For sketches, Perimeter dimension can be used to constraint total length of selected lines and/or arcs.
Note: Perimeter constrained dimension can not be created for Ellipses, Conics or Splines.
NX – Create Perimeter Dimension
In a active sketch
Home tab > Rapid Dimension drop down > Perimeter Dimension or
Menu > Insert > Sketch Constraint > Dimension > PerimeterSiemens NX CAD – Sketching Tips – Perimeter Dimension Dialog
Select the required curves (lines/arcs) to create perimeter dimension.
Note that, Perimeter dimension will not be displayed in the graphics window but it will created as a expression. Go the expressions (Ctrl+E), notice the generated expression. It will look like “perimeter_p01” as shown.
If you try to create perimeter dimension for the curves for which it is already created then NX will show error dialog with the message that constraint already exists.
NX – Edit Perimeter Dimension
You can edit perimeter dimension value in the following ways.
- Go to expression (Ctrl+E or Menu > Tools > Expression) and edit the value of perimeter expression.
- When sketch is inactive, From part navigator select sketch > RMB > Edit Parameters. In ‘Edit Sketch Dimensions’ dialog, select the perimeter dimension and edit it’s value.
- Edit Sketch, From part navigator select sketch > RMB > Edit Parameters. In ‘Sketch Parameters’ dialog, select the perimeter dimension and edit it’s value.
NX – Delete Perimeter Dimension
Perimeter expression can not be deleted directly from expressions dialog.
To delete it, Edit the sketch and from part navigator select sketch > RMB > Edit Parameters. In ‘Sketch Parameters’ dialog, select the perimeter dimension and click on delete icon.
Note: If one or more curves are deleted that are used to create perimeter dimension then the perimeter dimension is also deleted.