Selected Faces Do Not Form a Patternable Object

[neljoshua]

I am working on modeling a heat exchanger plate.  I need it to be as close to the real thing as possible.  In any event, the plate is symmetrical and held together with spot welds.  In order to model the spot welds I created a revolute feature (I am planning to shell the part later).  Fusion, however, does not like the pattern and keeps giving the error message shown below.  I cannot simplify the pattern by excluding faces, as there are only two faces in the pattern.

Would someone be able to help me with this?  Here is the design: http://a360.co/2l1WFPW  I really do not want to do all of these manually.

[jeff_strater · Accepted solution]

Not really sure why the defaults don't work here.  I know that pattern faces (the default) won't work with some geometry cases.  This must be one of them.  Instead, use pattern features (Identical) instead.  That seems to work.

Jeff

[neljoshua]

@jeff_strater,

That worked great.  Thanks a ton!

I am not sure I understand why making a pattern of a feature rather than a face works, but I am thankful that it does.  The fact that one must click in the timeline rather than on the feature in the window is a bit confusing.  Can this be done in the direct modeling environment?  If so, how would one select the feature to pattern?

[neljoshua]

@jeff_strater,

The part is made of 18 gauge (1.21 mm) 403 stainless; there are two halves and they are welded together.  My plan was to shell the component after making all of the dimples.  The issue is that Fusion does not seem to like this operation.  I cannot get the shell to work.

[TheCADWhisperer]

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@neljoshua wrote:

The part is made of 18 gauge (1.21 mm)  ...  I cannot get the shell to work.

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What do you get for Rmin - .121=?

Hmmm, I think I would find a way to break the problem down into a pattern(s) of the shell.

I tried to shell at a thinner thickness and it brought my machine to its knees.

[neljoshua]

What do you get for Rmin - .121=?

@TheCADWhisperer,

I am not sure I understand your question.

I was thinking that if there was a way to turn the body from a solid object into faces that I could delete the back face and then thicken the part...but I do not know how to do that.

[jeff_strater]

OK, a few questions here that I will try to answer:

1. Face pattern vs. feature pattern.  This topic is a bit technical, but I can sort of explain.  A Face pattern is implemented by literally copy/pasting individual faces from the selected geometry back into the body.  This is very efficient, but has limitations.  The face along which the pattern occurs must be the same face.  Some geometries just cannot be pasted this way.  Tangencies complicate this process, which I suspect is what is happening here.  Feature pattern, on the other hand, works in several ways.  "Optimized" is actually very similar to Face Pattern.  I've lost what the actual differences are, to be honest.  "Identical", however, copies the tool body from the selected feature, and patterns that, and follows up with one big Combine.  "Adjust" actually copies the data model of the feature for each instance, and recomputes it.  Only use this if you need this level of compute - it is very inefficient.

2. Shelling this model.  To what thickness do you want to shell this?  I measured the distance from the bottom of the dimples to the back side, and it was 1.21 mm.  I was able to shell that design to 0.5 mm in the video below, and even up to 1 mm later.  What are you trying to do here?

Jeff

[neljoshua]

@jeff_strater,

Thanks for the explanation.

The minimum thickness on the part should be 1.21 mm, so I was hoping that I could use the shell feature to remove all of the material except where the spot welds are.  This may be too much to ask of Fusion.  Maybe I can increase the thickness of the part so that I can then give it the appropriate shell thickness.  The thing is that we are concerned about vibration modes and resonant frequency, so I really need this model to be spot on.

[jeff_strater]

Hi @neljoshua,

I still may not be 100% understanding what you are trying to do here.  But, here is another approach:  Just turn this into a surface body in the Patch workspace:

Jeff

[TheCADWhisperer]

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@neljoshua wrote:

What do you get for Rmin - 1.21=? 

I am not sure I understand your question....

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It is not physically possible to have a minimum radius of 1mm and a shell thickness of 1.21mm and have uniform thickness sheet metal material.

The outside bend radius should be at least Rmin+Shell (or sheet metal thickness).  The outside bend-inside bend should = thickness (shell).

If not, the sheet is not uniform thickness. (see image)

Also, I think I would reconsider using Spline in spotface geometry with the intention of Shell.

[neljoshua]

@TheCADWhisperer,

Thanks for the clarification.  I am going to make some adjustments to the fillets and try again.

@jeff_strater,

My intent is to have an accurate model of the plate so that I can perform some analysis on it (stress and modal frequency).  I realize that I am likely asking a lot of Fusion, but I have my hopes.

[neljoshua]

@TheCADWhisperer & @jeff_strater,

Thanks for your help thus far.  I spent some time re-working the model.  As per your suggestions I changed some of the fillets and changed the revolved spline sketch to a set of tangent curves.  Still, I am not able to produce the shape I want.

I tried using the patch workspace to delete the faces I do not need (the back and sides) and then thicken the surface.  This is the result:

I tried shelling the feature (to the outside) & this was the result:

What I really want to know is if I am running into a software limitation or if it is something I am modeling incorrectly.

[neljoshua]

I finally got it to work!

I am not certain what did the trick (maybe a combination of everything that I did), but here are the changes I made from the original model:

-Changed the revolved cut from a spline to two tangent arcs

-Significantly reduced the fillet radius

-Removed all of the fillets

-Deleted the back and sides in the Patch workspace

-Thickened the surface

Based on qualitative observations regarding number of crashes and processing time after each change, it seems that removing the fillets was the most helpful.  I am going to try to add the fillets back in now that I have the shell completed.

@jeff_strater & @TheCADWhisperer--many thanks to both of you for the help.