BD1 WildFire

INTRODUCTION TO Pro/DETAIL Pro/ENGINEER Wildfire™

Subject: Pro/DETAIL Lesson # 1 Topics: • • • •

Drawing Mode vs. Pro/Detail Creating a Drawing Adding Views Modifying Views

FroTime Tutorials – Copyright 2003 – Do Not Duplicate Find More FroTime Tutorials at www.frotime.com BD1_Wildfire_01

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Tutorial Guidelines

How to Read This Tutorial Below is a quick outline of how to read this tutorial. Underneath each item is an example of how it might be used throughout the document. All menu picks in Wildfire are designated by #this text. • Part menu: #Feature, #Create, #Datum, #Plane, #Default. Explanation or comments about what you’re doing are noted by this text ** To begin, we will create a new part with default datum planes ** Any file selection is noted by • File menu: #Open, Name: , #OK. Any input into Wildfire will be displayed with [this text]. • File menu: #New, Name: [surf_1], #OK.

Disclaimer and Terms of Use All material written in this document has been thoroughly reviewed for accuracy and tested for the release designated on the title page. However, FroTime is not responsible for any information that is incorrect or does not operate correctly when the tutorial instructions are followed. Pro/ENGINEER, Wildfireand the related modules discussed within this tutorial, as well as all screen captures, are registered trademarks of PTC. For more information, please consult their web site at www.ptc.com


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Table of Contents I.

Introduction – Drawing Mode Vs. Pro/DETAIL.................... 4

II.

Tutorial Lesson – Creating a Drawing........................................ 5

III.

Tutorial Lesson – Creating a View .............................................. 9

IV.

Tutorial Lesson – Modifying Views........................................... 15

V.

Summary ...................................................................................... 19


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I. Introduction – Drawing Mode Vs. Pro/DETAIL Drawing mode provides you with the ability to document your parts and assemblies created using Pro/E in drawings that share a two-way associativity with the model. When you modify a part or assembly in Pro/E the drawing is automatically updated and reflects the changes. When you make changes to your part or assembly in the drawing, those changes will be reflected in the models. You can use basic Pro/ENGINEER to create drawing views of one or more models in several standard view types and dimension them. You can also annotate the drawing with notes, manipulate the dimensions, and use layers to manage the display of different items. Pro/DETAIL is an optional add-on module for Pro/E. It extends the drawing mode capability allowing you to create additional view types as well as the ability to use multiple sheets. Pro/DETAIL includes numerous commands for manipulating items in a drawing, and enables you to add and modify different kinds of textual and symbolic information. You can use Pro/DETAIL to customize drawings by utilizing sketched geometry, creating custom drawing formats with company logos. This tutorial, as well as the rest of the tutorials in the FroTime Detailing series, will assume that you have the Pro/DETAIL module.


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II. Tutorial Lesson – Creating a Drawing ** Bring the part named “fan_housing” into session ** •

FILE menu: #File, #Open, Name: , #Open

** We will now create a “C” size drawing for this part. ** •

FILE menu: #File, #New


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** The NEW dialog box appears. Select “Drawing” from the “Type” box and then add the name”FAN_HOUSING”. New for 2000i2 is the “Use default template” check box. This allows you to use a default template for your drawing that already has default views defined. For this lesson we will create our own views. Uncheck the “Use default template” check box. **


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** Make sure that the model “fan_housing” is showing in the “Default Model” box. Under the “Specify Template” box select”Empty” (You can also select “Empty with format” to select your own format or “Use Template” to use a default template.) Select “Landscape” in the “Orientation” box. Inside the “Size” box select “C” for the Standard Size. Select OK. **


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** A blank “C” size format should now be on your screen. **

** Note that the model “fan_housing” is associated to the drawing. This can be verified by looking at the bottom of the graphics window. **


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III. Tutorial Lesson – Creating a View ** Create a front view of the fan_housing part. ** • •

Insert menu: #Drawing View… VIEW TYPE menu: #General, #Full View, #No Xsec, #No Scale, #Done

** You are now prompted to select a CENTER POINT for the drawing view. ** ** Select the center of the “C” size blank format. The default view of the fan_housing appears and the “Orientation” box shows up in the upper right. **


