TRN-4501-400-01_SG-Ins_Exc_EN.pdf

Introduction to Creo Parametric 3.0

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Date 03/28/2014

Description Initial Printing of: Introduction to Creo Parametric 3.0

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Training Agenda Day 1 Module 01 Module 02 Module 03 Module 04 Module 05 Module 06

― Introduction to the Creo Parametric Basic Modeling Process ― Understanding Creo Parametric Concepts ― Using the Creo Parametric Interface ― Selecting Geometry, Features, and Models ― Editing Geometry, Features, and Models ― Creating Sketcher Geometry

Day 2 Module Module Module Module Module Module

07 08 09 10 11 12

― Using Sketcher Tools ― Creating Sketches for Features ― Creating Datum Features: Planes and Axes ― Creating Extrudes, Revolves, and Ribs ― Sketcher Workflow ― Creating Sweeps and Blends

13 14 15 16 17 18

― Creating Holes, Shells, and Draft ― Creating Rounds and Chamfers ― Project I ― Group, Copy, and Mirror Tools ― Creating Patterns ― Measuring and Inspecting Models

19 20 21 22 23 24

― Assembling with Constraints ― Assembling with Connections ― Exploding Assemblies ― Drawing Layout and Views ― Creating Drawing Annotations ― Using Layers

25 26 27 28

― Investigating Parent/Child Relationships ― Capturing and Managing Design Intent ― Resolving Failures and Seeking Help ― Project II



Day 5 Module Module Module Module

Table of Contents Introduction to Creo Parametric 3.0 Creating Extrudes, Revolves, and Ribs ..................................................................................... 10-1 Creating the Crankshaft ..................................................................................................... 10-2 Thickening the Piston Wrist Pin Hole................................................................................... 10-5 Completing the Crankshaft ................................................................................................. 10-7 Creating Profile Rib Features............................................................................................ 10-10 Creating Sweeps and Blends..................................................................................................... 12-1 Creating a Sweep Through a 3-D Curve.............................................................................. 12-2 Creating a Blend Feature on FLYWHEEL.PRT and Embedding the Orientation Datum ........... 12-4 Creating Holes, Shells, and Draft............................................................................................... 13-1 Common Dashboard Options: Hole Depth........................................................................... 13-2 Creating Coaxial Holes ...................................................................................................... 13-3 Creating Linear Holes ........................................................................................................ 13-7 Creating Radial and Diameter Holes ................................................................................... 13-8 Shelling the Fuel Tank...................................................................................................... 13-10 Creating Rounds and Chamfers ................................................................................................ 14-1 Creating Rounds on the Rear Engine Block 1 ...................................................................... 14-2 Creating Rounds on the Gearbox Front ............................................................................... 14-4 Creating Rounds on the Rear Engine Block 2 ...................................................................... 14-7 Creating Full Rounds on the Connecting Rod ...................................................................... 14-8 Creating Chamfers on the Crankshaft ................................................................................. 14-9 Project I ..................................................................................................................................... 15-1 Group, Copy, and Mirror Tools................................................................................................... 16-1 Rotating a Copy of a Boss on the Engine Block ................................................................... 16-2 Copying and Translating Carburetor Features...................................................................... 16-4 Mirroring Selected Carburetor Features............................................................................... 16-6 Creating Patterns....................................................................................................................... 17-1 Patterning Vents Using a Two Directional Pattern ................................................................ 17-2 Creating Flywheel Blades Using an Axis Pattern.................................................................. 17-3 Creating Exhaust Cuts in the Muffler Using a Two Directional Axis Pattern ............................ 17-4 Patterning Rounds on the Cylinder Fins Using Reference Patterns ....................................... 17-6 Measuring and Inspecting Models ............................................................................................. 18-1 Analyzing Design Models ................................................................................................... 18-2 Assembling with Constraints..................................................................................................... 19-1 Creating the Engine Assembly using Automatic Constraints ................................................. 19-2 Creating the Drill Chuck Assembly using Automatic Constraints............................................ 19-6 Creating the Crank Assembly using Automatic Constraints................................................... 19-9 Creating the Piston Assembly using Automatic Constraints ................................................ 19-11

Drawing Layout and Views ........................................................................................................ 22-1 Creating Drawing Views ..................................................................................................... 22-2 Creating Drawing Annotations................................................................................................... 23-1 Annotating Drawings.......................................................................................................... 23-2 Using Layers.............................................................................................................................. 24-1 Creating and Managing Layers ........................................................................................... 24-2 Project II .................................................................................................................................... 28-1

Module 10 Creating Extrudes, Revolves, and Ribs

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Module 10 | Page 1

Exercise 1: Creating the Crankshaft Objectives After successfully completing this exercise, you will be able to: • Create multiple extrude features to create the CRANKSHAFT.PRT.

Scenario As part of the new design for the gas powered drill, you have been assigned to the crankshaft. Create the crankshaft main journal and connecting rod journal, adhering to the existing sketch. Close Window Extrude\Crankshaft Task 1:

Erase Not Displayed CRANKSHAFT.PRT

Create reference geometry and a sketch feature on CRANKSHAFT.PRT.

1. Enable only the following Datum Display types: . 2. Select datum plane TOP from the model tree. from the Datum group. 3. Click Plane 4. Drag the drag handle up to an offset value of 14, editing it if necessary. 5. In the Datum Plane dialog box, select the Properties tab. • Edit the Name to OFFSET. • Click OK. 6. With datum plane OFFSET still selected, press CTRL and select datum plane RIGHT. from the Datum group. 7. Click Axis 8. In the model tree, right-click the newly created axis and select Rename. Type CRANK_PIN and press ENTER.

Module 10 | Page 2

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9. Click Sketch . 10. Select datum plane FRONT, and click Sketch in the Sketch dialog box. 11. Enable only the following Sketcher Display types: . 12. Click References and select datum axis CRANK_PIN as a new reference. 13. Click Close in the References dialog box. 14. Select Center and Point from the Circle types drop-down menu and sketch the circle with the center snapping to the CRANK_PIN reference. Middle-click to stop circle creation and edit the diameter to 10. . 15. Click OK 16. Click in the background to de-select the sketch. Task 2:

Create the main crankshaft journal.

1. Disable Plane Display

and Axis Display

.

2. Click Extrude . 3. Select the SKETCH_CRANK sketch from the model tree. 4. Select the Options tab in the dashboard and for SIDE 2. select Blind 5. Edit the depth for SIDE 1 to 46.5 and the depth for SIDE 2 to 73.5. 6. Click Complete Feature

.

7. Click Extrude . 8. Select the SKETCH_LOBE sketch from the model tree. 9. Select the Options tab in the dashboard and for SIDE 1. select To Selected • Select datum plane LOBE_FRONT from the model tree as the reference. 10. In the Options tab of the dashboard, select To for SIDE 2. Selected • Select datum plane LOBE_REAR from the model tree as the reference. 11. Click Complete Feature

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.

Module 10 | Page 3

Task 3:

Create the cut for the connecting rod journal.

1. Click Extrude . 2. Select the Sketch 1 sketch from the model tree. 3. In the dashboard, click Remove Material necessary. • Click Change Material Direction • Edit the depth to Symmetric depth value to 10.

4. Click Complete Feature

if

.

, and edit the

.

from the Quick Access toolbar. 5. Click Save 6. Click File > Manage Session > Erase Current > Yes to erase the model from memory.

This completes the exercise.

Module 10 | Page 4

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Exercise 2: Thickening the Piston Wrist Pin Hole Objectives After successfully completing this exercise, you will be able to: • Create a thicken feature to strengthen the PISTON.PRT.

Scenario You have determined that the piston model and the stress that will be generated by the wrist pin are too high for the current amount of material around the wrist pin hole. Add additional material around the wrist pin hole so it meets design criteria. Close Window Extrude\Thicken Task 1:

Erase Not Displayed PISTON.PRT

Thicken the piston's wrist pin hole area.

1. Disable all Datum Display types. 2. Middle-click and drag to orient the model.

3. Click Extrude from the Shapes group. 4. Select Sketch 5 from the model tree. 5. Select the Options tab in the dashboard and for Side 1. select To Next • Select To Next

for Side 2.

. • Click Thicken Sketch • Edit the material thickness to 2. as • Click Change Thickness Side necessary to toggle the thickness to the outside of the sketch. 6. Click Complete Feature

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.

Module 10 | Page 5

Task 2:

Cut out the center of the thickened extrude feature.

1. Click Extrude . 2. Select Sketch 5 from the model tree. 3. In the dashboard, click Remove Material

.

. • Click Symmetric • Edit the depth to 14. • Click Thicken Sketch . • Edit the material thickness to 2. as • Click Change Thickness Side necessary to toggle the thickness to the outside of the sketch. 4. Click Complete Feature

.



Module 10 | Page 6

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Exercise 3: Completing the Crankshaft Objectives After successfully completing this exercise, you will be able to: • Create multiple revolve features to complete the CRANKSHAFT.PRT.

Scenario You have been assigned to complete the crankshaft. Create the tapers on either end of the crankshaft. Close Window

Erase Not Displayed

Revolve\Solid Task 1:

CRANKSHAFT.PRT

Create the sketch for the taper on one side of the CRANKSHAFT.PRT.

1. Disable all Datum Display types. 2. Click Sketch from the Datum group. 3. Select datum plane RIGHT, orient datum plane TOP to face Top, and click Sketch in the Sketch dialog box. 4. Click Sketch View from the In Graphics toolbar. 5. Enable only the following Sketcher Display types: . 6. Select No Hidden from the Display Style types drop-down menu in the In Graphics toolbar. and select the top and right 7. Click References surfaces of the main shaft as new references. 8. Click Close in the References dialog box. 9. Create the sketch: from the Datum group • Click Centerline and sketch a horizontal geometry centerline down the center of the shaft. • Zoom in on the right side of the sketch. from the Line types • Select Line Chain drop-down menu and sketch two lines, snapping the endpoints to the references. • Click Normal . Dimension and edit the sketch as shown. . 10. Click OK 11. Orient to the Standard Orientation. from the Display Style types 12. Select Shading drop-down menu in the In Graphics toolbar.

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Module 10 | Page 7

Task 2:

Cut the taper on the crankshaft using the sketch.

1. Click Revolve 2. Click Solid

from the Shapes group. from the dashboard.

3. Click Remove Material

from the dashboard.


.

Task 3:

Create the sketch for the step on the other side of the CRANKSHAFT.PRT.

1. Click Sketch . 2. Click Use Previous in the Sketch dialog box. 3. Click No Hidden

.

4. Click Sketch View

.

and select the top and left 5. Click References surfaces of the main shaft as new references. 6. Click Close in the References dialog box. 7. Create the sketch: and sketch a horizontal • Click Centerline geometry centerline down the center of the shaft. from the • Select Corner Rectangle Rectangle types drop-down menu and sketch the rectangle, snapping to the references. • Edit the dimensions as shown. . 8. Click OK 9. Orient to the Standard Orientation. 10. Click Shading

Module 10 | Page 8

.

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Task 4:

Cut the step on the crankshaft using the sketch.

1. Click Revolve

.

2. Click Remove Material


.

.



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Module 10 | Page 9

Exercise 4: Creating Profile Rib Features Objectives After successfully completing this exercise, you will be able to: • Create profile rib features.

Scenario Rib features are used to add structural strength to parts. Product testing has indicated that the engine block part needs an additional rib to strengthen it against premature failure. Your assignment is to add the additional profile rib feature. Close Window Rib\Profile Task 1:

Erase Not Displayed ENG_BLOCK.PRT

Create a profile rib on ENG_BLOCK.PRT .

1. Enable only the following Datum Display types: . 2. Select datum plane RIB and click Sketch from the Datum group. 3. Enable only the following Sketcher Display types: . 4. Click Sketch View toolbar. 5. Disable Plane Display

from the In Graphics .

6. Click References from the Setup group. • Select the three silhouette edges shown (highlighted in green in the following figure) as references, resulting in a total of five specified references. • Click Close in the References dialog box.

