Sheetmetal Body moves after unfold-refold operation

[swalton]

Inventor 2020.2.1

I made a contour flange sheetmetal part.  The original contour sketch is tied to the part origin.  After some unfolding, cutting, patterning and refold features, the solid body is offset from the part origin.  

What do I need to do so that the body stays flush with the origin planes? 

[DavidTunnard]

Hello. I just tried opening the part but appears to be derived from another part as it has no history so I can't look at what you've done. Could you post the original part?

One quick thing I can think of though is to make sure the same face is selected as reference when folding/unfolding.

[TheCADWhisperer]

It appears to me that you did not select the correct reference face for the Refold.

Well, I tried to select correct reference when editing your feature and saw same behavior.

But if I create a new feature - it works as expected for me.

This issue can be avoided altogether by using Project Flat Pattern and Cut-Across Bend rather than Unfold/Refold.

[TheCADWhisperer]

---

@DavidTunnard wrote:

Hello. I just tried opening the part but appears to be derived from another part as it has no history ....

---

The history is there. 

You must be using an older release of Inventor than the file.

Although @swalton signature indicates using 2019, in the body of the problem description indicates using 2020 for this file.

[DavidTunnard]

Ah that would make sense. Yes, I am on 19 still.

[swalton]

I don't usually use the project flat pattern tool.  Old Creo habits, I guess.

I may have rolled the EOP back and forth as I decided on the various features in the part.  I wonder if that is why you see a newly created feature keep the offset from the origin plains.

I'll use the project flat pattern technique for this part.

@johnsonshiue : Is this expected behavior from the modeling kernel?

[TheCADWhisperer]

---

@swalton wrote:

I'll use the project flat pattern technique for this part.

---

Here is example.

(See Attached.)

[Curtis_Waguespack]

Hi @swalton ,

It seems like a bug to me, hopefully johnson can help us understand the issue better.

I had a hunch as to what the issue was and took a few seconds to test with the file.

Here's what I found:

• If I made the Extrusion feature a Cut feature with the Cut Across Bends option selected, the issue persisted.
• If I made the sketch for the cut feature a simple rectangle and added the fillets as feature fillets using the Sheet Metal tool called "Corner Rounds" then the part refolded properly without moving.

Edit: also I should include the extrusion version and note that if the fillets were added as features rather than in the sketch it refolds as expected, regardless of a using Cut feature or Extrusion feature

Here are the example files (Inventor 2020), in case it helps you or helps Johnson in determining the issue with Refold. 

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[jeremy_wasserstrass]

If you do a split face to get the bend extents to go across the face of the part before refolding the part will not shift around. I have had issues with those particular sketches going sick as soon as I make a split feature. See the attached part.

[CCarreiras]

Hi!

First, the unfold/refold is a very complex feature, and i only use it if there's no other option.

In this case, you could avoid it easily.

I think the problem is that you change a lot the primary stationary face, and when you try to refold it again, the stationary face reference is somehow different.

In these cases, if you use another face as stationary, that remains almost the same at the refolding stage, the refold will have a more expected result.

My part in attach.

[johnsonshiue]

Hi Steve,

This is a bug. Unfold and Refold should not relocate the body. I just try it on our internal build targeting 2020.3 update. It seems to work fine now. You do need to use Manage -> Rebuild All, when 2020.3 update becomes available.

Many thanks!

[lena.talkhina]

Hello @swalton  !

Great to see you here on Inventor Forum.

Did you find a solution?
If yes, please click on the "Accept as Solution" button as then also other community users can easily find and benefit from the information.
If not please don't hesitate to give an update here in your topic so all members know what ́s the progression on your question is and what might be helpful to achieve what you ́re looking for. 🙂

[teepee11]

I was having this same problem with a cone, I was making a cut of .1 mm in wall of cone,(rectangular sketch projecting out to cut material) and cone would flat pattern ok. but when i unfold it and refold it it would move away from part location.

The solution I found was when i made the cut, if i cut the 0.1mm using evenly in both directions choice instead of selecting one direction only, it will unfold and fold in the correct location.

[johnsonshiue]

Hi! The original issue has been addressed in recent releases. The Refold will not alter the body position before Unfold. However, I do recall there are still some unresolved cases. For example, a partial cone can still lead to unwanted move.

This is because the Unfold/Refold reference somehow cannot be found. It is a bug.

To avoid the behavior, you may want to create good planar reference (like a flange tangent to the cone). In this way the Unfold/Refold can rely on a stable planar reference.

Many thanks!