Create and Place Models using Skeleton References for Creo 5, 6, 7, 8

Summary

In Creo Parametric, once you have copied references from the skeleton part, you can begin to create solid geometry utilizing the copied references. You can also redefine unplaced components. You can select either the newly created solid geometry or copied geometry to define placement using constraints or connections. Using the skeleton references, you can create features in less time than it would take for you to first imagine the references, then create those in the model, and then create features using those references.

While creating models, you can either open the component in its own window or activate the component and model in the context of the assembly. You can use the copied references such as surfaces, planes, axes, and so on by referencing them when creating sketches, solid features, and other datum features in the model or when placing the model. Once you have referenced the copied geometry in the creation of model features, edits to the skeleton propagate to the model.

Видео урок.

Tutorial Tasks

TASK 1

Reference copied features to create features in the block part.

1. Click?File > Options.
2. In the Creo Parametric Options dialog box, select the?Configuration Editor?category.
3. Click?Add.
4. In the Option name field, type?multiple_skeletons_allowed, edit the Option value to?yes, and click?OK.

Note

The multiple_skeletons_allowed configuration file option determines whether multiple skeletons can be created.

1. Click?OK?and click?No?to confirm that the configuration edits made are applied to the current session only.

Note

If the Yes option is selected, the settings are saved to a configuration file and loaded during the next session.

1. Click?Open?from the Quick Access toolbar and double-click AC40.ASM.
2. Enable?Axis Display?and?Plane Display.
3. In the model tree, expand the ENGINE.ASM node and open BLOCK.PRT.
4. Select the?View?tab.
5. Click the Appearances drop-down menu from the Appearance group.
6. Select?Clear All Appearances?from the Clear Appearance types drop-down menu.
7. Click?Yes?in the Confirm dialog box.
8. Select the?Model?tab.
9. Select the?Extern Copy Geom?feature from the model tree.
10. Click?Thicken?from the Editing group.
11. Edit the thickness to?2?and press ENTER.
12. Click?OK?from the dashboard.
13. Select datum plane TOP and click?Extrude?from the mini toolbar.
14. Click?Project?from the Sketching group.
15. Click?Loop?in the Type dialog box.
16. Select the datum curve on the right side of the model.
17. Click?OK.
18. Edit the depth to?4?and press ENTER.
19. Click?OK.
20. Disable?Plane Display.
21. Click?Hole?from the Engineering group and select axis HOLE1.
22. Press CTRL and select the hole's placement surface, as shown in the figure.
23. Edit the diameter to?3?and select?Through All?as the depth.
24. Click?OK.
25. With the hole still selected, press CTRL+C and then CTRL+V.
26. Select axis HOLE2, press CTRL, and select the hole's placement surface, as shown in the figure.
27. Click?OK.
28. Hide the?Extern Copy Geom feature.
29. Click?Close?from the Quick Access toolbar.

TASK 2

Reference copied features to create features in the block part.

1. Open CRANK.PRT from the model tree.
2. Select the?View?tab.
3. Click the Appearances drop-down menu from the Appearance group.
4. Select?Clear All Appearances?from the Appearance Gallery types drop-down menu.
5. Click?Yes?in the Confirm dialog box.
6. Select the?Model?tab.
7. Select the?Extern Copy Geom?feature from the model tree and then click?Solidify?from the Editing group.
8. Click?OK.
9. Click?Extrude?and select the rear cylinder surface.
10. Click?Project?and select?Loop.
11. Select the datum curve and click?OK.
12. Flip the feature direction towards you and drag the depth to?6.
13. Click?OK.
14. Click?Extrude?and select the rear surface.
15. In the graphics window, press ALT and select datum axis PIN_1.
16. Right-click and select?Add references.
17. Sketch a circle with a diameter of?5?centered on PIN_1.
18. Click?OK.
19. Edit the depth to?6?and click?OK.
20. Hide the?Extern Copy Geom?feature.
21. Click?Close.
22. Edit the definition of CRANK.PRT.
23. Click?OK.

Note

You could use placement constraints at this time to properly place the component.

TASK 3

Clean up the display and assemble bolts.

1. Hide MAIN_SKEL.PRT and CRANK_SKEL.PRT.
2. Select BLOCK.PRT.
3. Click the Model Display group drop-down menu and select?Component Display Style > Transparent.
4. Edit the definition of BOLT_8.PRT.
5. Click?Show In Assembly?Window from the dashboard.
6. Constrain the bolt as shown in the figure and then click?Complete Component.
7. Disable?Axis Display.
8. Select BOLT_8.PRT, press CTRL+C and then CTRL+V.
9. Constrain the bolt into the last hole as shown in the figure and then click?Complete Component.