Module 10 | Page 10

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7. Zoom in and sketch, as shown in the following figure: • Right-click and select Line Chain . Sketch a horizontal line starting from the diagonal reference, stopping short of the vertical reference. • Right-click and select 3-Point / Tangent End . Start the arc on the unfinished end of the sketched line, and finish on the vertical reference. Middle-click to stop sketching arcs. • Right-click and select Dimension . Select the left end of the arc and the horizontal reference, and place the first dimension. • Type 2 and press ENTER. • Select the horizontal line you sketched and the horizontal reference, and place the second dimension. • Type 5 and press ENTER. from the Operations • Click One-by-One group and edit the arc radius to 6. 8. Click OK from the ribbon. 9. Middle-click and drag to orient the model.

10. With the sketch still selected, select Profile Rib from the Rib types drop-down menu. Select the References tab. Click Flip and then edit the thickness to 2. Click Change Thickness Option as necessary to set the rib feature symmetric about the sketch.

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Module 10 | Page 11


.



Module 10 | Page 12

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Module 12 Creating Sweeps and Blends

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Module 12 | Page 1

Exercise 1: Creating a Sweep Through a 3-D Curve Objectives After successfully completing this exercise, you will be able to: • Create a sweep through a 3-D curve.

Scenario You are assigned to create the cord of the coil part that connects the main body of the coil to the spark plug adapter. Sweep a solid along the existing 3-D curve. Close Window

Erase Not Displayed

Sweep\Open-Trajectory_Solid Task 1:

COIL.PRT

Create a sweep using the curve as a trajectory.

1. Disable all Datum Display types. 2. Select Sweep from the Sweep types drop-down menu in the Shapes group. 3. Select the 3-D curve as the trajectory in the graphics window. 4. Click Create Section from the dashboard. 5. Enable only the following Sketcher Display types: .

6. Sketch as shown: • Right-click and select Circle . • Sketch a circle at the intersection of the centerlines. • Double-click the dimension and edit the diameter to 5.5. • Click OK

Module 12 | Page 2

.

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7. Click Complete Feature and click in the background to de-select all geometry. 8. In the ribbon, select the View tab. from the 9. Select Appearances Manager Appearance Gallery types drop-down menu. 10. Load the appearance.dmt if necessary, and click Close. 11. Select the solid_black appearance sphere from the Appearance Gallery types drop-down menu. 12. Complete the following: • Press CTRL and select the front and back sweep surfaces. • Click OK in the Select dialog box. from the Quick Access toolbar. 13. Click Save 14. Click File > Manage Session > Erase Current > Yes to erase the model from memory. This completes the exercise.

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Module 12 | Page 3

Exercise 2: Creating a Blend Feature on FLYWHEEL.PRT and Embedding the Orientation Datum Objectives After successfully completing this exercise, you will be able to: • Create blend features. • Embed the orientation datum plane.

Scenario You are assigned to create the initial blade of the flywheel. The design specification document recommends using a thin protrusion to create this feature. Close Window

Erase Not Displayed

Blend\Sketch-Sections_Solid Task 1:

FLYWHEEL.PRT

Insert a thin blend on the FLYWHEEL.PRT.

1. Enable only the following Datum Display types: . 2. Create a datum plane as shown: • Click Plane . • Select datum plane FRONT. Press CTRL and select axis CRANK. • Double-click the angle and edit it to 11.25 or -11.25 to obtain the direction shown. • Select the Properties tab in the Datum Plane dialog box. Type ANGLE as the Name, and click OK. 3. Click in the background to de-select the datum plane. 4. In the ribbon, click the Shapes group drop-down menu and select Blend

.

5. In the dashboard, click Thicken Sketch . • Select the Sections tab and verify that Sketched sections is selected. 6. Right-click in the graphics window and select Define Internal Sketch. 7. Select datum plane TOP as the sketching plane. 8. In the Sketch dialog box, select Bottom as the Orientation and select datum plane ANGLE to face the bottom of the window. • Click Sketch.

Module 12 | Page 4

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9. Enable only the following Sketcher Display types: . 10. Begin the sketch as shown: • Select the CRANK axis as a reference. • Click Close in the References dialog box. and Plane Display • Disable Axis Display . • Click Shading With Edges . • Click Sketch View

.

from the • Click Construction Mode Sketching group to enable it. • Right-click in the graphics window and select . Circle • Sketch two construction circles. and dimension the diameters, • Click Normal editing the values as shown. 11. Click Construction Mode

to disable it.

12. Sketch the first blend section as shown: • Right-click and select 3-Point / Tangent End . Sketch an arc as shown. . • Right-click and select Dimension Dimension the sketch and edit the values as shown. 13. Click OK

.

14. Sketch and constrain the second blend section as shown: • Right-click in the graphics window and select Insert. • Right-click and select Sketch to begin sketching Section 2. • Right-click and select 3-Point / Tangent End . Sketch the smaller arc as shown. from the Constrain group • Click Coincident and constrain the right arc endpoint coincident to the right arc endpoint from the first sketched section. • In the Resolve Sketch dialog box, select the Point On Entity constraint and click Delete. from the Constrain group • Click Tangent and constrain the arc tangent to the first sketched section. • Click One-by-One dimension to 11. • Click OK

© 2014 PTC

and edit the radius

from the ribbon.

Module 12 | Page 5

15. Press CTRL+D to orient to the Standard Orientation. 16. in the dashboard, type 2.1 as the thickness.

17. Enable Plane Display and select Shading from the Display Types drop-down menu in the In Graphics toolbar. 18. In the dashboard, select the Sections tab. • Select Section 2. • Select Reference and select datum plane FIN_HEIGHT. 19. Click Complete Feature

Task 2:

.

Embed the datum plane ANGLE into the blend feature.

1. Click and hold the datum plane ANGLE in the model tree. Drag the feature and drop it on the Blend feature. 2. Expand the Blend feature. 3. Notice that the datum plane ANGLE is now embedded in the blended protrusion feature and hidden.

Creating the blend on an angular datum and then embedding the datum enables the features to be easily patterned with the Dimension option. The angular datum plane is not necessary when patterning with the Axis option.

Module 12 | Page 6

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4. Click Save from the Quick Access toolbar. 5. Click File > Manage Session > Erase Current > Yes to erase the model from memory. This completes the exercise.

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Module 12 | Page 7

Module 12 | Page 8

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Module 13 Creating Holes, Shells, and Draft

© 2014 PTC

Module 13 | Page 1

Exercise 1: Common Dashboard Options: Hole Depth Objectives After successfully completing this exercise, you will be able to: • Specify hole cut depths.

Scenario Edit the definition of a hole feature and test the available depth options. Get an good understanding of each depth option by observing the results each option produces. Close Window Hole\Depth Task 1:

Erase Not Displayed CYLINDER.PRT

Edit the depth of a hole feature.

1. Enable only the following Datum Display types: . 2. Select HOLE_2 in the model tree. Right-click and select Edit Definition . Notice that the current depth option is Blind. 3. Drag the depth handle to 20, editing the value if necessary, and click Preview Feature from the Hole dashboard. Then click Resume from the dashboard. Feature 4. Cursor over the depth handle. Right-click and select To Next. Click Preview Feature from the dashboard. Then click Resume Feature from the dashboard. 5. Cursor over the depth handle. Right-click and select Through All. Click Preview Feature from the dashboard. Then click Resume from the dashboard. Feature 6. Cursor over the depth handle. Right-click and select To Selected. Middle-click to spin the model and select the bottom surface of the fin, as shown. Click Complete Feature . Depth options can also be specified by selecting the flyout depth options from the dashboard. 7. Click Save from the Quick Access toolbar. 8. Click File > Manage Session > Erase Current > Yes to erase the model from memory. This completes the exercise.

Module 13 | Page 2

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Exercise 2: Creating Coaxial Holes Objectives After successfully completing this exercise, you will be able to: • Create axes through cylinders. • Create linear axes. • Create coaxial holes.

Scenario To assemble the drill, you must create holes on a number of parts that act as bolt interfaces. You create the holes with predefined shapes that remove material on the front engine block to enable you to insert bolts during assembly. Close Window Hole\Coaxial Task 1:

Erase Not Displayed ENG_BLOCK_FRONT.PRT

Create a datum axis through a cylinder and a coaxial hole feature.

1. Enable only the following Datum Display type: . 2. From the Datum group, click Axis . • Select the cylindrical surface shown in the upper figure as the reference. • Select the Properties tab from the Datum Axis dialog box and type GEARBOX1 as the Name. • Click OK. The axis should remain selected between these steps. Do not click in the graphics window, as this will de-select it.

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Module 13 | Page 3

3. With datum axis GEARBOX1 still selected from the (highlighted in green), click Hole Engineering group. • Press CTRL and select the surface shown as the second placement reference. from the dashboard. • Click To Next • Edit the diameter to 6 and click Complete . Feature The datum axis GEARBOX1 serves as the first placement reference. The surface reference is the second placement reference. The surface reference provides you with a starting location defining the depth of the hole. 4. Select the axis GEARBOX1 from the model tree and drag it onto the Hole 1 feature. 5. Expand the Hole 1 feature in the model tree and notice that the axis GEARBOX1 is now embedded in the hole feature and hidden. Embedding the axis GEARBOX1 in the hole feature simplifies the model tree and adds additional design intent to the model. Note that all embedded datums are automatically assigned a hidden display status.

Task 2:

Create a second coaxial hole feature using an embedded datum axis.

1. From the Engineering group, click Hole

.

2. In the dashboard, click Datum and select Axis . • Select the cylindrical surface shown in the figure as the reference. • Click OK to complete the feature.

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3. Click Resume Feature to continue creating the hole feature. • Press CTRL and select the surface shown as the second placement reference. from the dashboard. • Click To Next • Edit the diameter to 6 and click Complete . Feature

4. Expand the Hole 2 feature in the model tree and notice that the axis was created as an embedded datum.

Task 3:

Create a linear axis and a coaxial hole feature.

1. Enable Plane Display 2. Click Hole

.

.

and select 3. In the dashboard, click Datum . Select the surface in the location Axis shown in the following figure. Right-click and select Offset References. Press CTRL and select the FRONT and RIGHT datum planes from the model tree. 4. Double-click each distance dimension and type 17.50. Select the Properties tab from the Datum Axis dialog box and type CYLINDER1 as the Name. Click OK to complete the feature.

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Module 13 | Page 5

5. Disable Plane Display

.

6. Click Resume Feature to continue creating the hole feature. • Press CTRL and select the surface shown as the second placement reference. • Edit the diameter to 5 and the depth to 10, then click Complete Feature . You can edit values from the dashboard or directly from the model.


Module 13 | Page 6

© 2014 PTC

Exercise 3: Creating Linear Holes Objectives After successfully completing this exercise, you will be able to: • Create linear holes.

Scenario To assemble the drill, you must create holes on parts that act as bolt interfaces. You create the holes with predefined shapes that remove material on the rear engine block to enable you to insert bolts during assembly. Close Window Hole\Linear Task 1:

Erase Not Displayed ENG_BLOCK_REAR.PRT

Create a linear hole feature.

1. Disable all Datum Display types. 2. From the Engineering group, click Hole and select the surface shown as the placement reference. 3. Right-click and select Offset References Collector. Press CTRL and select datum planes FRONT and RIGHT from the model tree as the offset references. You can also drag the reference handles to snap to reference. 4. Drag the location, diameter, and depth handles to the approximate positions shown. 5. Edit the diameter to 5 and the depth to 10 in the dashboard. Then select the Placement tab in the dashboard and type 17.5 for the offset values. Click Complete Feature . You can edit values from the dashboard or directly from the model. To move the hole to the opposite side of the model, you can either drag the hole using the handles or you can type a negative value. The negative value moves the hole to the opposite side of the RIGHT datum plane. 6. Click Save from the Quick Access toolbar. 7. Click File > Manage Session > Erase Current > Yes to erase the model from memory.

This completes the exercise. © 2014 PTC

Module 13 | Page 7

Exercise 4: Creating Radial and Diameter Holes Objectives After successfully completing this exercise, you will be able to: • Create a radial hole on a cylindrical surface.

Scenario Add an additional hole to the chuck part for the chuck key. Close Window

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Hole\Radial_Diameter Task 1:

CHUCK.PRT

Create a radial hole feature.

