Part Modeling > Sketcher > References > To Create References
To Create References
You can create references to dimension and constrain geometry when using a sketch tool or through the References dialog box. When using a sketch tool, select a tool and press ALT. Select one or more valid geometric entities to use as references.
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Adding references when pressing the ALT button is available when the Automatic reference creation from selected background geometry check box is selected in the Sketcher area of the Creo Parametric Options dialog box or when the sketcher_auto_create_references configuration option is set to yes.
1. To use the References dialog box, click Sketch > References. The References dialog box opens.
2. Select the type or reference to create:
◦ —Projects the selected geometry onto the sketching plane.
◦ —Intersects the selected geometry with the sketching plane.
3. Click and select one or more valid geometric entities to use as references.
4. Use any of the following additional commands:
◦ —Replaces a selected reference.
◦ —Updates a failed reference. This option is only available when there are unresolved references in the sketch.
◦ —Deletes selected references.
◦ —Filters and highlights the types of references available for selection.
▪ None—No references are highlighted.
▪ Project/Offset/Thicken—References for Project, Offset, and Thicken tools are highlighted.
▪ Unused as References—Unused references are highlighted.
▪ All References—All references are highlighted.
◦ Sketch Status displays the status of the sketch.
◦ —Updates the sketch when there are no missing or failed references.
5. Click Close.
About References
To Replace a Reference