Part Modeling > Creo Flexible Modeling > Moving Geometry > To Move Geometry Using Constraints
To Move Geometry Using Constraints
1. Select geometry to move.
2. Click Flexible Modeling > Move > Constraints. The Move tab opens. The Automatic constraint is selected by default.
3. Select references for fixed geometry and moving geometry.
4. Use the dragger to place the geometry in the approximate position. Drag a handle to translate geometry, drag an arc to rotate geometry.
5. Type an offset value for the constraint.
6. Click to change the direction of the offset.
7. To move the selected rounds and chamfers that attach the moved geometry to the model, click the References tab and check the Transform selected attachment rounds/chamfers check box. If you do not check this check box, the selected attaching rounds and chamfers are removed and optionally recreated.
8. To set additional attachment and propagation options, right-click and use the shortcut menu or use the Attachment and Options tabs.
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When the Attach moved geometry check box is not selected, the resulting geometry is a quilt. The appearance of the original solid surfaces is propagated to both sides of the resulting quilt.
9. To maintain tangency between the moved geometry and neighboring geometry:
a. Click Keep Tangency.
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If the flex_tan_propagation_default configuration option is set to on, tangency is automatically propagated.
b. If needed, set conditions for neighboring geometric entities using the Conditions tab, the Add condition option, or the shortcut menu.
10. To create a copy-move feature, click Create a Copy.
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When the selected geometry is an open quilt, and you select Create a Copy, clear the Attach moved geometry check box on the Attachment tab.
11. To navigate through other possible solutions for geometry configurations, on the Attachment tab, click Next or Previous.
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When you click Next, the system might stop responding while it tries to find the best possible solution. This is because it checks for all possible combinations for the solution. The system might also stop responding if a solution does not exist.
At this point, to interrupt the check and continue working:
1. While the model is regenerating, click Stop at the bottom of the window to interrupt the regeneration. A failed feature is created.
2. In the Model Tree, click the failed feature and select Edit Definition. Even if you do not make any changes in the settings, this gives you the opportunity to check if the result is what you want.
3. Click OK. The feature regenerates.
When the system is unable to find more than one solution, the Previous and Next options are not available.
You can select a different solution when you redefine the Move feature.
12. Click OK or middle-click to accept the feature.