topic two sections of sheet metal part fail to product flat patterns. in Fusion Support Forum

two sections of sheet metal part fail to product flat patterns.

artiedXDLWP — Thu, 24 Oct 2024 10:47:08 GMT

So i constructed this Y tee from scratch in fusion. Two of the sections generate error when making flat pattern. The two components are named "no flat pattern" in the model. This is the error "Error: FlatPatternAlign1(FlatPattern1)
Compute Failed" I don't know what the issue is or how to resolve. .F3D File is attached. Any help and suggestions are appreciated

Re: two sections of sheet metal part fail to product flat patterns.

HughesTooling — Fri, 25 Oct 2024 09:30:09 GMT

I think the problem is the end faces are not perpendicular to the sheet face. If you right click on the face there's no option to create a sketch which also means it's twisted and not flat.

Not sure how to construct the shape you want but doing a simple test trimming the end away and it does flat pattern.

Re: two sections of sheet metal part fail to product flat patterns.

HughesTooling — Fri, 25 Oct 2024 12:32:00 GMT

This bugged me a bit so played around a bit more. I've found a workaround if I trim one end (sharp corner) then extrude to create a flat face to select for the unfold. The fact this works points to it should work any way but Fusion is struggling to find how to flatten. @Phil.E Who would be best to tag for sheet metal?

I've attached my test. You could reduce the extrusion\trim to 0.001" once you've set it up and got it working.

Re: two sections of sheet metal part fail to product flat patterns.

HughesTooling — Fri, 25 Oct 2024 12:39:43 GMT

Testing a bit more and found I only need to create a flat face that's axial to the axis of the cylinder and it will flat pattern.

Here just a 0.001" flat.

File's attached.

Re: two sections of sheet metal part fail to product flat patterns.

artiedXDLWP — Fri, 25 Oct 2024 13:37:39 GMT

Thank you for the solution. Can you let me know the step you took to fix the part?

Re: two sections of sheet metal part fail to product flat patterns.

Phil.E — Fri, 25 Oct 2024 14:11:08 GMT

Thanks for letting us know. I'll notify the sheet metal team.

Re: two sections of sheet metal part fail to product flat patterns.

HughesTooling — Fri, 25 Oct 2024 14:26:18 GMT

@artiedXDLWP You should be able to follow the timeline to see what I did, helps if you activate the component so only the features for that component are in the timeline.

One thing that might not be obvious is I set the component's origin so it's rotated to match the axis of the tube. I first roll the timeline back to where the component was created before the body. Then make the component's origin visible and create a joint to position and rotate the component.

Then move the timeline maker after the thicken and create an axis through cylinder and add an offset plane for the sketch to extrude through the corner to create the flat.

In the sketch use Project, Intersect and the axis to create a point at the centre of the cylinder then draw a radial line to cut the corner off the component. At this point the part should flat pattern. I've attached the file again with the timeline rolled back to this point.