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** There are two ways to orient the view in order to be a “front” view. With the “Type” box set to “Orient by Reference”, you could go ahead and select the “MID_CENTER” datum plane on the fan_housing part as the Reference 1 Front plane and then select the “HORZ_CENTER” plane on the fan_housing part as the Reference 2 Top plane. This would generate a “front” view. The second way is to simply select on the “Saved Views” menu and pick “FRONT” from the list of saved views and then “SET”. This view was created in part mode. Both methods should produce the same result as shown below. The second method is preferred since it takes advantage of the views that have already been created. **


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** Now create top, bottom and right side projection views off of the front view just created. ** • •

Insert menu: #Drawing View… VIEW TYPE menu: #Projection, #Full View, #No Xsec, #No Scale, #Done

** Again you are prompted to pick a CENTER POINT for the view. **

** Select a location above the “front” view you created in the previous step. The view will automatically be created in the proper orientation as a projection off the “front” view. **


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** Repeat this process for the bottom and the right side views. When completed, your drawing should look like the following image. **


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** Finally, create an isometric view in the upper right corner of the format. Use “General” from the view type menu and then select “FRONT_ISO” form the “Saved Views” menu in the “Orientation” Box. Pick “Set” and then “OK”. **

•

• DRAWING menu: #Drawing View… VIEW TYPE menu: #General, #Full View, #No Xsec, #No Scale, #Done


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** Your drawing should now look like the image below. **


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IV. Tutorial Lesson – Modifying Views ** Move the front view of the fan_housing to the left side of the format. ** •

Screen: select the Front view, right click, uncheck Lock View Movement

•

Screen: The move cursor should now show when you have the Front view selected, click on the view to drag it to the left of the screen.

** All the drawing views become highlighted with a red boarder around them. Select the front view and then pick the new location on the left side of the format. Notice that the two projection views (top, bottom) move along with the front view. These projection views are children of the parent front view. Projection views can only move along one axis of the parent view. Verify this by moving the right side projection view to the left side of the format. **

** Your drawing should now look like the following image. **


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** Next, change the orientation of the isometric view in the upper right side of the drawing format form a FRONT_ISO to a REAR_ISO. ** • •

Screen: select ISO view, right click #Properties VIEW MODIFY menu: #Reorient

** Select the isometric view in the upper right side of the drawing. The “Orientation” box appears. Select “REAR_ISO” from the “Saved Views” menu. Pick “Set” and then “OK”. **


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** Now that the views are all positioned and oriented correctly, you need to set the view display. This is different form setting it in the environment pull-down menu because this will only change the view display in the current secession of Pro/E. If someone else were to work on the drawing his or her settings may be different from yours and confusion could set in. In order to prevent this the view display must be set specific to the drawing so that no matter who works on the drawing the same display will be shown. ** • • •

Screen: hold Ctrl key, select front, top, bottom and right view Screen: right click, #Properties VIEW MODIFY menu: #View Disp

** These views will be set to display no hidden lines and no tangent edges ** •

VIEW DISP menu: #No Hidden, #No Qlt HLR, #No Disp Tan, #Hide Skeleton, #Done

** Select the rear isometric view. This view will be set to display hidden lines and no tangent edges ** • • • •

Screen: select ISO view Screen: right click, #Properties VIEW MODIFY menu: #View Disp VIEW DISP menu: #Hidden Line, #No Qlt HLR, #No Disp Tan, #Hide Skeleton, #Done

** Your drawing should now look like the image below. **


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** As an added exercise you can make additional drawings using the default template functionality as well as your own formats. **


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V. Summary After completing the above tutorial, you should be able to do the following: • • •

Create a drawing related to a part or an assembly created in Pro/E. Add views to the drawing (general views, projection views) Modify the views you created (move view, reorient the view, set view displays)

This was a basic introduction to the Pro/DETAIL module of how to generate a drawing in Pro/ENGINEER This concludes the 1st Frotime detailing tutorial. To continue your detailing training please obtain the 2nd Tutorial in the Frotime detailing series at www.frotime.com!


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NOTES


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NOTES


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BD1 WildFire

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