Use planes from assembly in parts as reference

[Anonymous]

Hello everyone,

With more than 10 years experience in SolidWorks I recently started with Inventor2020 since I switched jobs.

In SolidWorks I often made references with planes and points/construction lines in an (sub)assembly to control dimensions and positions of parts inside the assembly. In Inventor I wanted to do the same thing, but don't seem to make it a succes. Inside the assembly I can make planes and axis that define the eventual product. But on part-level I cannot refer to the planes and axis.

How can I make the references possible? Or what is the 'official' method to make this work?

[mdavis22569]

If you want to something in the part level from the Assembly you'll like need to Project it ( project geometry for the plane - axis) and use it that way. It would be adaptive

[Anonymous]

But for example when I transfer an assembly plane into a part with Project Geometry, and afterwards change the dimension that defines that plane (in case of an offset from another plane), how can I get the projection to move in the part? 

Because that doesn't seem to happen right now. I want to keep the link between the planes in assembly and projections in parts, so that I can control the dimension in the assembly and not in the different parts.

[johnsonshiue]

Hi! The cross projection is a bit cumbersome here. You will need to edit the part and create an offset workplane based on the assembly workplane. Then you can project the adaptive workplane to a sketch.

Many thanks!

[Anonymous]

That seems a bit cumbersome indeed, but if it works.. 🙂

I do run into a problem: when editing the part in the assembly to make an offset plane, I cannot select the plane in the assembly I want as a reference. The plane in the assembly is visible, but I cannot select it. 

(In SolidWorks this occurs when External References are prohibited, but I cannot find a similar function in Inventor?)

[johnsonshiue]

Hi! This is a case of memory corruption and multi-threading error on my part. I am sorry that I described the behavior incorrectly. To get the adaptive workplane in the part, you need to create a sketch on the assembly plane while you edit the part in place. Could you try it and see if it works?

Many thanks!

[Anonymous]

When editing the part, I can make a sketch on an assembly plane indeed. With that sketch I can make a plane in the part (or subassembly), which has same geometry as the assembly plane. 

This seems to work but in my view it is too cumbersome, isn't there a more simple method?

For my understanding: If I select "Adaptive" on a plane of sketch, this meens this feature will follow the mother reference? For instance, when sketching in a part on a plane in assembly, if I move the plane in assembly, the sketch moves with it? Let's say, the plane is on 400mm offset from center point, so the sketch is 400mm away from center point. If I edit the offset from 400 to 500, the sketch should move also to 500mm?

[johnsonshiue]

Hi! Indeed, this workflow is cumbersome to say the least. It should work but it has not been implemented. I think it has something to do with Adaptive support. Adaptivity is mainly between two parts. So if you project a workplane from one part to another within the assembly, it will be adaptively associative. Such relationship does not exist between an assembly work plane and the part sketch.

Another alternative is to create a part and a part workplane instead of an assembly workplane.

Many thanks!