Fusion
Your Fusion 360 is probably setup with a Z-Axis Up configuration (default) so you are modeling your sheet metal component on X-Z plane which will cause the flat pattern to be created on edge to your view. Create you sheet metal initial sketch on the X-Y plane and you will get expected results.
John Hackney, Retired
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The application has to work on some rules and just because you do not agree with those rules, it is not a bug. The X-Z plane is basically modeling a model hanging on the wall, the X-Y plane is modeling one lying on the floor or base surface.
Edit: Also, do not use the Quick Reply icon, it addresses your post to yourself. Use the Reply icon, on the Forum post of the person you are addressing instead.
John Hackney, Retired
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Why do you want a flat pattern of something that's already flat. Does this still happen if you have something more complicated with bends added.
Mark
Mark Hughes
Owner, Hughes Tooling
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Just doing a simple test adding a flat to the circle and it works correctly so it looks like the problem is only caused when you have a flat circular part. I guess having just one surface edge is the problem and not something most people would ever come across because what's the point of creating a flat pattern of a flat part. Yes probably a bug but doubt there would be a rush to fix something like this. @Phil.E What do you think?
Here's what I get by just adding one flat.
Mark Hughes
Owner, Hughes Tooling
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Was the more complicated part also flat with no straight edges?
@chance_hogelie wrote:
is there a work around? Yes there is, reorientation or rework of a certain part just for dxf export file purposes just adds another step. Adding the small flat section to the circle is interesting though, could make it small enough that cnc could barely notice it though.
An easier workaround would be just create a sketch on the face of the finished part and project the face into the sketch then export the sketch using Save As DXF. Note. Be careful if you have autoproject enabled as it will automatically project the face so no need to project again.
Mark
Mark Hughes
Owner, Hughes Tooling
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@chance_hogelie wrote:
Adding the small flat section to the circle is interesting though, could make it small enough that cnc could barely notice it though.
I experimented a bit with this and it doesn't seem to matter where the flat is, inside a hole, outside or just a square hole and the pattern is created correctly.
Any of the flats below give a good flat pattern!
Mark Hughes
Owner, Hughes Tooling
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Thanks everyone. This is definitely a bug, but also what I would call a corner case.
Typically more effort is given for flat pattern workflows that require flattening to create patterns, but as @chance_hogelie points out, this is narrow thinking because flat pattern export = flat pattern export when it's your daily workflow. Especially if 99% of what you do has bends, and then this "corner case" comes along and breaks your daily workflow. This makes it a higher priority case.
I'll log this as a bug and ask the sheet metal team to take a look. It is entirely dependent on the Z axis. No matter what the default "up" axis is, with designs like this the flat pattern will default to Z up exclusively. Just looks like a case that wasn't anticipated or caught yet.
Phil Eichmiller
Software Engineer
Quality Assurance
Autodesk, Inc.
Logged as FUS-104899. The reason for this is the flat pattern logic will default to Z up when there are no model edges that can give the flat pattern coordinate system a direction. Hence, adding a flat will get around it. (pardon the pun)
Phil Eichmiller
Software Engineer
Quality Assurance
Autodesk, Inc.
Hi again.
The latest Fusion updates (since November 19) should have the fix for this issue in it. Can you please give it a try and let me know how it goes?
Update can be activated from the help menu.
Phil Eichmiller
Software Engineer
Quality Assurance
Autodesk, Inc.
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