1. Enable only the following Datum Display type: . 2. From the Engineering group, click Hole . • Select the cylindrical surface in the location shown. It is important to select the surface in the quadrant shown below, to ensure that the angle is measured properly.

3. In the graphics window, right-click and select Offset References Collector. • Press CTRL and select datum planes FRONT and TOP from the model tree. • Select the Placement tab from the dashboard. Edit the angle to 60 and the axial distance to 52.5. • Edit the diameter to 5.5 and the depth to 8, as shown.

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4. Click Complete Feature 5. Disable Plane Display

. .

6. Click Save from the Quick Access toolbar. 7. Click File > Manage Session > Erase Current > Yes to erase the model from memory.


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Module 13 | Page 9

Exercise 5: Shelling the Fuel Tank Objectives After successfully completing this exercise, you will be able to: • Create shell features that remove single surfaces.

Scenario To complete the drill’s fuel tank, you hollow out the part and create an opening using a shell which provides the drill with a gasoline storage location. Close Window Shell\Shell Task 1:

Erase Not Displayed FUEL_TANK_SHELL.PRT

Create a shell feature.

1. Disable all Datum Display types. 2. From the Engineering group, click Shell . 3. Select the surface for the shell to remove, as shown. 4. Edit the shell thickness to 1 and click Preview from the dashboard. Feature

5. Click Resume Feature to 3. 6. Click Complete Feature

and edit the thickness .


Module 13 | Page 10

© 2014 PTC

Module 14 Creating Rounds and Chamfers

© 2014 PTC

Module 14 | Page 1

Exercise 1: Creating Rounds on the Rear Engine Block 1 Objectives After successfully completing this exercise, you will be able to: • Create an edge to surface round.

Scenario Create an edge to surface round on a boss that is part of the engine block. Close Window

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Round\Surface-Edge Task 1:

ENG_BLOCK_REAR_1.PRT

Attempt an edge chain round on ENG_BLOCK_REAR_1.PRT.

1. Disable all Datum Display types. 2. Click Named Views from the In Graphics toolbar and select ROUND. from the Round types 3. Select Round drop-down menu in the Engineering group. • Press CTRL and select the two edges shown. Edit the radius to 2. from the Round • Click Preview Feature dashboard. Notice that the Troubleshooter dialog box appears because the rounds overlap. • Click Cancel in the Troubleshooter dialog box and click Yes. • Click Cancel Feature dashboard. Click Yes.

Task 2:

from the Round

Create a surface-to-edge round on ENG_BLOCK_REAR_1.PRT.

1. Click Round . • Select the surface shown. • Press CTRL and select the edge shown. • Edit the radius to 4.

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2. Click Complete Feature dashboard.

from the Round



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Module 14 | Page 3

Exercise 2: Creating Rounds on the Gearbox Front Objectives After successfully completing this exercise, you will be able to: • Create basic rounds.

Scenario In order to reduce stresses and remove sharp edges, add rounds to the front gearbox. Close Window Round\Gearbox Task 1:

Erase Not Displayed GEARBOX_FRONT.PRT

Create the first of three edge round features on GEARBOX_FRONT.PRT.

1. Disable all Datum Display types. 2. Select Round from the Round types drop-down menu in the Engineering group and select the large circular edge as shown. • Drag the radius handle to 5.

3. Press CTRL and select the small circular edge to add it to the round set. 4. Type 3 as the radius in the Round dashboard, and notice that both rounds update. 5. Select the Sets tab in the Round dashboard. Select the Edge:F7(PROTRUSION) reference, right-click and select Remove. You can also de-select references by pressing CTRL and selecting the reference. 6. Click Complete Feature dashboard.

from the Round

7. Click Round and select the large circular edge as shown. 8. Edit the radius to 2 and click Complete Feature .

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Task 2:

Create the second of three edge round features on GEARBOX_FRONT.PRT.

1. Click Named Views from the In Graphics toolbar and select 3D_BACK. , select the edge shown, and 2. Click Round edit its radius to 2. 3. Click Complete Feature

.

4. Click Round . • Select the surface highlighted in green, as shown. • Press CTRL and select the edge shown. • Drag the radius handle to 6 and click . Complete Feature

Task 3:

Create the final edge round feature on GEARBOX_FRONT.PRT.

1. Select the RIB_ROUND from the model tree, right-click, and select Edit Definition . • Press CTRL and select the two additional edge references shown.

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Module 14 | Page 5


.



Module 14 | Page 6

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Exercise 3: Creating Rounds on the Rear Engine Block 2 Objectives After successfully completing this exercise, you will be able to: • Create a surface to surface round.

Scenario Create a surface to surface round on a boss that is part of the engine block. Close Window

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Round\Surface-Surface Task 1:

ENG_BLOCK_REAR_2.PRT

Create a surface to surface round on ENG_BLOCK_REAR_2.PRT.

1. Disable all Datum Display types. 2. Click Named Views from the In Graphics toolbar and select ROUND. from the Round types 3. Select Round drop-down menu in the Engineering group. • Press CTRL and click the two surfaces, as shown. • Edit the radius to 4.

4. Click Complete Feature dashboard.

from the Round



© 2014 PTC

Module 14 | Page 7

Exercise 4: Creating Full Rounds on the Connecting Rod Objectives After successfully completing this exercise, you will be able to: • Create full rounds.

Scenario In order to reduce stresses and remove sharp edges, add rounds to the connecting rod. Close Window Round\Full Task 1:

Erase Not Displayed CONNECTING_ROD.PRT

Create a full round on CONNECTING_ROD.PRT.

1. Disable all Datum Display types. 2. Select Round from the Round types drop-down menu in the Engineering group. 3. Press CTRL and select the two edges shown.

4. Right-click and select Full round. 5. Click Complete Feature

Task 2:

.

Create edge rounds on CONNECTING_ROD.PRT.

1. Click Round . 2. Press CTRL and select the two edges as shown. 3. Edit the radius to 2.


.


This completes the exercise. Module 14 | Page 8

© 2014 PTC

Exercise 5: Creating Chamfers on the Crankshaft Objectives After successfully completing this exercise, you will be able to: • Create chamfers.

Scenario In this exercise, you create multiple chamfers on the crankshaft. Close Window Chamfer\Sets Task 1:

Erase Not Displayed CRANKSHAFT.PRT

Create the first of three chamfer features on CRANKSHAFT.PRT.

1. Disable all Datum Display types. 2. Select Edge Chamfer from the Chamfer types drop-down menu in the Engineering group. 3. Select the far-left circular edge, and edit its value to 2 using the Chamfer dashboard.

4. Select the far-right circular edge of the crankshaft (without pressing CTRL). 5. Drag the distance handle to 1, then edit its value to 2, as shown. 6. Click Complete Feature

.

The chamfer sets are independent of each other. Selecting references without pressing CTRL creates independent sets. Selecting while pressing CTRL adds/removes references to the same set. Task 2:

Create the second of three chamfer features on CRANKSHAFT.PRT.

1. Select Edge Chamfer and select the edge shown. • Select the D1 x D2 dimension scheme in the dashboard. • Edit D1 to 2 and D2 to 3 in the dashboard. • Click Interchange Distances • Click Preview Feature

© 2014 PTC

.

in the dashboard.

Module 14 | Page 9

2. Click Resume Feature . • Select the Angle x D dimension scheme in the dashboard. . • Click Switch Surfaces • Edit the angle to 15 and the distance to 3 by double-clicking the model dimensions. • Click Complete Feature

Task 3:

.

Create the final chamfer feature on CRANKSHAFT.PRT.

1. Select Edge Chamfer . • Press CTRL and select the two edges shown. • Edit the chamfer distance to 2. • Click Complete Feature

.

Unlike the previous chamfers, this one has added material.


Module 14 | Page 10

© 2014 PTC

Module 15 Project I

© 2014 PTC

Module 15 | Page 1

Objective 1: Creating the PISTON_PIN.PRT Scenario ACME Incorporated develops and markets several consumer, industrial, and defense goods. The Light Industrial Division of ACME creates a number of products, including industrial fans, heating, air conditioning, and pumps. You work for the Light Industrial Division of ACME Inc., which has recently started using Creo Parametric for its product designs. Upon returning from Creo Parametric training, you are assigned to create the AC-40 Air Circulator. You apply the skills learned in previous topics of this course to create the final assembly and components of the air circulator. Close Window

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Projects\Intro-1_working Task 1:

CREATE NEW

Create the piston pin part.

1. Create a new part named PISTON_PIN.PRT. 2. Enable only the following Datum Display types: . 3. Create the extrude feature, as shown. 4. Save the model and close the window. You must center the model on datum plane FRONT. Use the mmns_part_solid template for this and all models in this project. To help verify the correct datum entities, enable datum tag display for this project. This completes the objective.

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Objective 2: Creating the PISTON.PRT Task 1:

Create the piston part and extrude the main body.

1. Create a new part named PISTON.PRT. 2. Create the extrude feature, as shown. Use the mmns_part_solid template for this and all models in this project.

Task 2:

Hollow the piston to make room for the connecting rod.

1. Remove material, as shown. 2. Rename the cut as OVAL_CUT. The sketch should be symmetric about the vertical reference. Control the upper wall thickness of the piston by placing the sketch on an embedded datum plane, offset from datum plane TOP. Regardless of the length of the original protrusion, the cut should always extrude though the entire model.

Task 3:

Remove material from the bottom of the piston.

1. Remove material, as shown.

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Module 15 | Page 3

Task 4:

Create a hole to attach the piston pin.

1. Create a hole through the model. The hole should be placed on datum plane FRONT and its depth should extend through the entire model in both directions. It should be aligned to datum plane RIGHT.

Task 5:

Apply an appearance to the piston.

1. Apply the Blue_Dark appearance to the model. 2. Save the model and close the window.

This completes the objective.

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© 2014 PTC

Objective 3: Creating the CONNECTING_ROD.PRT Task 1:

Create the connecting rod and extrude the main body.

1. Create a new part named CONNECTING_ROD. PRT. Use the mmns_part_solid template for this and all models in this project. 2. Create the extrude feature, as shown. Create the sketch on datum plane FRONT, and extrude it symmetric about datum plane FRONT. Sketch two circles, two tangent lines, and then use dynamic trim to create the sketch. Because this is the first feature of the model, with the Lock Scale option to use Modify modify the dimension values. Task 2:

Create extrude features at both ends of the connecting rod.

1. Create two extrude features, one at each end of the connecting rod. The extrude features should be symmetric about datum plane FRONT.

Task 3:

Create holes at each end of the connecting rod.

1. Create coaxial holes at both ends of the connecting rod. The hole depths should extend through the entire model. Create embedded axes to locate each hole.

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Module 15 | Page 5

Task 4:

Create a round to strengthen the connecting rod.

1. Create a round feature, as shown. Each of the four rounded edges should be driven by the same dimension.

Task 5:

Create a lubrication hole.

1. Create a radial hole on the right end of the model. The hole depth should only extend through the next surface.

Task 6:

Apply an appearance to the connecting rod.



Module 15 | Page 6

© 2014 PTC

Objective 4: Creating the CRANKSHAFT.PRT Task 1:

Create the crankshaft and extrude the main body.

1. Create a new part named CRANKSHAFT.PRT. Use the mmns_part_solid template for this and all models in this project. 2. Create the extrude feature, as shown.

Task 2:

Create the crankshaft lobe.

1. Create an extrude feature, as shown. Use a construction circle to control the outer diameter of the lobe and a vertical centerline to imply symmetry.

© 2014 PTC

Module 15 | Page 7

Task 3:

Create the crankshaft pin.

1. Create an extrude feature, as shown.

Task 4:

Create a hole to hollow out a portion of the crankshaft.

1. Create a hole, as shown. The hole should be coaxial to the original cylindrical feature.

Module 15 | Page 8

© 2014 PTC

Task 5:

Create an opening for intake gases to enter the crankcase.

1. Remove material, as shown. 2. Rename this cut as INTAKE_CUT. The cut's sketch plane should be embedded in the cut feature. The cut should extend through only one side of the crankshaft.

Task 6:

Create a cut that is used to interlock with the impeller.

