Inventor Pattern Work Planes In Assembly By Formula or iLogic?

[Des_Seals]

I know you can offset work planes but is there a way to create a pattern of work planes? Or any other way to generate a number of work planes thats controlled by a formula

kelly.young has edited your subject line for clarity: Is there a way to pattern work planes

[philip1009]

Yes it's possible, open your Parameters window and create the necessary User Parameters that control the Qty and Offset, keep in mind that you have to make sure that the end result of Qty unit type has to be "ul" or Unitless number instead of a distance number as Inventor is specific about that.  Then when you make the pattern instead of putting numbers in the Qty and Offset spaces, type in the name of the appropriate Parameters.  I've attached a sample below.

[hncarle]

No need to get fancy. You can do exactly the same with planes as with any other feature. Circular pattern, Rectangular pattern.  Don't think you could find a useful result from doing a rectangular pattern going in TWO directions though.

Take a look at this thing that our good friend at Neil at TFI did.  https://www.youtube.com/watch?v=aq8rRc9H_TI

I did the exact thing using circular pattern. 

[Des_Seals]

That works on parts but I forgot to mention Im trying to do it in an assembly. When I try the same thing in an assembly it doesnt let me select the work plane.

[philip1009]

Sorry, I forgot to double check in assemblies, patterns only work on occurrences for some reason, maybe there's an idea in the Inventor Ideas forum to vote for.  What's your end goal for this workflow, maybe there's a better method we could come up with?

[Jon.Dean]

Hi @Des_Seals, Following on from @philip1009 suggestion. Take a look at my screencast explaining the process Philip described.

Cheers Jon.

[Jon.Dean · Accepted solution]

Hi @Des_Seals, So, you want to pattern inside an assembly. You are correct this is not possible, you will get an error.

Cheers

Jon

[Des_Seals]

@philip1009 wrote:

Sorry, I forgot to double check in assemblies, patterns only work on occurrences for some reason, maybe there's an idea in the Inventor Ideas forum to vote for.  What's your end goal for this workflow, maybe there's a better method we could come up with?

---

I already have another solution, I was just trying work planes and I was a little surprised it didnt work in the assembly. Thanks for the help though. Ill check the Inventor Ideas section for it

[philip1009]

The closest you can get is to have the equations on an assembly level and then use a little iLogic rule to synchronize the pattern inside of the part, I've attached a sample.  The part is marked as reference, so it won't appear in any BOMs.

[Tom_Sturtevant]

One possible workaround for an Assembly Workfeature pattern is:

* Create a part with a single visible work plane

* Place and constrain in the assembly

* Pattern the component

 

Regards,

T.0.M.