We try to create every purchased product as a part, as we dont have/want to handle the components in our product structure. This is an autoimposed rule, but I would like to mantain it. I think it shouldnt be difficult to create a deformable part that follows an external plane but I am not very familiar with this kind of deformable parts.
I haven't looked at your file, but this is how I do it.
Use a distance constraint between your planes / components, this will create an expression (you will see it in the expression editor)
Now make the Deformed length of you deformable component = the distance constraint expression.
When and what error do you get?
If I understood your question correctly - You want change final geometry according to Datum Plane(4), follow below steps:
1. Hit Ctrl + T to invoke "Move Object" dialog.
2. Select Datum Plane(4).
3. Drag ZC handle as you want to change distance.
4. OK. You'll find final geometry is being changed as per Datum Plane.
Similar to @joewhite's solution, try to create your deformable part using an Offset Datum, rather than a fixed datum that is used to define the length (see attached). You can then use a Measure feature, or a Distance Positioning Constraint to define the offset distance of the Datum in the deformable part.
I was able to get your version to work by WAVE linking a face from the spindle component (called screw in this assembly) and using that linked face for the reference in your deformable part.
Thank you very much.
I like the method of creating the deformable based on a parameter and then as deforming the part in the assembly use expresion to relate the parameter to the measure. In fact, I think I will use this method for other projects too.
Just I find a problem with the orientation because the pattern of figures is created in the opposite direction when I insert in the assembly, like it is saved in the assembly attached.
When the deformable part is 'deformed' its features are recreated in the destination part. I wonder if the vectors that were used when creating the deformable part (Sketch axis, Extrude direction vectors, Pattern direction vector) were based on the coordinate system rather than physical, child features. Hence, when the part is deformed it uses the coordinate system of the destination part, rather than the child features that belong to the part being deformed.
I tried to make the features based on physical instead of coordinate systems, that is something you teached me some time ago. The revolve features work properly in the assembly when deforming part, the only problem is with the pattern, but I cant find what mistake I am doing. I tried to rebuilt the pattern but without success.
I created a simple part and I'm seeing similar results. Please open an incident report with GTAC and have them submit a problem report to development (mention internal PR 9177683).