Can't unfold sheet metal

[calvinisthor]

I cant seem to fully unfold this sheet metal to be flat, even if I put a split in the face with the rip tool, as only some of the curves show up as bends.

File: a360.co/4nuwAYI 

[TheCADWhisperer]

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@calvinisthor wrote:

 with the rip tool

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@calvinisthor 

I do not see the history of how the part was created in the Timeline?

I do not see this Rip feature in the file that you referenced?

[calvinisthor]

I undid the rip as it didn't help, and the part was created by using the offset tool on a surface, then thickening it to create the part, as suggested by the fusion docs.

[Warmingup1953]

Yes, agreed that Sheetmetal body won't unfold or flat pattern as it is and probably can't be saved I'd say by a quick play with it. Can you post your original Fusion file?

[TheCADWhisperer]

@calvinisthor 

[calvinisthor]

When I try to use the lofted flange tool I get his error message: Cannot create lofted flange with the current selection. Adjust the flange settings or select different profiles.

[Warmingup1953]

We can't help (effectively) without your Fusion file.

[Warmingup1953]

I think you'll need to create a different way...Here is my quick go

NB. Ignore the file name

[calvinisthor]

Here is my fusion file

[TheCADWhisperer]

@calvinisthor 

Sketch22 is missing dimensions.

When I start to add the missing dimensions the geometry size does not make logical sense.  Are your intended units mm or inches?

I recommend modeling with symmetry about the Origin.

Blue curves should keep you awake at night.

Sketch 23 not symmetrical.  Missing Tangent Constraints. Missing Coincident Constraint.

I would model the Rip in the Lofted Flange sketches.

Fully defined sketch symmetrical about the origin...

Well, after experimenting with this I could not get Fusion to create the Lofted Flange...

[Warmingup1953]

I have had a quick look aty your file and as expected I am not seeing a way forward in Sheetmetal. What are you trying to do here? Just design or will you laser cut steel and form to this shape? What will it be?

[johnsonshiue]

Hi! The two sketch profiles contain elliptical corners. The Loft based on the two profiles has spline faces, which cannot be unfolded. The Lofted Flange command does not like the profiles either. I did find a workflow to approximate the intended geometry. I modified the sketches and recover the sharp corners (two rectangular profiles). Next, create a Loft surface from the two rectangular profiles. Add chamfers to the four corners. And add fillets to the edges approximating the quarter ellipse. Lastly, thicken the surface body, convert the body to a Sheet Metal body, and rip a face. The resultant body can unfolded. Please take a look at the attached file.

Many thanks!

[TheCADWhisperer · Accepted solution]

@calvinisthor 

OK, I got it to work..

Edit the dimensions as needed and let me know if it breaks.

I think this could be further simplified by sketching only 1/4 then mirror the surfaces twice and rip (trim) before thickening.

[calvinisthor]

I changed all the dimensions, but now the sheet metal wont refold

[TheCADWhisperer]

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@calvinisthor wrote:

I changed all the dimensions, but now the sheet metal wont refold

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@calvinisthor 

Can you File>Export your edited *.f3d file to your local drive and then Attach it here to a Reply?

Unfold/Refold is different than Flat Pattern.