I am having unexpected results when using the sketched bend tool. I am using the Solidworks API to make a sheet metal part through creating a flat pattern, then sketching
the bends. When I try to bend the selected sketch line, shown in the next two pictures
, Solidworks extends the bendline across the bend relief zone, as shown below:
Any idea why this is happening and how I could prevent this, while still using the sketched bend feature?
Thanks.
Hi Colin,
not sure what is going on. In general, the sketched bend should stop at the bend relief when the line that defines the sketched bend does not extend the bend relief:
But it is hard to tell without actually looking at the model.
Kind regards
Frank Ruepp
Product Definition Team
I'm also having this problem and I've had it in a few dozen files, where solidworks just flat out ignores reliefs and sends all sketched bends to even far unrelated parts of a sketch. I have no idea why it's programmed to be so intent on pushing those bends over gaps as much as possible.
I mean granted, i try to use sketched bend as infrequently as possible, as it's basically useless for anything where you need a firm finished dimension (like anything that isn't purely decorative), but unfortunately a ton of legacy data and bad files give me little choice. File attached. Normally the problem goes away if I just make the bend relief ridiculously large, but that forces me to mess parts up and make them not to spec in order to get them in a drawing, which is unacceptable.
Look at flange Position. After you have picked edge flange, the 4th Item down "flange Position" By changing that it should help. Wish I could do a screen shot.
Forget that check this video and notice how he changes the position second Item down.
How to create sketched bends SOLIDWORKS tutorials Sheet Metal - YouTube
It's the same issue: the relief is still bigger than it has to be because the bend has been moved out. When we're talking about building components of machinery that have to be welded watertight or otherwise need to be made properly in a certain fashion, software glitches preventing me from doing my job are a problem,
I shouldn't have to put that burden on our welders because our software that costs more than everything I own combined can't perform simple tasks consistently and correctly.
Now if I spend a few hours replicating geometry perfectly through other means, I can get it, but that's impractical and suffers from yet other relief issues. SW has grown on me a lot and I now prefer it over others just from familiarity, but these bugs are deeply frustrating, and make me envious of those using SW competitors.
Hey Christopher,
here's something that I just tried and is a 'hacky' fix for our problem. You can select the faces that are co-planar but split by the extended bend line, then insert a 'Delete Face' feature with the 'Delete and Fill' function. This should merge the faces together.
Hope this is helpful for you,
Colin
Awesome, love it!
Is this the option you were referring to? Using this means I have to re-position the bend lines, but it doesn't seem to have the bug where the bend line is carrying over.
Thanks for showing me this!
The problem is that the bend lines can't be moved and geometry can't be changed because on parts like this they are job shop work, I can't alter the geometry. They send a DWG with the dimensions and geometry defined, and I've got to make it work or go have a technical argument with non technical people about it that will take up a couple days and cause drama. Now those DWGs were created from some 3d software at some point, but you know what a mess that is.
On my own parts of course I just change the geometry to work, on others parts I have to deal with solidworks glitching where other software packs don't on the same geometry. I guess it's more a whine than anything, Colin's solution seems effective.
I have run into this many times, my 'solution' was to simply specify a .001 bend radius but use the correct bend allowance/deduction for the actual tooling. I'm not really a fan of K-Factors, especially when I know the actual bend deductions.
I should clear up what I meant by saying move the bend line. Instead of drawing the center line of the bend allowance, draw a line on the edge of the bend allowance where the bend begins. When you insert the sketch bend, select the 'bend outside' option. If you position the line correctly you still end up with the same finished dimensions. I attached a modified version of your file to show what I mean.
Is this the option you were referring to? Using this means I have to re-position the bend lines, but it doesn't seem to have the bug where the bend line is carrying over.
Thanks for showing me this!