTOUR_AREA_NON_STEEP operation.
Generate the tool path. In the Operation Navigator, highlight the CONTOUR_AREA_NON_STEEP operation and MB3 Generate. OK the Tool Path Generation dialog.
Notice the edge tracing has been removed.
662
Using Area Mill to Machine a Core Creating a Contour Zig Zag Finish Operation You need to create an operation that finishes the entire part.
Create a CONTOUR_ZIGZAG operation using the following parent groups: Choose the Create Operation icon. Choose mill_contour as the Type. Choose the CONTOUR_ZIGZAG icon as the subtype. Specify the parent groups as indicated below.
OK to begin creating the operation. Specify a Cut angle of 0.0000 degrees and a Stepover of 25 percent of the tool diameter.
663 Under Drive Method, choose Area Milling. Choose User Defined as the Cut Angle and OK to accept 0.0000 degrees. Key 25.0000 for the Stepover Percent. OK to accept the parameters. Generate the tool path.
OK to complete the operation.
Using Area Mill to Machine a Core Creating a Contour Area Directional Steep Finish Operation You need to create an operation that finishes only the steep areas.
Create a CONTOUR_AREA_DIR_STEEP operation using the following parent groups: Choose the Create Operation icon. Choose mill_contour as the Type. Choose the CONTOUR_AREA_DIR_STEEP icon as the subtype. Specify the parent groups as indicated below.
664
OK to begin creating the operation. Verify that the Steep Containment is defined as Directional Steep and that Steep Angle is 35 degrees. Under Drive Method, choose Area Milling. Specify a Cut angle of 90 degrees and a Stepover of 25 percent of the tool diameter. Choose User Defined as the Cut Angle and OK to accept 90.0000 degrees. Key 25.0 for the Stepover Percent. OK to accept the parameters. Generate the tool path.
OK to complete the operation.
Using Area Mill to Machine a Core Creating a Contour Zig Zag Finish Operation You need to create an operation that finishes the core with a very small stepover.
665
Create a CONTOUR_ZIGZAG operation using the following parent groups: Choose the Create Operation icon. Choose mill_contour as the Type. Choose the CONTOUR_ZIGZAG icon as the subtype. Specify the parent groups as indicated below.
OK to begin creating the operation. Specify a Cut angle of 0.0000 degrees and a Stepover of 10 percent of the tool diameter. Under Drive Method, choose Area Milling. Choose User Defined as the Cut Angle and OK to accept 0.0000 degrees. Key 10.0 for the Stepover Percent. OK to accept the parameters. Define the core as the cut area. Under Geometry, choose the Cut Area icon and Select. Turn on the Features selection option and choose the surface region illustrated below.
666
OK to accept the Cut Area. Generate the tool path.
OK to complete the operation. The operations and groups should now appear in the Geometry View of the Operation Navigator.
667
Using Area Mill to Machine a Core Displaying Material Removal You need to visualize the tool path for the entire program and compare the finished machined part to the original solid model. Use dynamic material removal to visualize the tool path for the entire program. In the Program Order View of the Operation Navigator, highlight the PROGRAM icon. Choose the Verify Toolpath icon in the Toolbar. Choose the Dynamic Tab. Choose the Play Forward icon.
Compare the machined part to the original model. Choose Compare in the Toolpath Visualization dialog.
Cancel to dismiss the Toolpath Visualization dialog. Close the part.
668
Using Flow Cut to Finish a Cavity This part contains a cavity machined from a solid block of material. The completed machining program consists of six operations that rough, semi-finish, and finish the part. You will create the last two operations of the program using Flow Cut to finish the corners and fillets.
To complete this project, you should be familiar with the following types of operations. FLOWCUT_SINGLE FLOWCUT_REF_TOOL You will also Animate the tool paths to graphically simulate material removal.
Using Flow Cut to Finish a Cavity Functions Used to Machine the Part In this project you will: Create a FLOWCUT_REF_TOOL operation to finish the corners and fillets using multiple passes.
669 Create a FLOWCUT_SINGLE operation to finish the corners using a single pass and a small tool.
Use Verify Toolpath to graphically simulate material removal for the entire program.
Compare the finished machined part to the original model.
Using Flow Cut to Finish a Cavity Design Intent The completed program must be able to cut the part from a solid block of material, using flow cuts to finish the corners and fillets.
670
Using Flow Cut to Finish a Cavity Open the Part File Open part file srf_proj_2.prt from the srf subdirectory. Enter the Manufacturing Application. Fully expand the objects in the Program Order View of the Operation Navigator. Choose the Program Order View icon in the Toolbar. In the Operation Navigator, select the plus (+) signs next to the PROGRAM group.
Using Flow Cut to Finish a Cavity Displaying Material Removal You need to visualize the tool path for the entire program and compare the finished machined part to the original solid model. Use dynamic material removal to visualize the tool path for the entire program. In the Program Order View of the Operation Navigator, highlight the PROGRAM icon. Choose the Verify Toolpath icon in the Toolbar. Choose the Dynamic Tab. Choose the Play Forward icon.
671
Compare the machined part to the original model. Choose Compare in the Toolpath Visualization dialog.
The white areas indicate that further finishing is required to machine to the specified Outtol. Cancel to dismiss the Toolpath Visualization dialog. You will create two Flow Cut operations to finish the corners and fillets.
Using Flow Cut to Finish a Cavity Creating a Reference Tool Flow Cut You need to create an operation that finishes the corners and fillets with multiple passes.
672 Create a FLOWCUT_REF_TOOL operation using the following parent groups: Choose the Create Operation icon. Choose mill_contour as the Type Choose the FLOWCUT_REF_TOOL icon as the subtype. Specify the parent groups as indicated below.
OK to begin creating the operation. Key in a Stepover Distance of 0.05. Specify the sequence of cuts to start at the center flow cut and move toward the outside passes. Choose Inside-Out for Sequencing. Define the cut region so that it covers at least the width of the 0.1500 radius fillets. Key in 0.375 for the Reference Tool Diameter to establish a cut region that is a little wider than the fillets. Generate the tool path.
OK to complete the operation.
Using Flow Cut to Finish a Cavity Creating a Single Pass Flow Cut You need to create an operation that finishes just the corners with a single pass.
673
Create a FLOWCUT_SINGLE operation using the following parent groups: Choose the Create Operation icon. Choose mill_contour as the Type Choose the FLOWCUT_SINGLE icon as the subtype. Specify the parent groups as indicated below.
OK to begin creating the operation. Specify that the tool should cut along as flat an angle as possible. Choose the More tab. Key in a Maximum Concavity of 179.0. Be sure the tool cuts all the way across the top of the part in a continuous motion and does not retract. Key in 0.25 for the Hookup Distance. Generate the tool path.
674
OK to complete the operation.
Using Flow Cut to Finish a Cavity Displaying Material Removal You need to visualize the tool path for the entire program and compare the finished machined part to the original solid model. Use dynamic material removal to visualize the tool path for the entire program. In the Program Order View of the Operation Navigator, highlight the PROGRAM icon. Choose the Verify Toolpath icon in the Toolbar. Choose the Dynamic Tab. Choose the Play Forward icon.
Compare the machined part to the original model. Choose Compare in the Toolpath Visualization dialog.
675
Cancel to dismiss the Toolpath Visualization dialog. Close the part.