Model Analysis > Model Analysis > Creo Behavioral Modeling Tools > Analyses > PTC Mathcad Analysis and PTC Mathcad Analysis Feature > Example: Driving an Angular Dimension Using a PTC Mathcad Generated Parameter
Example: Driving an Angular Dimension Using a PTC Mathcad Generated Parameter
Summary: This example shows you how to drive angular dimensions using PTC Mathcad generated parameter.
Problem: Need to drive a Creo Parametric angular dimension, d37, with the PTC Mathcad analysis generated parameter MC_Y.
Solution: Create a PTC Mathcad analysis feature and define a unit-sensitive relation.
The following basic steps outline this example:
1. In PTC Mathcad, load an existing PTC Mathcad file with a .xmcd extension.
2. In the Math region, select a PTC Mathcad results variable, y=0.52 rad.
3. Click Format > Properties. The Properties dialog box opens.
4. Click the Display tab and edit the tag information for the variable.
5. In the Tag box, enter the value mc2proe and click OK.
6. Click File > Save to save the PTC Mathcad file with a .xmcd extension.
7. In Creo Parametric, open the model and click Analysis > Analysis. The ANALYSIS dialog box opens.
8. Under Name, enter a name for the analysis, for example, ANALYSIS1or accept the default name.
9. Under Type, click Mathcad Analysis.
10. Click Next. The Mathcad Analysis dialog box opens.
11. Click Load File under File and select a file with a .xmcd extension.
12. After loading the PTC Mathcad file, define the analysis as required.
13. Click Outputs under Mathcad to PTC Creo Parametric to select the PTC Mathcad results variable y to compute from the Outputs Selection dialog box.
14. Click OK to continue. The selected PTC Mathcad results variable y appears in the Outputs box in the Mathcad Analysis dialog box.
15. Click Compute to run the analysis.
16. Click Close to return to the ANALYSIS dialog box. The Result params window opens. All PTC Mathcad results variables selected for the output settings appear in the Result params table. The table lists the status, name, and description of each parameter.
17. To create a parameter, select it from the Result params table and click YES under Create.
18. Click to create the Analysis feature.
19. To create a relation, click Tools > Relations. The Relations dialog box opens.
20. Under Look in, select the Feature object type to apply the relation.
21. Select the ANALYSIS1 feature on the Model Tree to create a relation.
22. Under Relation, type the unit-sensitive relation d37=MC_Y:FID*180/pi and press ENTER. This relation shows that Creo Parametric dimension d37 driven by PTC Mathcad analysis generated parameter MC_Y.
23. Click Utilities > Verify to validate the relations you have entered.