Flat Pattern DXF Export Issue

[Anonymous]

Hi all,

I'm looking for some help. I get the following error when exporting the flat pattern to DXF.

Error Shown

I've looked around the forum for other posts but I don't believe they solve my problem.

The only "work around" I've used is described here where i've had to adjust two of the bend angles to be 89.99 degrees:

https://forums.autodesk.com/t5/fusion-360-design-validate/flat-pattern-not-flat-and-warning-not-read...

I've attached the model, any help would be appreciated.

Thanks.

[Anonymous · Accepted solution]

It appears I've found the issue.

I had created multiple holes by using sketch and cut "through all". This meant I cut through multiple faces when folded which seemed to confuse the DXF export. 

Adding the screw holes a face at a time, or adding the holes when flat, appears to fix the issue.

Rather frustrating!

[stevsmar13]

Looks like I'm having the same issue too.

[robLBYMJ]

Sounds like a bug that needs to be fixed.  I, for one, would rather be able to drill bolt holes through so the bolts align properly.  I have a hard time imagining how to do this without doing it in this manner.

[robLBYMJ · Accepted solution]

Ok,  so I tried a number of things and did some experimentation.
First, I went through history to find what holes were causing the issue.  Turns out there were four holes that were causing the DXF export to freak out.  The holes that were causing the issue were generated using a sketch within a child component.  To do this, I backed up my history until the DXF import worked, then suppressed the features that were causing the issue and fast-forwarded my history to make sure nothing else was causing issue.   It turns out holes punched from sketches on the same component (even holes punched from sketch in copy A through to copy B) work just fine, the issue happens when you punch holes through different components.  It would be appropriate if I were to name these components for you so you understand.   The "Barrel" component has a motor mount on it, we'll now call "Mount."  Anyway, the sketch was in the Mount component.  At first I had holes bored through the Mount and Barrel.  I deleted the holes through the Barrel, and re-bored them only through the Barrel (Mount was unaffected) but that still didn't work.   So what I ended up doing was creating sketches in the Barrel, projecting the holes through from the sketch in Mount, and boring from there.   This worked and now I don't have problems exporting the DXF file.

[HughesTooling]

In the model in the first post the tabs are at a 0.1° angle. Because of this the extrusion cutting the holes is only perpendicular to the face the sketch in on, also as it goes through the faces on the other side of the model the holes that side are out of place and angled through the steel.

Instead of angling the face you could extrude the face a small amount before creating the flanges.

With all the faces parallel the flat pattern works and can be exported as a DXF. File Attached.