Flat pattern error after mirror of sheet metal part. Error: "Cannot create flat pattern because the relief radius..."

[johan_lidberg98EA4]

Hi! 

Ive run into a strange flat pattern error. Ive got a project that includes a number of sheet metal components. They are all well and healthy including flat pattern. Then i made a mirror of these components, deleted the flat pattern on the mirror components and and made new flat patterns. This was all well and good for 8 of the components, but for 1 of them the flat pattern is dead and i cant figure out what is wrong. I have included the error warning that i get when i try to make a flat pattern. Could this be a bug? Thankfull for you insights! / Johan

 

 

[jhackney1972]

Please attach your model.  Open in Fusion 360, select the File menu, select Export and save to hard drive. Attach to a reply post using the Attachment section.

[johan_lidberg98EA4]

Oh ofcourse.

Ive only exported the one plate that has an error due to business secrecy. 

Would be thankfull for the help! 

[jhackney1972]

The marked extrusion was causing the issue.  Model attached

[johan_lidberg98EA4]

Okay, thanx for you looking into the problem. 

But i have tried to both delete that feature and supress it. And i still get the same error both in my original design and in the file you sent. 

What was wrong with that cutout and how did you find out? 

Regards/ Johan 

[HughesTooling]

It looks like the problem goes back to the first body before it's mirrored. 

I created a flat pattern and stepped the timeline to different places to see where a good pattern was created. When these 2 pockets are created you get a warning.

Step back before and you get a good flat pattern.

Not sure what's causing the error. I tried offsetting the edge on the bend so they where no longer aligned but that doesn't help.

[johan_lidberg98EA4]

Thanks for looking into my problem! 

Hm Okay, will look more into those cutouts.

But its still strange that the other side before the mirror made a fine flat pattern of the same cutouts and has been sent to manufacturing with no problem. and now suddenly its error! 

Only thing i can think of is the fusion maintence they did this saturday.

So annoying! 

[TheCADWhisperer]

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@johan_lidberg98EA4 wrote:

But its still strange

So annoying! 

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I would expect to see unpredictable "strange and annoying" behavior using the modeling technique that you used for this part.

1. I would have only one Unfold/Refold (go back in history to add additional items to Unfold).

2. I would fully define each and every sketch.

3. Be particularly careful how you define geometry that crosses (or especially meets up to) bends.

[HughesTooling · Accepted solution]

Started typing below before @TheCADWhisperer reply but looks like his advice about using too many unfolds is the problem.

Ater some more experimenting it almost seems like Fusion's getting confused by all the unfolds and refolds. By deleting most I get a good flat pattern but as soon as I roll the timeline past the last unfold\refold I get a warning even though there was no change to the body!

With the timeline here you get a flat pattern with no warning. See attached file. I've removed some earlier unfold\refolds as well and modified the 2 rectangular cutouts so they're mode in the folded condition.

[johan_lidberg98EA4]

Yeah that may be so 😅

Will try to minimise the amounts of fold commands. 

And i thought i had constrained all the sketches, but maybe not. Will look into that also

[TheCADWhisperer]

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@johan_lidberg98EA4 wrote:

Yeah that may be so 😅

Will try to minimise the amounts of fold commands. 

And i thought i had constrained all the sketches, but maybe not. Will look into that also

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@johan_lidberg98EA4 

I would have only one Unfold/Refold.

Unconstrained sketches show blue and white dots and no Lock symbol in browser - hard to miss.

But especially these two edges should be constrained relative to the edge of the bend...

When adding geometry to Unfold/Refold...

1. Unfold the part.

2. Sketch on the part face with appropriate P for Project.

3. Create feature (generally a cut).  (Any cuts that can be done before Unfold - do those on before Unfold.)

4. Unfold to check

5. Flat Pattern to double check (examine in wireframe shademode to verify no double edges).

5b. Ctrl b (or CMD b on Mac) for sanity check.

6. Step the Timeline back one step before Refold.

7. Sketch additional cuts and repeat steps 4 and 5. (Update Flat Pattern)

[johan_lidberg98EA4]

Aha! Thank you!

All my sketches are fully constrained. But i had managed to make the sketch for this (and probebly more) feature in another component cuz im tired and stupid early in the mornings! 

And when i exported only this component for u guys this highlighted the problem cuz then the sketches didnt follow the exports and thus turning the sketches unconstrained! 

Thanx for your help! 

This is how the sketch looks for me.

 

[johan_lidberg98EA4]

Thanx for your help! 

Yeah it works to take away the unfolds and do a normal cut on the folded part in this case where the bend is 90 deg. But this happens to be the only 90 deg bend in the whole design 😅. On other bends i need to go in and unfold the part if im gonna cutout over the bend right? Or is there a better way to do it? 

Regards

[johan_lidberg98EA4]

Got it working now by a combination of your tips.

Got rid of all the unfolds, deleated the cutouts. made one onefold in the end of timeline. did a sketch that was IN THE SAME COMPONENT 🤣 and extrudcut with that and then refold! Perfect flat pattern! 

Thanx again for the help!