I've attached a part.
When I try to do an Insert Bends, I get an "The face belongs to an existing sheet metal body" message.
For some reason, SolidWorks thinks this part is already sheet metal.
Thanks for any help.
Just begin the convert to sheet metal, touch the base then escape out of it. Edit your sheet metal feature change material thickness and bend radius, then delete the face (any face on the surface) undo, then the insert bends works.
Interesting.. I don't know.. maybe Dennis Bacon or someone else familiar with a external reference body (8000-120_base_part.SLDPRT)?
It looks like the part was created by inserting another part or a mirror and it probably had the checkbox selected for sheet metal features.
Casey,.. I rolled up below the insert and was able to add/convert it to sheetmetal.. rolled back down.. it showed errors (as I expected).. but 2016 crashed and burned when I did a ctrl-q? (ouch!)
I don't get that error. But what I would do is:
Start another body using the sheet metal parameters you use. Use up to Vertex for your flange lengths. Convert the cut outs. Delete the original body as your last feature.
It should take you maybe 10 minutes.
for what it is worth... it works fine here... on 2017 SP1
I tried converting it on 2016 and it was erroring out as well. Looks like Jason Edelman says it works on 2017 below.
..interesting also.. I get the error in both 2016sp5 and 2017sp2?
See attached for 2017 SP1 file...
well,..if I pre apply R.004 and R.064 fillets.. it works in 2016sp5 and 2017sp2 using "convert to sheetmetal"
..after experimenting I got it to work but.. it crashed on me two other times just selecting a face..? (2016sp5)
..I'd guess the selection of the external reference maybe sending a call to find the file (which is not there).. and it goes into loop (memory error)?
btw,.. it also crashed after opening and exiting the original file in SW2016? (odd.. again.. maybe something to do with the external file?)
Interesting... I have run across this before. Notice that there is a greyed out thickness in your equations. SW thinks this is already sheet metal. What I ended up doing is delete a face then do an undo. Then I was able to do an insert bends without issues. Really quite simple. I got in on this a little late cuz I'm actually making money today!.. Now I hope I can remember this for similar issues in the future.
Hmm,, I'll bet that by adding the fillets it has the same effect as deleting a face then doing an undo. Good show Paul.
Thanks Dennis (and others).
That was a great find, the thickness defined in an equation.
I can't wait to try fixing it tomorrow when I get to my workstation.
I've never deleted a face before, not to ask a stupid question, but how do I do that?
Did simply deleting the thickness variable work?
No. I could not delete the thickness variable. It would not let me. When I deleted the face then did an undo then insert bends it did change the thickness variable to the correct thickness though. The variable was .075" (I think). Now is .060" (model thickness). I attached my file.
When you delete the face check the delete (only).. Then the green check mark After that and before you do anything else do an undo.
Edit:... If you uncheck Link to external file in your equation manager you will get rid of the irritating equation error. This alone does not allow you to insert bends but does make the feature tree look better.
Michael,,, Before you try what I have done and get really frustrated I better relate to you what I found out this morning. I tried it again from scratch and could not get this to work. Found out that I had to use "Convert to Sheet Metal" first. I just selected my base then hit escape. Once you do this you get the "Sheet-Metal" feature at the bottom of your tree. Then I edited the feature and set the material thickness and reduced the bend radius to .005. If you want to use a larger bend radius for some reason you will have to make your corner relief (cut extrude) slightly larger. Now you have your default sheet metal parameters set. Then do the delete face - undo - Insert Bends.
I had done some fiddling with this yesterday prior coming up with the delete face so was unaware that was a necessary step. This sort of stuff can drive you crazy but it is really easy and probably the quickest way if you follow.. I do prefer to use the "Insert Bends" also.
I wasn't able to get it to work.
I did a "convert to sheet metal" and ended up with just the bottom of the part.
I then deleted that sheet metal, tried an "Insert Bends", and ended up with the same error.
Michael... if it helps.. here is a fixed 2016 version,.. this will accept "Insert Bends" or "Convert to Sheetmetal"
My modified steps from Dennis to fix were....
1 - Manage Equations and Cancel.
2 - Pre-select a bottom face and "Insert Bends" (and. pre selecting seems to work as well??? )
Dennis,.... you had me scratching my head on your combo last night and now this one as well... how did you figure that combo out!?
My fixed 2016 file below was different...
2 - Pre-select a bottom face and "Insert Bends" (and,.. pre selecting seems to work as well??? )
Got it! Was able to follow your directions.
What a pain in the rump. Dang.
Thanks guys, that was a HUGE help! Very much appreciated.
I'm not the type to just throw in the towel and start the part from scratch again, I like to learn, which is what you guys helped me do.
I was able to delete the global variable easily.
So was I, but that didn't fix the problem.
I noticed I was able to delete it if I did it right after opening the file. When I opened the file and fiddled with it some then I could not delete it.
I have no clue Paul. Just dumb luck. Seems to work every time though. I am not able to replicate your method. I'm done with this. If I continue trying to figure out why,, the guys in white coats will be paying me a visit.
I'm able to convert the file to sheet metal in 2017.
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