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Unable to unfold: Won't let me select part to unfold

9 REPLIES 9
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Message 1 of 10
pranv
595 Views, 9 Replies

Unable to unfold: Won't let me select part to unfold

Greeting everyone!

I am trying to unfold a tab and make a flat (single plane) part of a part. Unfortunately it is not letting me select the bends to unfold. The whole part goes transparent when i click on unfold and it won't let me select "stationary entity" as well.

I tried doing this on Inventor as well and was not able to select bends. Inventor selects the whole part as stationary entity.

 

The final goal of doing this is to get a 2D of the entire part - Not projection.

Please see file attached.

9 REPLIES 9
Message 2 of 10
kellings
in reply to: pranv

Hi @pranv I believe I see the issue. Note my arrow in this image. two sheet metal bends intersect there. There would be deformation where the two folds meet and Fusion doesn't know how to deal with the deformation of the material there. Both Fusion and Inventor can't create a flat pattern because of this deformation. 

 

SheetmetalDeformation.png

Kevin Ellingson
Technical Specialist

If my post resolves your issue, please click the Accept Solution button.
Message 3 of 10
pranv
in reply to: kellings

@kellingsThanks for the response!

How would I trick the software into ignoring the deformation?

Or is there a way I can flatten the part without unfolding and still get the true dimensions?

Message 4 of 10
dan.banach
in reply to: pranv

Hi @pranv 

I agree with Kevin. This is currently a formed part. You could try to split the body into two along the plane where the bends intersect. I also noticed that the larger bend is a spline not an arc, I'm not sure if this will cause issues.

 

Hope this helps.

-Dan



Dan Banach
Sr. Technical Manager & Community Manager

If my post resolves your issue, please click the Accept Solution button.
Message 5 of 10
pranv
in reply to: dan.banach

Hello @dan.banach !

 

I tried to split bodies but it is proving hard to split it correctly. Please see my effort attached.

What do you recommend for me if i need to get the true flattened part?

Message 6 of 10
kellings
in reply to: pranv

Hi @pranv Do you have access to the original SolidWorks file that was used to create this step file? Could the angle of that flange line change so the two bends don't intersect? Once the two bends don't intersect, I think this will flatten just fine. Would it be possible to have the original file changed to avoid the bend intersection? 

 

Kevin

Kevin Ellingson
Technical Specialist

If my post resolves your issue, please click the Accept Solution button.
Message 7 of 10
pranv
in reply to: kellings

Hi @kellings !


Unfortunately I can't alter/change the CAD. Also I do have the file shared with me but i did not find a sketch in the feature tree. I have attached the file for reference.

My end goal is to get a 2D flat design of the part. Something like the attached screenshot. Is there any way I can get that without unfolding the part?

For the attached screenshot, I have used the bottom (concave side) as flatten geometry. If i use the top (convex side) to flatten geometry, then I get a slightly smaller part profile. I am not sure what is true profile.

Message 8 of 10
kellings
in reply to: pranv

That was why I was asking if you could edit the file in the original software. When you export a file to a neutral format like step, only the geometry is exported. Sketches and feature history don't make the translation process. 

 

I can't think of a way to use the flattening tools in Fusion as long as the two bends intersect. 

 

Kevin

Kevin Ellingson
Technical Specialist

If my post resolves your issue, please click the Accept Solution button.
Message 9 of 10
dan.banach
in reply to: pranv

Hi @pranv 

In Autodesk Inventor, there is an Unwrap command that will get you close. Note that the Unwrap command does NOT use a K-Factor, so this is NOT a prefect sheet metal flat pattern. Attached are a couple files for you to review that I exported from Inventor..

Otherwise, I'd suggest removing the middle section and remodeling it using Sheet Metal tools.

danbanach_0-1675107477384.png

 

Hope this helps.

-Dan

 



Dan Banach
Sr. Technical Manager & Community Manager

If my post resolves your issue, please click the Accept Solution button.
Message 10 of 10
pranv
in reply to: dan.banach

@dan.banach @kellings 

Thanks to your inputs I was finally able to unfold the whole thing.

The part thickness is 4mm, so I made a 2mm offset surface of the part, in the direction of the part. I converted this surface into sheet metal of 4mm thickness but ignored the intersecting bend.
Then folded the entire part. Once I get a dwg of this, i'll redraw this rectangle in.

I highly appreciate your efforts and thanks a lot for guiding me!

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