1. Remove material, as shown. The cut should not affect the overall length of the model.

© 2014 PTC

Module 15 | Page 9

Task 7:

Create a cut to form a circular shaft for threads.

1. Remove material, as shown. The cut should not affect the overall length of the model.

Task 8:

Bevel the edges of the intake cut and the end of the crankshaft.

1. Create a chamfer, as shown. Both legs of the chamfer should have the same dimension (D x D).

Task 9:

Apply an appearance and save the orientation.

1. Apply the Gray_Dark appearance to the model. 2. Save the current orientation to an orientation named 3D. 3. Save the model and close the window.


Module 15 | Page 10

© 2014 PTC

Objective 5: Creating the ENGINE_BLOCK.PRT Task 1:

Create the engine block part and revolve the main body of the model.

1. Create a new part named ENGINE_BLOCK.PRT Use the mmns_part_solid template for this and all models in this project. 2. Create the revolve feature, as shown.

Task 2:

Create datum features to use as references when constructing other features.

1. Create a datum plane offset from datum plane FRONT. Rename the plane to CTR. 2. Create a datum axis at the intersection of datum planes RIGHT and CTR. Rename the axis to CYL. Datum plane CTR and axis CYL are used later in the project as references for other features.

© 2014 PTC

Module 15 | Page 11

Task 3:

Create the engine block cylinder.

1. Create a straight three-section parallel blend protrusion, as shown. Sketch on datum plane TOP, and select datum plane CTR as a horizontal dimensioning reference. The second and third blend sections are identical. Specify Straight as the Option.

Module 15 | Page 12

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Task 4:

Add rounds to shape the cylinder.

1. Create a round on the four edges of the blend.

2. Create a single round feature, as shown.

© 2014 PTC

Module 15 | Page 13

Task 5:

Create a protrusion to use as a mounting flange.

1. Create an extrude feature, as shown. Select datum plane CTR and the silhouette edges of the revolve feature as references. The sketch should be symmetrical about datum plane CTR and mirrored about the vertical centerline. The depth of the feature should be symmetric about datum plane TOP.

Task 6:

Create mounting bolt holes.

1. Create coaxial holes, as shown. Create an embedded datum axis for each hole. The datum axes should be placed through the mounting flange arc centers.

Module 15 | Page 14

© 2014 PTC

2. Mirror the two holes to the other side of the engine block. 3. Group the extrude, two holes, and the mirror feature. 4. Rename the group as MOUNT1 .

Task 7:

Create holes for the crankshaft, crankcase, and cylinder bore.

1. Create a hole through the engine block.

2. Create another hole, as shown.

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Module 15 | Page 15

3. Create the cylinder bore hole, as shown. 4. Rename this hole as BORE. 5. Save the model and close the window.


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Objective 6: Creating the IMPELLER_HOUSING.PRT Task 1:

Create the impeller housing and extrude the main body of the model.

1. Create a new part named IMPELLER_ HOUSING.PRT. Use the mmns_part_solid template for this and all models in this project. 2. Create an extrude feature, as shown.

Task 2:

Begin creation of the exhaust geometry.

1. Create a 90° revolve feature, as shown. Create the sketch on datum plane TOP. The sketch should be symmetric about the horizontal reference.

© 2014 PTC

Module 15 | Page 17

Task 3:

Create the exhaust geometry.

1. Create a smooth parallel blend feature, as shown. This blend contains three symmetric rectangular sketches, each 25 mm apart. The first section should use the edges from the revolve feature. Be sure that the start point for each rectangle is at the same location and direction.

Task 4:

Shape the exhaust for maximum airflow.

1. Create round features, as shown.

Module 15 | Page 18

© 2014 PTC

Hollow out the housing.

Task 5:

1. Create a shell feature, as shown. Two surfaces are to be removed using this shell feature.

Task 6:

Create a hole for the impeller collar.

1. Create a hole feature, as shown.

© 2014 PTC

Module 15 | Page 19

Task 7:

Create the bolting flange.

1. Create an extrude feature, as shown. The extrude feature should extend over the model, as shown.

Task 8:

Create the mounting flange.

1. Create an extrude feature, as shown. The extrude feature should extend symmetrically in both directions from the datum plane FRONT.

Module 15 | Page 20

© 2014 PTC

Task 9:

Create an attach hole in the mounting flange.

1. Create the hole, as shown.

Task 10:

Create a profile rib to strengthen the mounting flange.

1. Create the profile rib feature on an embedded datum, as shown. The rib should be symmetric about the embedded datum. 2. Save the model and close the window.


© 2014 PTC

Module 15 | Page 21

Objective 7: Creating the IMPELLER.PRT Task 1:

Create the impeller and revolve the main body of the model.

1. Create a new part named IMPELLER.PRT. Use the mmns_part_solid template for this and all models in this project. 2. Create a revolve feature, as shown. Sketch on datum plane RIGHT with datum plane TOP facing right.

Task 2:

Create the interlock geometry.

1. Extrude the cut feature, as shown. Create the sketch on the small circular surface on the back of the model, orienting datum plane TOP so that it faces the top.

Module 15 | Page 22

© 2014 PTC

Task 3:

Create the first impeller blade.

1. Create an extrude feature with the thicken option, as shown. 2. Rename the extrude to BLADE. Create the sketch on datum plane FRONT so that it extrudes through the model. Dimension the arc using an arc angle dimension.

Task 4:

Round the sharp corner of the blade.

1. Create a round feature, as shown. 2. Rename the round feature to BLADE_ROUND.

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Module 15 | Page 23

Task 5:

Create an outer support for the blade.

1. Create an extrude feature, as shown. The depth of this feature should extend from the end of the blade, inward over the model. 2. Save and close the model.


Module 15 | Page 24

© 2014 PTC

Objective 8: Creating the FRAME.PRT Task 1:

Create the frame part and trajectory for the main rail.

1. Create a new part named FRAME.PRT. Use the mmns_part_solid template for this and all models in this project. 2. Create a sketch feature, as shown. This sketch can be used as the trajectory for a swept protrusion.

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Module 15 | Page 25

Task 2:

Sweep an I-profile section along the sketch trajectory.

1. Create a constant section sweep protrusion, as shown. Select the predefined I-profile from the as the section to sweep. Relocate Palette the X Location handle to the midpoint of the bottom edge. The section should be symmetric about the vertical reference and above the horizontal reference and trajectory.

Task 3:

Sweep another I-profile for the engine support.

1. Create a sketch feature on an embedded datum plane, as shown. This feature is the trajectory for your next sweep. Use datum plane FRONT as a dimensioning reference.

Module 15 | Page 26

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2. Create a swept protrusion, as shown. 3. Save the model and close the window.


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Module 15 | Page 27

Objective 9: Creating the BOLT.PRT Task 1:

Create the bolt and revolve the main body.

1. Create a new part named BOLT_5.PRT. Use the mmns_part_solid template for this and all models in this project. 2. Create the revolve feature, as shown.

Task 2:

Create a hex socket cut.

1. Remove material, as shown. Select the predefined 6–sided Hexagon section from the Palette as the section to extrude.

Module 15 | Page 28

© 2014 PTC

Task 3:

Create finishing features.

1. Create a round and chamfer, as shown. 2. Apply the Black appearance to the bolt. 3. Save the model.

Task 4:

Create two additional bolts of different lengths.

1. Save a copy of the part BOLT_5.PRT. Rename it as BOLT_8.PRT. 2. Close the window. 3. Open the new part BOLT_8.PRT. 4. Edit the length of the model from 5 to 8 and save the model.

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Module 15 | Page 29

5. Save a copy of the part BOLT_8.PRT. Rename it as BOLT_12.PRT. 6. Close the window. 7. Open the new part BOLT_12.PRT. 8. Edit the length of the model from 8 to 12. 9. Save the model and close the window.


Module 15 | Page 30

© 2014 PTC

Module 16 Group, Copy, and Mirror Tools

© 2014 PTC

Module 16 | Page 1

Exercise 1: Rotating a Copy of a Boss on the Engine Block Objectives After successfully completing this exercise, you will be able to: • Copy features by rotation.

Scenario In this topic, you will create a copy of a boss on the engine block. Close Window

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Feature_Operations\Move_Rotate Task 1:

ENG_BLOCK_REAR.PRT

Copy a boss on ENG_BLOCK_REAR.PRT.

1. Enable only the following Datum Display types: . 2. Select Group BOSS_1 from the model tree.

3. Copy the BOSS_1 group, as shown: • With the BOSS_1 group still selected, click Copy from the Operations group. • Select Paste Special from the Paste types drop-down menu in the Operations group. • Select the Apply move/rotate transformations to copies check box. • Click OK in the Paste Special dialog box. from the dashboard and • Select Rotate select datum axis MAIN. • Drag the angle handle counterclockwise and then type 120 for the angle in the dashboard. • Click Complete Feature dashboard.

Module 16 | Page 2

from the

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4. Expand Moved Copy 1 and Group COPIED_GROUP in the model tree. Press CTRL, select the datum plane and sketch, . right-click, and select Hide 5. Select Moved Copy 1, right-click, and select Rename. Type BOSS_2 and press ENTER. 6. Select the Group COPIED_GROUP from the . model tree, right-click, and select Edit Double-click the angle dimension and type 100. 7. Expand Group BOSS_1 and select the BOSS_HOLE feature. Double-click the diameter dimension and edit it to 5. Click in the background twice to de-select all features. 8. Click Undo toolbar.

twice from the Quick Access


© 2014 PTC

Module 16 | Page 3

Exercise 2: Copying and Translating Carburetor Features Objectives After successfully completing this exercise, you will be able to: • Copy features by translation.

Scenario In this topic, you will create a copy of an attachment ear on the carburetor. Close Window

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Feature_Operations\Move_Rotate Task 1:

CARBURETOR_1.PRT

Copy and translate the features on CARBURETOR_1.PRT.

1. Enable only the following Datum Display types: . 2. Select Group EAR from the model tree.

3. Copy the EAR group, as shown: • With the EAR group still selected, click Copy from the Operations group. • Select Paste Special from the Paste types drop-down menu in the Operations group. • Select the Apply move/rotate transformations to copies check box. • Click OK in the Paste Special dialog box. from the dashboard and • Click Translate select datum plane FRONT from the model tree. • Drag the offset handle forward, type 23.5, and press ENTER. • Click Complete Feature dashboard.

Module 16 | Page 4

from the

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4. Select the Moved Copy, right-click, and select Rename. Type EAR2 and press ENTER. 5. Click Save from the Quick Access toolbar. 6. Click File > Manage Session > Erase Current > Yes to erase the model from memory.


© 2014 PTC

Module 16 | Page 5

Exercise 3: Mirroring Selected Carburetor Features Objectives After successfully completing this exercise, you will be able to: • Mirror selected features.

Scenario In this topic, you will create a copy of an attachment ear on the carburetor. Close Window

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Feature_Operations\Mirror_Features Task 1:

CARBURETOR_2.PRT

Mirror the features on CARBURETOR_2.PRT.

1. Enable only the following Datum Display types: . 2. Mirror the EAR groups, as shown: • Press CTRL and select Group EAR and feature EAR2 from the model tree. from the Editing group. • Click Mirror • Select datum plane RIGHT from the model tree. • Click Complete Feature dashboard.

from the


Module 16 | Page 6

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Module 17 Creating Patterns

© 2014 PTC

Module 17 | Page 1

Exercise 1: Patterning Vents Using a Two Directional Pattern Objectives After successfully completing this exercise, you will be able to: • Create direction patterns in two directions.

Scenario You are assigned to increase the number of vents on the engine cover model. Complete this task quickly using a directional pattern. Close Window

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Pattern\Direction_Second Task 1:

ENGINE_COVER.PRT

Pattern the side vents on ENGINE_COVER.PRT.

