Define Graphic Representations for a Part

This task shows you how to create multiple graphic representations for a part. See also Switching Graphic Representations.
Once you have created a  part and specified a type, you can create one or more graphic representations, i.e., create the body of the part. You can define multiple graphic representations when you need to show more than one graphic of the same component. For instance, you may need to show a pipe as "double", which is like a 3D version, as "single", which means represented by a single line, or "envelope", which also includes the working area needed around the pipe or equipment. These three categories are defined in this application. A fourth category is also included, "exact", which is normally used for detailed representation. You can create these three graphics of the same pipe and place whichever one you prefer in a document.

Before you create multiple representations you should set up a Graphic Representations file. (You do this by creating a file - a default is provided if you want to use it - and noting its location in your resource management file. See Understanding Project Resource Management.) A Graphic Representations file allows you to classify each graphic that you create into a specific category. In addition to the four categories that are defined in the application and that were described above, you can create categories based on your specific needs.

NOTE: If you are creating a part as a light object you do not need to create additional representations. The application will be able to generate double and single representations for the part. You can, however, change the wording 'double' and 'single' in the text file.

1. When you create a part as explained in Create a Part with specified type, it is given the first classification listed in your Graphic Representations file. In this example it is Double as shown in the illustration below. To start making graphic representations for the part, you will first create a graphic for the Double representation that you have already created. To do this double click on Elbow1 to bring up the Part Design product. (Not all users may have a license for Part Design - contact your system administrator.)


2. Create your part (in this case an elbow) using Part Design. (See Part Design documentation if you need help.) You have now created the Double graphic representation of the part. 

3. To create a second graphic representation, double click on CONDUIT_ELBOW_1(Conduit-Part01) to return to Conduit Design.
4. Click on the Build Conduit Part button to display the Create Part dialog box and click on the elbow to make it active. The buttons in the Create Part dialog box will become active.
5. Click on the Manage Representations button . The Manage Graphic Representations dialog box will display.

If you are creating a light part then you will not have a graphic for it. Create a light part, or open a typed part, and click the Manage Graphics Representations button. The following dialog box displays.

Click on the down arrow to select a name for each of the two representations. You can also select the default representation that you want displayed.

6. The Defined column shows which representations exist for the part. If a name has No against it you can create a representation by clicking on No. It will change to Yes and the graphic name will be added to the specifications tree. You now need to create a body for it, as described above.  In the illustration below you can see both double and single representations. The single representation is the white line running through the 3D elbow.

7. If the value for a graphic in the Activated column is Yes it means you can see that graphic. (You can toggle between Yes and No by clicking on it.) If you check the box Expand representations you will see all representations of the part that have been defined.