Contour Roll/Chamfer Issue with Flat Patterns

[bbrownXJGFR]

Hello gang. I've only been using Inventor for 6 months but I have 8+ years of NX modeling experience prior to this job opportunity. These forums are quite awesome and I'm posting for the first time. Please be gentle.

I'm currently trying to model a conical transition (read contour flange). I've been able to use the Unfold/Refold command successfully and easily created a flat pattern. I was even able to add some chamfers and a hole cut in the Unfolded state since that's realistically the easiest method for our shop folks.

This all worked splendidly until I tried to chamfer the outside edges of the part. At that point, my flat pattern turned into a Picasso painting of some sort.

 I have tried all sorts of things, but as soon as I apply an chamfer to these external edges, stuff goes sideways real quick. If I suppress the chamfer, the world gets better again. Either of these 2 edges causes the problem even if I only select one of them.

   Note that this material is 1.25" thick and doesn't qualify for the classic definition of Sheet Metal. In my world, though, this is thin stuff and we roll it and treat it like most shops would treat thin gauge material. I don't think that has anything to do with this "glitch", but I'm sure someone will notice that wrinkle in the fabric and point it out.

   I've attached the .ipt file for the wizards out there.

  My apologies if I've violated any basic posting etiquette. Thanks in advance. 

 

[kacper.suchomski]

Try adding a chamfer on the folded model.

[bbrownXJGFR]

@kacper.suchomski Thank you for the quick response. That didn't work for me either. It looks like the direction of the thickness is the issue. When creating my cone, I flipped the thickness in the opposite direction compared to your video. Can you see if you get the same behavior by either chamfering your inner edge or flipping the thickness direction?

It must only allow chamfering on the edges coincident with the original angled line in the sketch or something. Very cornfuzzling.

EDIT: It seems like my file didn't upload the first time. I just added it to my original post.

[kacper.suchomski]

It seems that the chamfer on side A cannot be created.

You can only add on one side so as not to disturb the base surface for the algorithm.

You have several exits:
1. Create a flat pattern chamfer. In the drawing, you will only see it in the flat pattern view.
2. Let it go if it doesn't significantly affect the work of the model and describe the chamfers in the drawing.

[bbrownXJGFR]

@kacper.suchomski I appreciate the confirmation of the behavior. I doubt this is an intentional limitation of these features, though. I'm planning on putting these parts into a weldment assembly anyway, so I can create the conical weld prep in that stage while still showing the bevel in the flat pattern, as you have suggested.

I'm curious to see if anyone else has experienced the same issue and found an alternate workaround.

Thank you!

[johnsonshiue]

Hi! I believe it is a bug or a limitation. The issue here is that the Unroll process creates a bad body. It is possible the Chamfer16 isn't compatible with the Unroll. You may need to create the chamfer in the flat pattern body.

Many thanks!

[IgorMir]

Here is a part in IV2020 format. Looks error free.
Try to put edge Chamfers at the very end of modeling. That way you will keep the sheet metal features uninterrupted by the standard feature. Just a suggestion on my part.

Cheers,

Igor.

[SBix26 · Accepted solution]

In 2023, it appears that the Unfold - Refold operation leaves the edges in a strange state.  I'm not able to select the end faces at all.

I was able to get the job done, though, by initially rolling a bit past 180°, unfold, place hole, refold, then trim back to 180° (using the YZ plane).  Then I could chamfer all edges in one operation, and the flat pattern looks as it should.

Note that there is no need to use the Contour Roll tool for this, though I suppose it doesn't hurt anything-- I just used Revolve.

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Sam B

Inventor Pro 2023.2 | Windows 10 Home 21H2

[kacper.suchomski]

@SBix26  wow! Works for me too when I use revolve.

[bbrownXJGFR]

@johnsonshiue Unfortunately that doesn't really improve my workflow. Typically, we like to show all chamfering first for drawings and detailing which allows it to show up in the weldment assembly already prepped for welding these two cone halves together to make a bowl shape. Thank you for the suggestions, though!

[bbrownXJGFR]

@IgorMir Thank you for the effort. It seems that the issue is the perfectly square vertical ends of the rolled cone. Yours works only because you chamfered those vertical edges also. When i eliminated those, the same error occurs.

Thank you!

[bbrownXJGFR · Accepted solution]

@SBix26 I think you've found the culprit. I can roll this to any angle other than 180 degrees (179.9 or 180.1 for example) and the issue is resolved. Additionally, @IgorMir solved it accidentally by chamfering the vertical edges as well, which actually works perfectly with my workflow. This is a strange bug/glitch, but it seems we've found a viable long-term workaround.

EDIT: Well it looks like @IgorMir also solved it by not chamfering the top edge by more than half the thickness of the plate. Any chamfer under 1/2*thickness in conjunction with the vertical edge chamfers will produce a viable flat pattern.

I think the cause here is that the projected shape of the resulting flat pattern with all of my necessary chamfers applied actually produces an undercut part. It would seem that when chamfering edges results in a smaller flat pattern than the necessary base shape, IV throws out garbage. 

I'm actually not upset about this behavior at all since it will likely make some people adjust their workflow to prevent undercutting their parts, which is beneficial. It would be optimal, though, if Inventor simply offered an error message and/or a way to produce the proper flat pattern needed to be able to apply said chamfering. Nonetheless, the behavior is at least understandable, now.

Thank you!

Thank you all!

[IgorMir]

Yes, the FP is going strange when vertical chamfers are removed. I put them there initially because I thought - you need a weld prep all the way around the edges.

Cheers,

Igor.

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@bbrownXJGFR wrote:

@IgorMir Thank you for the effort. It seems that the issue is the perfectly square vertical ends of the rolled cone. Yours works only because you chamfered those vertical edges also. When i eliminated those, the same error occurs.

Thank you!

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