1. Disable all Datum Display types. 2. From the In Graphics toolbar, click Named and select LEFT. Views 3. Select the SIDE_VENT group from the model tree, right-click, and select Pattern . 4. Edit the pattern type to Direction in the dashboard and create a pattern, as shown: • Select datum plane FRONT from the model tree as the direction reference. • Right-click and select Direction 2 Reference. • Select datum plane TOP from the model tree. in the • Click Flip Second Direction dashboard. • Edit the number of members in the first direction to 3 and its spacing to 23. • Edit the number of members in the second direction to 5 and its spacing to 8. 5. Click Complete Feature dashboard.

from the Pattern



Module 17 | Page 2

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Exercise 2: Creating Flywheel Blades Using an Axis Pattern Objectives After successfully completing this exercise, you will be able to: • Create axial patterns.

Scenario You are assigned to increase the number of blades on the flywheel model. Complete this task quickly using an axial pattern. Close Window

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Pattern\Axis_First Task 1:

FLYWHEEL.PRT

Create an axis pattern on the FLYWHEEL.PRT.

1. Enable only the following Datum Display types: . 2. Select Group BLADE from the model tree, right-click, and select Pattern . 3. In the Pattern dashboard, edit the pattern type to Axis and create a pattern, as shown: • Select datum axis CRANK from the model as the axis reference. • Drag the angle handle on the model to approximately 45°. • Edit the number of members in the dashboard from 4 to 6, and then drag the angle handle on the model to approximately 30°. • In the dashboard, click Set Angular Extent . • Edit the number of members in the dashboard from 6 to 16. 4. Click Complete Feature from the Pattern dashboard. The pattern takes a few moments to calculate. from the Quick Access toolbar. 5. Click Save 6. Click File > Manage Session > Erase Current > Yes to erase the model from memory.

This completes the exercise. © 2014 PTC

Module 17 | Page 3

Exercise 3: Creating Exhaust Cuts in the Muffler Using a Two Directional Axis Pattern Objectives After successfully completing this exercise, you will be able to: • Create axial patterns in two directions.

Scenario You are assigned to create exhaust cuts in the muffler model. Complete this task quickly using an axis pattern in two directions. Close Window

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Pattern\Axis_Second Task 1:

MUFFLER_PATTERN.PRT

Create a two directional axis pattern on MUFFLER_PATTERN.PRT.

1. Enable only the following Datum Display types: . 2. From the In Graphics toolbar, click Named and select TOP. Views 3. Select feature EXHAUST from the model tree, right-click, and select Pattern . 4. Select the pattern type Axis in the dashboard and create a pattern, as shown: • Select datum axis CENTER from the model as the axis reference. • Edit the number of members in the first direction from 4 to 6. to evenly space • Click Set Angular Extent the instances. • Edit the number of members in the second direction to 5 with a spacing of 3. 5. Click Complete Feature 6. Disable Axis Display

Module 17 | Page 4

. .

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7. Select Pattern 1 of EXHAUST in the model tree, right-click, and select Edit Definition . • Select the Dimensions tab from the dashboard and activate the Direction 2 dimension collector. • Select the 0.5 dimension from the graphics window and edit the Increment to 3.


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Module 17 | Page 5

Exercise 4: Patterning Rounds on the Cylinder Fins Using Reference Patterns Objectives After successfully completing this exercise, you will be able to: • Create reference patterns of features.

Scenario You are assigned to add some rounds to the fins on the cylinder model. Complete this task quickly using a Reference pattern. Close Window

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Pattern\Reference_Features Task 1:

CYLINDER_2.PRT

Create and reference pattern a round on the cooling fins of CYLINDER_2.PRT.

1. Disable all Datum Display types. 2. Create a full round, as shown: • From the In Graphics toolbar, click Named and select FIN_CUT. Views • Select Round from the Round types drop-down menu in the Engineering group. • Select the upper surface of the fin, as shown. • Press CTRL, right-click to query the underside surface of the same fin, and select it. • Select the outer thin surface of the fin. • Click Complete Feature dashboard.

from the

3. Orient to the Standard Orientation. 4. With the previous round still selected, select from the Pattern types drop-down Pattern menu in the Editing group.

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5. Notice that the Reference pattern type is specified in the dashboard. 6. Click Complete Feature

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Module 18 Measuring and Inspecting Models

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Module 18 | Page 1

Exercise 1: Analyzing Design Models Objectives After successfully completing this exercise, you will be able to: • Configure the mass properties of a model. • Analyze components for distance, angles, surface area, and interferences.

Scenario While designing a drill at your company, your manager asks you to confirm that the component models adhere to the design specifications. For example, you need to verify the mass properties of the fuel tank to confirm that the raw material estimates are correct. Next, you need to calculate the surface area of the cylinder to confirm the proper thermal cooling. Also, the crankshaft's center of gravity needs to be set along the axis of rotation. Finally, you need to check the engine assembly for interferences between its components. Close Window Analysis\Models Task 1:

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Analyze the FUEL_TANK.PRT. Determine the volume of fluid that fits in a full tank. Also determine the volume and mass of material to use when molding the part.

1. Disable all Datum Display types. 2. Click File > Prepare > Model Properties to access the Model Properties dialog box. Notice the current system of units specified in the Units row of the Materials section. 3. Click Close in the Model Properties dialog box. 4. Select the Analysis tab from the ribbon. 5. Click Mass Properties from the Model Report group. 6. Type the Density (kg/mm3) for the nylon fuel tank as 1.2E-6 in the Mass Properties dialog box. 7. Click Preview in the Mass Properties dialog box. Notice the computed volume and mass values. 8. Click OK in the Mass Properties dialog box. 9. Select the Model tab. 10. Click the Operations group drop-down menu and select Resume > Resume All to resume the SHELL TANK feature. 11. In the ribbon, select the Analysis tab. 12. Click Mass Properties . • Click Preview. • Notice that the values have updated, as shown in the following figure.

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13. Note that the volume of the fluid that fills the tank can be computed as follows: VOLUME_BEFORE_SHELL – VOLUME_AFTER_SHELL = FLUID_VOLUME 434,300 – 101,600 = 332,700 MM3 = 0.333 L. 14. The volume of material required to mold the tank model is approximately 101,600 mm3. 15. The mass of material required to mold the tank model is approximately 0.122 KG. 16. Click OK in the Mass Properties dialog box. 17. Click Save from the Quick Access toolbar. 18. Click File > Manage Session > Erase Current > Yes to erase the model from memory. Task 2:

Analyze the mass properties of the CYLINDER.PRT. Determine whether the model has adequate surface area for air-cooling the engine. Thermal analysis has indicated that the surface area must be greater than 50,000 mm2.

1. Click Open from the Quick Access toolbar. • Select the CYLINDER.PRT and click Open.

2. Click File > Prepare > Model Properties. Notice the current system of units specified in the Units row of the Materials section. 3. In the Materials section, click change in the Mass Properties row. Type the Density (kg/mm3) for the cylinder as 2.7E-6 and click OK in the Mass Properties dialog box. in the 4. In the Materials section, click Info Mass Properties row. Notice the surface area of the model, as shown in the following figure. 5. The surface area of the model is approximately 64,290 mm2. This is greater than the stated minimum requirement of 50,000 mm2 for air-cooling the engine. If the calculated value does not meet the specification, we could modify the pattern to add additional cooling fins. 6. Close the Mass Properties Report dialog box and click Close in the Model Properties dialog box.

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Task 3:

Determine the diameter of the spark plug hole to ensure that sufficient material is present to tap threads for a standard 16 mm spark plug. At least 2 mm smaller is required.

1. Select the Analysis tab from the ribbon. 2. In the Measure group, select Diameter from the Measure types drop-down menu and select the cylindrical surface of the spark plug hole, as shown. 3. Note that the diameter is 13.75 mm. Since this value is less than 14 mm, it meets the requirement.

Task 4:

Measure the area of the base of the cylinder to determine whether there is sufficient surface area to adequately seal the cylinder to the crankcase. For an engine of this displacement, the recommended gasket surface area is at least 850 mm2.

1. Orient the model, as shown. 2. Click Area from the Measure dialog box. Select the engine block interface surface, as shown. 3. Note that the area is 1,005.55mm2. Since this value is greater than 850 mm2, it meets the requirement.

Task 5:

Measure the distance between the exhaust and intake surfaces.

1. Orient the model, as shown. 2. Click Distance from the Measure dialog box. • Edit the selection filter to Surface. • Select the exhaust interface surface, as shown.

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3. Reorient the model. 4. Press CTRL and select the carburetor interface surface, as shown. 5. Note that the distance is 62mm. 6. Close the Measure dialog box. 7. Click Save . 8. Click File > Manage Session > Erase Current > Yes to erase the model from memory.

Task 6:

Analyze the mass properties of the CRANKSHAFT.PRT. Determine the location of the center of gravity (COG) on the model.

1. Click Open . • Select the CRANKSHAFT.PRT and click Open 2. Click File > Prepare > Model Properties. Notice the current system of units specified in the Units row of the Materials section. 3. In the Materials section, click change in the Mass Properties row. • Type the Density (kg/mm3) for the steel crankshaft as 7.8E-6 and click OK in the Mass Properties dialog box. • Click Close in the Model Properties dialog box. 4. Click Named Views and select RIGHT. 5. Select the Analysis tab from the ribbon. 6. Click Mass Properties and click Preview. Note that the center of gravity (indicated by the arrow) is below the axis of revolution (horizontal axis of the other coordinate system). The system displays the default coordinate system as a reference when computing model mass properties. 7. Click OK in the Mass Properties dialog box.

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Module 18 | Page 5

Task 7:

Measure the CRANKSHAFT.PRT. Determine the length of the keyway slot. This length must be between 11 mm and 12 mm so the flywheel key does not shear during normal operating conditions.

1. Reorient the model. from 2. In the Measure group, select Length the Measure types drop-down menu. • Select the edge of the keyway. 3. Note that the distance is approximately 8.19mm. This value does not meet the requirement. and 4. In the Measure dialog box, click Save select Save Analysis. • Type KEYWAY_LENGTH in the text box field and click OK. • Close the Measure dialog box. 5. Click Saved Analysis from the Manage group to open the Saved Analysis dialog box. Click All > Hide All. This hides the analysis from the graphics window. Close the Saved Analysis dialog box. 6. Select the KEYWAY feature from the model tree, then right-click and select Edit . • Edit the diameter from 13 to 15.5. • Click twice in the background of the graphics window to de-select all features. and double-click 7. Click Saved Analysis the KEYWAY_LENGTH analysis in the Saved Analysis dialog box. 8. Note that the distance is now 11.75mm. This value meets the requirement. If the Saved Analysis is left unhidden, the result of the analysis automatically updates in the graphics window. Icons enable you to easily determine whether the analysis is unhidden or hidden. 9. Close the Measure dialog box. 10. In the Saved Analysis dialog box, select the KEYWAY_LENGTH analysis and click Delete Analysis to delete it. 11. Close the Saved Analysis dialog box.

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Task 8:

Measure the angle between the lobes of the CRANKSHAFT.PRT.

1. Orient to the standard orientation. from the 2. In the Measure group, select Angle Measure types drop-down menu. • Edit the Selection Filter to Surface. • Select the left surface. • Press CTRL and select the right surface.

3. The indicated angle is approximately 30°.

4. Expand the Measure dialog box, if necessary, and select Supplement from the Angle drop-down list. The angle is now approximately 150°. 5. Click Close from the Measure dialog box. 6. Click Save . 7. Click File > Manage Session > Erase Current > Yes to erase the model from memory.

Task 9:

Analyze the mass properties of the ENGINE.ASM.

1. Click Open . • Select ENGINE.ASM and click Open.

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Module 18 | Page 7

2. Select the Analysis tab from the ribbon. 3. Click Mass Properties

and click Preview.

The components of the engine have been assigned appropriate density values for either steel or aluminum. 4. Note the displayed values for volume, surface area, average density, mass, and center of gravity. 5. Click OK from the Mass Properties dialog box. Task 10:

Analyze interferences within ENGINE.ASM components.

1. In the Inspect Geometry group, click Global Interference and click Preview. Notice that there is one pair of interfering components. 2. The ENG_BLOCK_REAR.PRT interferes (areas in dark red) with the ENG_BLOCK_FRONT.PRT around the alignment pins. Click OK in the Global Interference dialog box.

Task 11:

Resolve the interference.

