Step 2: Specify Shrinkage

In this section, we will show how to apply shrinkage to a RefPart.

There are two methods to apply the shrinkage:

A method that scales the complete model
A method to define each dimension one by one.

We will apply a 2% shrinkage by scaleto the RefPart in all directions:

"By Scale" means that the overall model will be scaled.
We use here the "1+S" formula to expand the overall model by 2%
- 1+S : if S is 0.02 (2%), the overall model size is multiplied by (1+0.02), so, modelsize = oldsize * 1.02... the model is ENLARGED by 2%.
- 1/(1+S) : in this case, with the same values, we would have the new modelsize = oldsize / 1.02... the model would be REDUCED by 2%.
Coordinate System: it is recommended to select a RefPart Coordinate System (we select here the CSYS named "CS0").
- You may select the Assembly CSYS; it works, but in that case, you will receive a warning message: "Selecting External CSYS here may lead to circular references"
- IMPORTANT: the overall scale will be calculated from this CSYS as the origin of the scale deformation.
Isotropic: the model is scaled by 2% in all directions. If you unchecked this box, you will have the opportunity to define a different scale on each direction.
Forward References: Shrinkage does not create new geometry but changes the existing geometry so that all existing references continue to be a part of the model; If you clear the Forward References check box, Pro/ENGINEER creates new geometry for the part on which you are applying shrinkage.

Validate the feature: a new feature is added at the RefPart level: if you were using the original model rather than an associative copy (see page before) this step would mark the original model as modified!

You may measure the inside hole diameter: this hole was created at a diameter of 10 mm; the measure will report 10.2 mm.

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