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Help w/error: "part contains features that cannot be unbent"

Question asked by Stephen Reed on Oct 25, 2010
Latest reply on Oct 26, 2010 by Stephen Reed

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I hope someone can help with this. First let me say that I'm not a sheet metal person, so I'm not very familiar with that function in SolidWorks. However, I have this part (see attached) that is giving me an error that says "This part contains features that cannot be unbent" and flags the flat pattern in the tree with red. The odd thing is that everything was fine until I added the last feature, "Cut-Extrude3" which puts a notch on the inside corners of each "leg". As soon as I added the notch, I started getting the error. No doubt it is something in the way I've applied this feature but I have no idea what it is or how I can add the notch without corrupting the flat pattern.

Any help from you sheet metal experts will be much appreciated,

Steve

Wayne Tiffany Oct 25, 2010 9:48 AM

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Can't tell for sure since you only posted a pic, not the part. But most likely you made the cut such that you exposed an edge of the part that is not material thickness, as in ended the cut in the radius . Depending on what you need, change the cut to cut up above the top of the radius, or put in an Unfold, put your cut in, put in a Fold. This should let you leave a bit hanging down in that area if that's what you need. If still a problem, post the part.

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Wayne Tiffany Oct 25, 2010 9:48 AM

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Deepak Gupta Oct 25, 2010 11:06 AM

Try selecting "Normal to" or "Link to Sheet thickness" in the cut extrude feature.

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Daniel Melendez Oct 25, 2010 12:50 PM

Hi Stephen I'm with Wayne on this one. It appears you've cut the notch so that it bisects the radius. Either cut the notch past the bend line on either side of the radius. Or before the cut extrude do an unfold command. Put in the notch at the desired location, mid radius or not, and the do the fold commmand and you should be good to go. Thanks, Daniel

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Carter West Oct 26, 2010 11:04 AM

Hi Stephen,

I was able to duplicate your error. It may be possible that you have a coincident relationship setup between your sketched line, and the back edge of the bend:

In this example, the flatten option is now disabled, and indeed has turned red in the tree. Take a look at your sketch geometry and for the moment, delete any relationship that may be stopping the feature from unfolding.

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Stephen Reed Oct 26, 2010 11:59 AM

Yes! That was it, just as Wayne and others of you indicated the cut was in the radius. Once I made the suggested change, it flattens just fine, without any errors. And, just as I suspected, it was how I applied the feature. Since we are a woodworking plant, I haven't had much reason to do sheet metal and was just trying to follow the help and tutorials. Also, using the unfold/fold commands as suggested, I was able to put in a radius cut in the vertical part of the leg without error.

Thank you Wayne, Deepak, Daniel & Carter (hope I didn't miss anybody) for the sheet metal lesson. You guys are the greatest!

Thanks Much,

Steve

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Wayne Tiffany Oct 25, 2010 9:48 AM
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Can't tell for sure since you only posted a pic, not the part. But most likely you made the cut such that you exposed an edge of the part that is not material thickness, as in ended the cut in the radius . Depending on what you need, change the cut to cut up above the top of the radius, or put in an Unfold, put your cut in, put in a Fold. This should let you leave a bit hanging down in that area if that's what you need. If still a problem, post the part.

WT
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Deepak Gupta Oct 25, 2010 11:06 AM
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Try selecting "Normal to" or "Link to Sheet thickness" in the cut extrude feature.
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Daniel Melendez Oct 25, 2010 12:50 PM
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Hi Stephen I'm with Wayne on this one. It appears you've cut the notch so that it bisects the radius. Either cut the notch past the bend line on either side of the radius. Or before the cut extrude do an unfold command. Put in the notch at the desired location, mid radius or not, and the do the fold commmand and you should be good to go. Thanks, Daniel
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Carter West Oct 26, 2010 11:04 AM
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Hi Stephen,

I was able to duplicate your error. It may be possible that you have a coincident relationship setup between your sketched line, and the back edge of the bend:
In this example, the flatten option is now disabled, and indeed has turned red in the tree. Take a look at your sketch geometry and for the moment, delete any relationship that may be stopping the feature from unfolding.
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Stephen Reed Oct 26, 2010 11:59 AM
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Yes! That was it, just as Wayne and others of you indicated the cut was in the radius. Once I made the suggested change, it flattens just fine, without any errors. And, just as I suspected, it was how I applied the feature. Since we are a woodworking plant, I haven't had much reason to do sheet metal and was just trying to follow the help and tutorials. Also, using the unfold/fold commands as suggested, I was able to put in a radius cut in the vertical part of the leg without error.

Thank you Wayne, Deepak, Daniel & Carter (hope I didn't miss anybody) for the sheet metal lesson. You guys are the greatest!

Thanks Much,
Steve
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Help w/error: "part contains features that cannot be unbent"

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