1. Resolve the interferences in ENG_BLOCK_ FRONT.PRT by editing the depth of the ALIGN_PINS, as shown in the figure. • Select ENG_BLOCK_FRONT.PRT from the model. • Right-click and select Open . • Select the ALIGN_PINS feature from the model tree. . • Right-click and select Edit Definition Drag the depth handle to 5, editing it if necessary. • Click Complete Feature

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2. Click Close 3. 4. 5. 6.

to return to the ENGINE.ASM.

and click Preview. Click Global Interference The Message Log indicates that there are no interfering parts. Click OK in the Global Interference dialog box. Press CTRL+G to regenerate the assembly.

7. Click Save

.

8. Click File > Manage Session > Erase Current, then click Select All the model from memory.

and OK to erase


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Module 19 Assembling with Constraints

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Module 19 | Page 1

Exercise 1: Creating the Engine Assembly using Automatic Constraints Objectives After successfully completing this exercise, you will be able to: • Create assembly models.

Scenario Assemblies are used to combine parts into larger models. These models can either be a top-level model, which represents the entire product, or a subassembly, that will be further assembled. You are assigned to begin creating the engine assembly, used later in the top-level drill assembly. Close Window

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Assembly\Automatic-Bs Task 1:

CREATE NEW

Create ENGINE.ASM.

1. Click New from the Quick Access toolbar, and select Assembly as the Type. Type engine as the Name, clear the Use default template check box, and click OK. 2. In the New File Options dialog box, select mmks_asm_design as the Template, and click OK. 3. Disable all Datum Display types. 4. Select Assemble from the Assemble types drop-down menu in the Component group, select ENG_BLOCK_REAR.PRT, and click Open. from the

5. Select Constraint Type Default dashboard. 6. Click Complete Component

.

It is a standard practice to constrain the initial component in an assembly using the Default constraint type. 7. Click Assemble . Select ENG_BLOCK_ FRONT.PRT and click Open. 8. Reorient the component approximately, as shown.

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9. Zoom in and select the cylindrical surfaces on an alignment pin and its corresponding hole, as shown by the selection arrows below. Rotate the assembly, if necessary. To easily select the surfaces, zoom in before selecting.

10. Spin the assembly, as shown. 11. Select surfaces from the other pin and hole. 12. Select the Placement tab and notice that a Coincident constraint and Oriented constraint have been automatically created. 13. Notice that the 3D Dragger has dynamically updated to only allow movement in the unconstrained degrees of freedom.

14. Select the two surfaces, as shown by the selection arrows. 15. Notice that this selection has created another Coincident constraint. 16. Click Complete Component dashboard.

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from the

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17. Orient the assembly to the Standard Orientation. . Select CYLINDER.PRT 18. Click Assemble and click Open. 19. Use the 3D Dragger to position the component approximately as shown.

20. Zoom in and select the cylindrical surfaces from a pair of corresponding holes, as shown.

21. Spin the assembly and select cylindrical surfaces from the other pair of corresponding holes, as shown.

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22. Select the two mating surfaces, as shown. 23. Edit the constraint Type to Coincident necessary. 24. Click Complete Component

25. Click Save

, if

.

from the Quick Access toolbar and click OK to save the model.


and OK to erase


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Module 19 | Page 5

Exercise 2: Creating the Drill Chuck Assembly using Automatic Constraints Objectives After successfully completing this exercise, you will be able to: • Create assembly models.

Scenario Assemblies are used to combine parts together into larger models. These models can either be a top-level model, which represents the entire product, or a subassembly, that will be further assembled. You are assigned to begin creating the drill chuck assembly, used later in the top-level drill assembly. Close Window

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CREATE NEW

Create DRILL_CHUCK.ASM.

1. Click New from the Quick Access toolbar, and select Assembly as the Type. Type drill_chuck as the Name, clear the Use default template check box, and click OK. 2. In the New File Options dialog box, select mmks_asm_design as the Template, and click OK. 3. Disable all Datum Display types. 4. Select Assemble from the Assemble types drop-down menu in the Component group, select CHUCK.PRT, and click Open. 5. Right-click and select Default Constraint. 6. Click Complete Component

.

It is a standard practice to constrain the initial component in an assembly using the Default constraint type.

7. Click Assemble , select CHUCK_COLLAR. PRT, and click Open. 8. Use the 3D Dragger to position the component approximately, as shown.

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9. Select cylindrical surfaces to create a Coincident constraint, as shown.

10. Spin the assembly, as shown. Drag the translation arrow to place the component towards the front of the assembly.

11. Select the two surfaces on the back to create a Coincident constraint, as shown.

12. In the dashboard, edit the constraint Type to Distance . Type -10 to establish a better view of the offset and direction. 13. Edit the offset value to 1 and click Complete from the dashboard. Component The CHUCK_COLLAR.PRT is assembled as fully constrained by selecting the Allow Assumptions option. In this case, the rotation of the component is not important.

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Module 19 | Page 7

14. Click Assemble , select STANDARD_BIT. PRT, and click Open. 15. Orient the assembly, as shown. Use the 3D Dragger to position the component approximately as shown.

16. Select cylindrical surfaces to create a Coincident constraint, as shown.

17. Drag the drill bit back out of the chuck using the 3D Dragger. 18. Select the end of the bit and the bottom inside surface of the chuck to create a Coincident constraint, as shown. 19. Edit the constraint Type to Coincident necessary.

20. Click Complete Component

, if

.

from the Quick Access toolbar 21. Click Save and click OK to save the model. 22. Click File > Manage Session > Erase Current, then click Select All and OK to erase the model from memory.


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Exercise 3: Creating the Crank Assembly using Automatic Constraints Objectives After successfully completing this exercise, you will be able to: • Create assembly models.

Scenario Assemblies are used to combine parts together into larger models. These models can either be a top-level model, which represents the entire product, or a subassembly, that will be further assembled. You are assigned to begin creating the crank assembly, used later in the top-level drill assembly. Close Window

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CREATE NEW

Create CRANK.ASM.

1. Click New from the Quick Access toolbar, and select Assembly as the Type. Type crank as the Name, clear the Use default template check box, and click OK. 2. In the New File Options dialog box, select mmks_asm_design as the Template, and click OK. 3. Disable all Datum Display types. 4. Select Assemble from the Assemble types drop-down menu in the Component group, select CRANKSHAFT.PRT, and click Open. 5. Right-click and select Default Constraint. 6. Click Complete Component

.

7. Click Assemble , select FLYWHEEL.PRT, and click Open. 8. Spin the assembly slightly. 9. Use the 3D Dragger to position the component approximately as shown.

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Module 19 | Page 9

10. Select the 2 conical surfaces as shown by the selection arrows.

11. In the dashboard, edit the Constraint Type shown from Coincident to Centered .

12. Enable Plane Display . 13. Right-click in the graphics window and select New Constraint. 14. Zoom in on the assembly. 15. Select the KEY datum planes from each component to create a Coincident constraint.

16. Click Complete Component 17. Disable Plane Display

.

.

18. Click Save from the Quick Access toolbar and click OK to save the model. 19. Click File > Manage Session > Erase Current, then click Select All and OK to erase the model from memory.


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Exercise 4: Creating the Piston Assembly using Automatic Constraints Objectives After successfully completing this exercise, you will be able to: • Create assembly models.

Scenario Assemblies are used to combine parts together into larger models. These models can either be a top-level model, which represents the entire product, or a subassembly, that will be further assembled. You are assigned to begin creating the piston assembly, used later in the top-level drill assembly. Close Window

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CREATE NEW

Create PISTON.ASM.

1. Click New from the Quick Access toolbar, and select Assembly as the Type. Type piston as the Name, clear the Use default template check box, and click OK. 2. In the New File Options dialog box, select mmks_asm_design as the Template, and click OK. 3. Disable all Datum Display types. 4. Select Assemble from the Assemble types drop-down menu in the Component group, select PISTON.PRT, and click Open. 5. Right-click and select Default Constraint. 6. Click Complete Component

.

7. Click Assemble . Select PISTON_PIN.PRT and click Open. 8. Select cylindrical surfaces to create a Coincident constraint, as shown.

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Module 19 | Page 11

9. Use Find to select the next set of assembly references: from the status bar to start the • Click Find Search Tool. Select Datum Plane as the Look for option, select PISTON_PIN.PRT as the Look in object, and click Find Now. • Select FRONT:F3(DATUM PLANE), click Add , and click Close. Item to start the Search Tool. Select • Click Find Datum Plane as the Look for option, select PISTON.PRT as the Look in object, and click Find Now. • Select FRONT:F3(DATUM PLANE), click Add , and click Close. Item • Click Complete Component Using Find assemblies.

.

can be very helpful when selecting references in large, complicated

10. Click Assemble , select PISTON_RING.PRT, and click Open. 11. Use the 3D Dragger to position the component approximately, as shown.

12. Select cylindrical surfaces from the PISTON_RING.PRT and the PISTON.PRT, as shown.

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13. Select the planer surfaces from the PISTON_RING.PRT and the PISTON.PRT, as shown.

14. In the dashboard, select the Placement tab. • Clear the Allow Assumptions check box. 15. Use the 3D Dragger to rotate the piston ring gap to the front. 16. Right-click and select Fix Constraint.

17. Click Complete Component

.

from the Quick Access toolbar 18. Click Save and click OK to save the model. 19. Click File > Manage Session > Erase Current, then click Select All and OK to erase the model from memory.


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Module 22 Drawing Layout and Views

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Module 22 | Page 1

Exercise 1: Creating Drawing Views Objectives After successfully completing this exercise, you will be able to: • Create drawings. • Add views to drawings.

Scenario The Manufacturing Department needs to begin planning the tooling necessary to create the piston part. You must show projected, cross-sectional, and detailed views of the piston. Additionally, a drawing of the completed engine assembly is required to begin planning the assembly process for the engine. For this, you create a second sheet that displays the engine assembly in an exploded state and includes a Bill of Materials. Erase Not Displayed

Close Window

Drawing_Views\Engine Task 1:

PISTON.PRT

Open PISTON.PRT and view the cross-section.

1. Disable all Datum Display types. 2. In the model tree, right-click cross-section A and select Show Section. 3. De-select the section. 4. Click Close

Task 2:

.

Create a new drawing with default views.

1. Click File > New > Drawing and type drill_components. Clear the Use default template check box and click OK to continue. 2. Notice that PISTON.PRT is selected as the Default Model. Select Use template, click Browse, select DRAWING_TEMPLATE.DRW, and click Open. 3. Click OK. Type your first initial, followed by your surname, and press ENTER 4. Note that the drawing template automatically creates three standard views (front, top, right) without displaying any hidden lines. 5. Click Show Navigator tree.

to toggle off the model

The drawing template is a special drawing *.drw file that configures new drawings. In this case, it has also loaded a format *.frm file containing a title block.

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Task 3:

Create projected views of the PISTON.PRT.

1. Select the front view (VIEW_TEMPLATE_1), right-click, and select Projection . Select a point under the front view to create the bottom view, as shown.

2. Create a projected view with a cross-section, as shown: • Select the front view, right-click, and select Projection . Select a location to the left of the front view to place the view. • With the view still selected, right-click, and select Properties. Select the Sections category in the Drawing View dialog box, select 2D cross-section, and click Add . Section • Select section A and click Apply > Cancel. • Right-click and select Add Arrows. Select the front view to place the arrows. • Right-click and clear Lock View Movement , if necessary. Select and move the bottom view downward, away from the section arrows. (Move views by first clicking to select them and then clicking and dragging to relocate them.) • Click in the background to de-select all views.

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Module 22 | Page 3

Task 4:

Insert a detail view.

1. Create a detail view, as shown: from the Model Views group • Click Detailed in the Layout tab. • Zoom in and select an edge of the ring groove cut in the right view (VIEW_TEMPLATE_3) as the detail center point. • Click points to create a spline curve around the selected ring groove cut. Do NOT close the spline curve when sketching it. Instead, leave a gap. • Middle-click to complete the spline curve.

2. Place the detail view, as shown: • Select a point to the right of the top view (VIEW_TEMPLATE_2) to place the detailed view. • Click in an empty area of the graphics window to de-select the view. • Select the view note, double-click the 4.000 scale on the view, type 5, and press ENTER. Click in an empty area of the graphics window to de-select the scale value. • Select the detail note in the right view. Drag it to reposition it as necessary.

