I need to insert a flat into my drawing of a mirrored part. But I can not find a way to create a flat with the part...
Is it possible to create a flat from a mirrored sheet metal part?
If you are not using 2015 I found that the part you posted converts to sheet metal easily by using "Convert to Sheet Metal" and flattens correctly. Might be another option. I noticed that your stamped in mirrored part number disappears.
Edit:... For some reason "Insert Bends" didn't work without errors.
I'm not sure if you can flatten a mirrored sheet metal part. I know there are several options when you mirror it. I will look into that, but, can't you just flip your flat pattern from your original (non mirrored) part?
That's is what I just did. I inserted the original part it was mirrored from. the just flipped and rotated it to be correct.
The problem is, they are no longer exact mirrors. I broke the link and made changes to the once mirrored part. So these things will show up in the flat. Which I can hide in the drawing view. But I need to also make a DXF and do not want to create problems with this.
I understand Keith. Seems like I have done the same exact thing in the past, adding/subtracting features in the mirrored part. I'm racking my senior brain (doesn't seem to work as well as it used to) trying to remember how I solved this issue. I may have done this with configurations in the original. Let me refresh my memory by playing with this.
Thank you! I appreciate the help!
I have attached the part in question.
2015 you can check the Sheet Metal Information box - then you'll be able to flatten it
What version are you using Keith. I think this was new in 2015 but while mirroring I have the option to retain Sheet metal information in the mirrored part. When I check this my mirrored flattens. I can add holes etc.
Do you have the same options?
Going to check the what's new.
I see that John beat me to it.
Thanks! This worked perfectly!
If you don't have SW2015, the old method was to create your mirrored part. Then add a "Convert to Sheet Metal" feature. This will reestablish the imported solid as a sheet metal part and you will be able to flatten. You can also keep it linked to the original (if that is your design intent) and then add unique features as needed.
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