How to create deformable seals in Siemens NX?

In this tutorial the modeling of deformable seal will be shown. To see how its work here you can find a video presentation:

  1. Step 1:

    Create your slot for the seal. If you use sweep feature for the slot make the guide curve visible. If you have not guide curve, create it.

  2. Step 2:

    Create the seal, open a new model file. For the guide curve, navigate to the Curve ribbon bar and select Arc. Create a full circle, with the required radius.

  3. Step 3:

    For the section curve, create a new sketch. Select On Path option for the plane, select the previously created arc for the path. Create an ellipse as section, give the minor and major radius (note if the seal is undeformed minor=major radius).

  4. Step 4:

    Create a Sweep Along Guide feature. The guide will be the Arc, the section will be the Ellipse.

  5. Step 5:

    Select the Define Deformable Part from the Tools menu. On the wizard define the name of the deformable part. Select the Arc and Sketch features.

  6. Step 6:

    Select the minor and major radius for the variable paramaters. Set the expression rules as you require. If all the parameters are set, click on the Finish button.

  7. Step 7:

    If you work in an assembly add your component, set the slot guide visible. Select WAVE Geometry Linker and link the guide.

  8. Step 8:

    Add your seal model to the assembly. Set the minor and major radius n the deformable component window. The sketch path and the guide of the sweep is the previously linked curve (select this curve to resolve the missing reference). Click on the OK button, and here is your deformed seal!