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Insert a general view.

Task 5:

1. If necessary, click Refit , and click in the drawing background to de-select all items. 2. Create a general view, as shown: • Right-click and select General . • Click OK in the Select Combined State dialog box. • Select a point in the upper-right corner of the sheet. • Move the Drawing View dialog box away from the view location. • In the Drawing View dialog box, select the 3D orientation and click Apply. • Select the Scale category, select Custom scale, type 3, and click Apply. • Select the View Display category and edit the Display style to Shading. • Click Apply > Cancel. Move views and change view display.

Task 6:

1. Manipulate the drawing, as shown: • Select and drag views to arrange them, as shown. (Move views by first clicking to select them and then clicking and dragging to relocate them.) • Select the cross-section view, right-click, and select Properties. • Select the View Display category. Select None as the Tangent edges display style. • Click OK. You can also change the Display Style of views to display hidden lines. Task 7:

Create a view of ENGINE.ASM.

1. Click anywhere in the drawing background to de-select the previous view. 2. Click Drawing Models from the Model Views group in the Layout tab. Click Add Model from the menu manager. Select ENGINE.ASM and click Open. Click Done/Return from the menu manager. 3. Click New Sheet

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. Type your first initial, followed by your surname, and press ENTER.

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4. Create a general view, as shown: • Right-click and select General . • Click OK to accept the No Combined State selection. • Select a point near the upper-right corner of the sheet. • Select EXPLODE_ORIENTATION as the Model view name and click Apply. • Select the Scale category and verify that Default scale for sheet is selected. • Select the View Display category. Select Shading as the Display style. • Click Apply > Cancel. • Double-click the scale in the lower-left corner of the screen, type 1, and press ENTER. Task 8:

Configure the view to display an explode state.

1. Manipulate the view, as shown. • Select the view, right-click, and select Properties. • Select the View States category and select the Explode components in view check box. • Select ENGINE_EXPLODE from the Assembly explode state drop-down list. • Click Apply > Cancel. • Move the view, as necessary. 2. Click Show Navigator

to toggle it on.

3. Click Save from the Quick Access toolbar and click OK to save the model. 4. Click File > Manage Session > Erase Current, then click Select All and OK to erase the model from memory. This completes the exercise.

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Module 23 Creating Drawing Annotations

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Module 23 | Page 1

Exercise 1: Annotating Drawings Objectives After successfully completing this exercise, you will be able to: • Add annotations to a drawing. • Add a BOM and Balloons.

Scenario You are continuing to work on the piston and engine drawings and add the dimensional detail needed by Manufacturing. You need to add the piston dimensions that are necessary for machining. Additionally, you need to add a BOM and Balloons that label each part of the engine assembly. Close Window

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Drawing_Details\Annotating Task 1:

DRILL_COMPONENTS.DRW

Show all dimensions on the PISTON.PRT.

1. Disable all Datum Display types. 2. Select the Sheet 1 sheet tab to activate it. The active model is shown at the bottom of the graphics window. 3. Select the Annotate tab from the drawing ribbon. 4. Click Show Model Annotations from the Annotations group. 5. In the Show Model Annotations dialog box, verify that the Dimensions Tab is selected. • Select PISTON.PRT from the model tree. • Click Select All

.

in the Show Model 6. Click Clear All Annotations dialog box. 7. Leave the Show Model Annotations dialog box open for now.

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Task 2:

Show dimensions by feature.

1. Select Cut id 1963 from the model tree. in the Show Model 2. Click Select All Annotations dialog box. 3. Note that the dimensions are displayed in various views, as shown. in the Show Model 4. Click Clear All Annotations dialog box. 5. Leave the Show Model Annotations dialog box open for now.

Task 3:

Show dimensions by feature and view.

1. Show the dimensions of the ring groove so they appear only in the detail view, as shown: • Select the ring groove F16(CUT) from the detail view. in the Show Model • Click Select All Annotations dialog box. • Clear the check box for the d32 dimension. • Click Apply.

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Module 23 | Page 3

2. Select the cut feature F20(CUT) in the bottom view

3. In the Show Model Annotations dialog box, select the d40 dimension check box. • Click Apply. 4. Leave the Show Model Annotations dialog box open for now.

Task 4:

Show dimensions by view and then show all remaining dimensions.

1. Show all the dimensions in the front view, as shown in the figure: • Select the front view. in the Show Model • Click Select All Annotations dialog box. • Click Apply. • Leave the Show Model Annotations dialog box open for now. When working outside of the context of the Show Model Annotations dialog box, you can also select a view, right-click, and select Show Model Annotations when the Annotate tab is selected in the drawing ribbon.

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2. Show the remaining dimensions on the drawing: • Select PISTON.PRT from the model tree. in the Show Model • Click Select All Annotations dialog box. • Click Apply > Cancel.

3. In the detail view, select and drag the two 1.5 dimensions so they are better oriented on the drawing view, as shown. 4. Drag the handles at the ends of the witness lines to position them appropriately.

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Module 23 | Page 5

Task 5:

Create a driven dimension for the inner diameter of the piston.

1. Click Dimension from the Annotations group. • Zoom in, press CTRL, and select the edges shown in the figure. • Middle-click to place the dimension, also shown in the figure. • Middle-click again to stop placing dimensions. 2. With the 12 dimension still selected, right-click and select Properties. • Select the Display tab. • Click in the Prefix field, click Text Symbol, select Ø (diameter), and click Close > OK. • Click in an empty area of the graphics window to de-select the dimension.

Task 6:

Use various detail options to manually arrange the dimensions.

1. Select one of the 360° dimensions on the top view. • Right-click and select Delete . • Repeat for the second 360° dimension. A drawing dimension that is located beneath other dimensions can be selected by placing your cursor over the dimension, right-clicking to query, and clicking to select it. Also, use care to select the appropriate dimension as there are multiple 360°, 12, and 25 dimensions that belong to completely different features.

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2. Select the Ø8 dimension on the front view, right-click, select Move to View , and select the left cross-section view. 3. Select the Ø12 dimension on the left cross-section view and drag the dimension outside of the view. Right-click and select Flip Arrows. 4. Drag the handles at the ends of the witness lines to position them appropriately.

5. In the front view, select the 16 dimension and drag it to the left until it snaps to the 14 dimension. 6. With the 16 dimension still selected, drag the handles at the ends of the witness lines to position them appropriately.

7. Select the detail view note and move it to the right. 8. Select the upper 1.5 dimension on the detailed view and drag it below the view. Drag the handles at the ends of the witness lines to position them appropriately.

9. Select the R3 dimension from the top view and from the Edit group. select Move to View Select the bottom view. 10. With the R3 dimension still selected, right-click and select Edit Attachment. Select the bottom-right purple edge of the highlighted round in the bottom view and middle-click. 11. Move the dimension to the outside of the view. Right-click and select Flip Arrows.

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Module 23 | Page 7

12. Continue using these methods to clean the drawing, as shown in the following figure.

Task 7:

Edit dimensions to update the model.

1. Select the Review tab in the drawing ribbon. 2. Edit the dimensions of the piston ring groove in the model, as shown in the figure: • Edit the dimensions of the ring groove so that it is 2 mm wide and 1 mm deep. from the • Click Regenerate Active Model Update group to update the model and the drawing.

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3. Edit the dimensions of the piston ring groove height in the model, as shown in the following figure: • Select the d32:F16(CUT) groove height dimension. • Edit the dimension to 26.5 and click from the Quick Access toolbar Regenerate to update the model and the drawing. There are two 25 dimensions: d32 controls the height of the groove cut and d5 controls the height of the inner piston cut. To determine the correct dimension, you can pre-select the dimension. When you pre-select a dimension, a pop-up note appears, indicating which dimension you are pre-selecting. 4. Select PISTON.PRT from the model tree, right-click, and select Open . Select the revolved ring groove cut, right-click, and select Edit to view the modified dimensions.

5. Double-click each dimension, and type the original values (1.5 x 1.5 and 25). 6. Click twice in the background to de-select all geometry. 7. Click Close to return to the DRILL_COMPONENTS.DRW. Notice that the dimensions have updated automatically in the drawing. 8. Click Save

© 2014 PTC

from the Quick Access toolbar. Note that this also saves the models.

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Task 8:

Create a Bill of Materials (BOM).

1. Select the Sheet 2 sheet tab to activate it. 2. Close the model tree by clicking Show Navigator 3. Select the Table tab in the drawing ribbon.

.

4. Click Table From File from the Table group. • Select BOM_TABLE.TBL and click Open. • Place the table in the upper-left corner of the sheet. 5. Double-click the sheet scale in the lower-left corner of the sheet and type 0.8. 6. Select the view. 7. Right-click and clear the Lock View Movement 8. Drag the view, as shown in the figure.

option, if necessary.

This parametric table was created with repeat regions. Repeat regions are special table cells that contain parametric notes. Parametric notes automatically update if components are modified (assembled, deleted, renamed, or suppressed).

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Task 9:

Add BOM Balloons to the view.

1. Click Create Balloons from the Balloons group and select Create Balloons - All. 2. Click and drag the Balloons to arrange them, as shown in the figure. You can select Cleanup Balloons to organize the Balloons. You can also select a BOM Balloon, right-click, and select Edit Attachment to change the component geometry to which the BOM Balloon points.

3. Open the model tree window by clicking Show Navigator 4. Click Save

.

.


and OK to erase


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Module 23 | Page 11

Module 23 | Page 12

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Module 24 Using Layers

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Exercise 1: Creating and Managing Layers Objectives After successfully completing this exercise, you will be able to: • Create layers containing reference geometry features.

Scenario While working on the MUFFLER.PRT, you discover that you need to remove unnecessary reference geometry by creating and managing layers effectively. You need to examine the default layers in the MUFFLER.PRT, create a layer for the exhaust holes, and manually hide the axes. Close Window

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View\Layers_Muffler Task 1:

MUFFLER.PRT

Examine the default layers in the MUFFLER.PRT.

1. Enable only the following Datum Display types: 2. In the ribbon, select the View tab. 3. Enable Plane Tag Display

and Axis Tag Display

. .

4. Notice that there are a number of datum features visible in the model.

5. Review the model tree and notice that there are several hidden sketches (Sketch 1-6). These sketches were automatically hidden during the creation of features. from the Visibility group to 6. Click Layers enable it. Expand the Hidden Items layer and notice that the hidden sketches from the model tree are listed, as well as a datum plane. Select the MOUNT datum plane in the layer tree to locate it on the model.

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7. Click in the graphics window to clear the display of the MOUNT plane. 8. Expand the 01__PRT_ALL_DTM_PLN and 01__PRT_DEF_DTM_PLN layers. Notice that datums RIGHT, TOP, and FRONT are common, but the 01__PRT_ALL_DTM_PLN layer contains additional items. Also notice that the symbol for each layer is different.

9. Select the 01__PRT_DEF_DTM_PLN layer, right-click, and select Layer Properties. Notice that the Contents tab displays the three datum features. Select the Rules tab and notice that there are no rules present. Click OK. 10. Select the 01__PRT_ALL_DTM_PLN layer, right-click, and select Layer Properties. Notice that the Contents tab displays the five datum features. Select the Rules tab and notice that there are two rules present. Click OK. 11. Select the 01__PRT_DEF_DTM_PLN layer, right-click, and select Hide. Then click Repaint . Notice that the default planes are removed from the display. 12. Select the 01__PRT_ALL_DTM_PLN layer, right-click, and select Hide. Then click Repaint . Notice that all planes are now removed from the display. 13. Select Save Status from the Status types drop-down menu in the Visibility group to save this layer display configuration in the model. If you need to save the layer status when saving the model, you must manually save the status of Hidden/Shown layers to the model.

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Module 24 | Page 3

Task 2:

Create a layer for the exhaust holes.

1. In the layer tree, right-click and select New Layer. Type EXH_HOLES as the Name in the Layer Properties dialog box. Leave the dialog box open. In the top of the layer tree, click Show and select Model Tree. Select the last four holes in the model tree. Click OK in the Layer Properties dialog box. 2. In the top of the model tree, click Show and select Layer Tree. Select the EXH_HOLES layer, right-click, and select Hide. Then click Repaint . Notice that the hole axes are hidden, but the holes themselves remain.

Task 3:

Manually hide the axes.

1. In the top of the layer tree, click Show and select Model Tree. Press CTRL and select axes HOLE_1 and HOLE_2, right-click, and select Hide . Then click Repaint . The axis features are hidden, and the hole axes remain visible.

2. Click Layers to enable it. Expand the Hidden Items layer and notice that the HOLE_1 and HOLE_2 axes are contained within this layer. 3. In the layer tree, right-click and select Save Status to save this latest layer display configuration to the model. 4. Disable Plane Tag Display Display .

and Axis Tag


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© 2014 PTC

Module 28 Project II

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Module 28 | Page 1

Objective 1: Creating the FLANGE.PRT Scenario ACME Incorporated develops and markets several consumer, industrial, and defense goods. The Light Industrial Division of ACME creates a number of products, including industrial fans, heating, air conditioning, and pumps. You are employed by the Light Industrial Division of ACME Inc., which has recently started using Creo Parametric for its product designs. Upon returning from Creo Parametric training, you are assigned to create the AC-40 Air Circulator. You apply the skills learned in previous topics of this course to create the final assembly and components of the air circulator. Close Window

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Projects\Intro-2_working Task 1:

CREATE NEW

Create the flange and extrude the main body.

1. Create a new part named FLANGE.PRT. 2. Enable only the following Datum Display types: . 3. Create the extrude feature as shown. Use the mmns_part_solid template for this and all models in this project. To help verify the correct datum entities, enable datum tag display for this project.

Task 2:

Create an attachment hole.

1. Create the radial hole as shown.

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Task 3:

Pattern the flange hole.

1. Pattern six evenly-spaced holes on the flange.

Task 4:

Apply an appearance to the flange.



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Module 28 | Page 3

Objective 2: Completing the IMPELLER.PRT Task 1:

Pattern the blade and round.

1. Open IMPELLER.PRT. 2. Create an axis pattern, evenly spacing six instances of the BLADE feature. Click Set Angular Extent space the six blades.

to evenly

3. Reference pattern the BLADE_ROUND feature.

Task 2:

Apply an appearance to the impeller.

1. Apply the Silver appearance to the model. 2. Save the model and close the window.


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Objective 3: Completing the ENGINE_BLOCK.PRT Task 1:

Create the first cooling fin.

1. Open ENGINE_BLOCK.PRT. 2. Use an embedded datum and an offset loop in sketcher to extrude the fin, as shown. 3. Rename the feature as FIN.

Task 2:

Pattern the cooling fin.

1. Create a direction pattern, as shown.

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Module 28 | Page 5

2. Reorder the BORE hole feature so it removes material from the fins, as shown.

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Task 3:

Create rounds to smooth edges.

1. Create three rounds, as shown.

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Module 28 | Page 7

Task 4:

Apply an appearance and create a cross-section.

1. Apply the Silver appearance to the model. 2. Create a cross-section named A. 3. Save the model and close the window.


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Objective 4: Completing the IMPELLER_HOUSING.PRT Task 1:

Create a hole in the mounting flange.

1. Open IMPELLER_HOUSING.PRT. 2. Create the radial hole as shown.

Task 2:

Pattern the bolting flange hole.

1. Create an axis pattern, evenly spacing six instances of the hole.

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Module 28 | Page 9

Task 3:

Mirror the hole and rib features, and round the mounting flange corners.

1. Mirror both the attach hole and strengthening rib about datum plane FRONT, as shown. 2. Round the corners as shown.

3. Mirror the mounting flange, ribs, holes, and rounds about datum plane RIGHT to the front of the model as one operation.

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Task 4:

Apply an appearance to the impeller housing.



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Module 28 | Page 11

Objective 5: Completing the FRAME.PRT Task 1:

Mirror the entire frame.

1. Open FRAME.PRT. 2. Mirror the entire model node as shown.

Task 2:

Add mounting holes to the frame.

1. Create a hole, as shown. 2. Select the Move/Rotate option in the Paste Special dialog box to create the second dependent offset hole. The holes should only drill to the next surface.

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© 2014 PTC

3. Create a hole, as shown. 4. Select the Move/Rotate option in the Paste Special dialog box to create the second dependent offset hole. The holes should only drill to the next surface. When possible, reference more stable surface geometry rather than edges and vertices when creating features. This practice creates more robust models that are easier to modify.

Task 3:

Smooth the sharp corners.

1. Add one round feature to the five edges shown.

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Module 28 | Page 13

Task 4:

Apply the same holes and rounds to the other side of the frame.

1. Adjust the feature order so the holes and rounds are on both sides of the frame. 2. Apply the Gray_Dark appearance to the frame. 3. Save the model and close the window.


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Objective 6: Creating the PISTON_ASSY.ASM Assemble the piston and piston pin parts.

Task 1:

1. Create a new assembly named PISTON_ASSY. ASM. Use the mmks_asm_design template for this and all assemblies in this project. 2. Assemble the PISTON.PRT in the Default location. 3. Assemble the PISTON_PIN.PRT. 4. Assemble the pin Coincident with the hole. Assemble the FRONT datum planes of both parts Coincident as well.

Assemble the connecting rod.

Task 2:

1. Assemble the CONNECTING_ROD.PRT. 2. Assemble the hole in the CONNECTING_ ROD.PRT (the end without a lubrication hole) Coincident with the PISTON_PIN.PRT. 3. Assemble the FRONT datum planes of both parts Coincident. 4. Clear the Allow Assumptions check box and complete the component. Clearing the Allow Assumptions check box enabled you to leave the CONNECTING_ROD.PRT a Packaged component, rather than a fully constrained component, of the assembly. This is the desired design intent, as the other half of the CONNECTING_ROD.PRT is ultimately assembled to another model. 5. Drag the packaged CONNECTING_ROD.PRT to a position, as shown. 6. Save the model, close the window, and erase all models from session. The Drag Component functionality is only valid for packaged components.

This completes the objective. © 2014 PTC

Module 28 | Page 15

Objective 7: Creating the BLOWER.ASM Task 1:

Assemble the impeller housing and flange.

1. Create a new assembly named BLOWER.ASM. Use the mmks_asm_design template for this assembly. 2. Assemble the IMPELLER_HOUSING.PRT in the Default location. 3. Assemble the FLANGE.PRT as shown. 4. Save the model, close the window, and erase all models from session.


Module 28 | Page 16

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Objective 8: Creating the ENGINE.ASM and ENGINE_BLOWER.ASM Task 1:

Create the engine assembly.

1. Create a new assembly named ENGINE.ASM. Use the mmks_asm_design template for this assembly. 2. Assemble the ENGINE_BLOCK.PRT in the Default location.

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Module 28 | Page 17

Task 2:

Assemble the crankshaft and piston assembly using mechanism connections.

1. Assemble the CRANKSHAFT.PRT using a Pin connection, as shown. Depending on how you create the constraints, you may have two Coincident constraints instead of a Coincident and Oriented constraint.

Module 28 | Page 18

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2. Open the PISTON_ASSY.ASM. 3. Convert the existing CONNECTING_ROD.PRT constraints to connections. To convert the constraints to connections, you must clear the Allow Assumptions check box. 4. Return to the ENGINE.ASM and assemble the PISTON_ASSY.ASM, creating a Cylinder connection between the piston and engine block, as shown.

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Module 28 | Page 19

5. Before completing the sub-assembly placement, add a second connection set, creating a Cylinder connection between the crankshaft and connecting rod, as shown.

6. Apply the Silver_Transparent appearance to the engine block component. 7. Save the assembly and close the window.

Task 3:

Create the engine blower assembly.

1. Create a new assembly named ENGINE_ BLOWER.ASM. 2. Assemble the FRAME.PRT in the Default location. 3. Orient the assembly as shown and save a view called 3D-1.

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Task 4:

Assemble the engine assembly and impeller part.

1. Assemble the ENGINE.ASM to the frame as shown.

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Module 28 | Page 21

2. Assemble the IMPELLER.PRT to the crankshaft as shown.

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3. Drag the impeller to observe the related assembly motion.

Task 5:

Assemble the blower assembly.

1. Assemble the BLOWER.ASM to the frame as shown. 2. Save the model and close the window.


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Module 28 | Page 23

Objective 9: Assembling the BOLT.PRT Task 1:

Assemble the bolts.

1. Open ENGINE_BLOWER.ASM. 2. Assemble one BOLT_12.PRT model to the engine block as shown. 3. Press CTRL+C and CTRL+V to copy and paste the BOLT_12.PRT into the three other engine block holes shown. When using copy and paste functionality, the system retains information regarding the component references.

4. Assemble four BOLT_8.PRT models to the impeller housing as shown.

5. Assemble and pattern a BOLT_5.PRT model as shown. 6. Save the model and close the window.


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Objective 10: Creating the ENGINE-BLOWER_MODELS. DRW Task 1:

Create a drawing of the engine blower models.

1. Create a new drawing named ENGINEBLOWER_MODELS. 2. Reference the ENGINE_BLOCK.PRT model and the drawing template named drawing_template.drw. 3. Type your name at the prompt. 4. Edit the drawing scale of this sheet to 1.75. Creo Parametric automatically creates three standard views based on the default drawing template. This drawing template also includes a drawing format. 5. Edit the right view to be a 2-D cross-sectional view named A. 6. Display cross-section arrows in the front view.

7. Insert a shaded general view in the upper-right corner of the sheet. Use the default orientation and a custom view scale of 2.

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Module 28 | Page 25

8. Insert a detailed view of the first few fins. 9. Adjust the hatching as shown. When creating the detail view, the prompts in the Message Log guide you through the process in steps.

Task 2:

Add a second model on a new sheet.

1. Modify the drawing properties so that it references a second model, the CRANKSHAFT.PRT. 2. Insert a new sheet and type your name at the prompt. 3. Insert a general view in the lower center of the sheet. Orient the view to the LEFT model view. 4. Edit the display of the general view to Hidden. 5. Modify the drawing scale of this sheet to be 2.5. 6. Insert projected views on each side of the first view. 7. Unhide datum plane DTM1. 8. Insert an auxiliary view and select DTM1 in the far right projected view as the reference. 9. Rename the drawing view to A. 10. Add arrows, as shown.

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11. Insert a view in the upper-right corner of the sheet as shown. 12. Orient the view to the 3D model view. 13. Set the view scale to 3.

Task 3:

Show dimensions in the drawing.

1. Show and position dimensions, as shown. 2. This drawing is utilized later in the project. Save the drawing and close the window.


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Module 28 | Page 27

Objective 11: Analyzing and Resolving Interferences Task 1:

Analyze static interferences in the engine blower assembly.

1. Open ENGINE_BLOWER.ASM. 2. Drag a blade on the impeller until the position of the piston is approximately at its highest location.

3. Perform a Global Interference check on the assembly. 4. Identify the areas of interference between the frame and impeller components.

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Task 2:

Resolve the interference between the frame and impeller components.

1. Remove material from the frame, as shown. 2. Run the interference check again to verify that the frame no longer interferes with the impeller components.

Task 3:

Check for collision detection on the moving parts.

1. Enable Collision Detection. 2. Drag a blade on the impeller. As the components proceed through their motions, check for component collisions. 3. Investigate the collision between the connecting rod and engine block.

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Module 28 | Page 29

Task 4:

Implement modifications to eliminate the interference.

1. Open the ENGINE.ASM and activate the ENGINE_BLOCK.PRT. 2. Create an extrude feature to remove a circular section of material, as shown.

3. Create a round feature on both edges, as shown. 4. Save the model and close the window.

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5. Open the ENGINE-BLOWER_MODELS.DRW. 6. Edit the 8.5 dimension on sheet 2 to 8, as shown. Update and save the model, close the window, and return to the ENGINE_BLOWER.ASM.

7. Verify that the modifications you made have removed the interference. 8. Save the model and close the window. This completes the objective.

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Module 28 | Page 1

TRN-4501-400-01_SG-Ins_Exc_EN.pdf

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