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Looking for help with Sheet Metal bend

Question asked by Sam R on Sep 25, 2013
Latest reply on Oct 3, 2013 by Sam R

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Hello folks;

I'm wondering if any of you advanced modelers can advise me on a strange twitch going on with sheet metal sketched bends.

I've built a couple of metal parts for a bicycle and I need to have the dropouts bend to accept the chainstays. Unfortunately after I build the part and sketch my bend line, This happened once before and, not being able to find the right forum, I ended up redrawing the part which resolved it in a roundabout way. But there must be a way to repair this

problem quickly.

Thank you in advance for any advice

Matt Sparks Oct 3, 2013 8:18 AM

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Sam, I opened your model and made a new sketch (Sketch3). This is a little trick we use at our sheet metal shop to configure bend lines. It not only marks where to bend the part in our press breaks but helps the operator as there is no lay out needed. The cut is large enough for our laser to cut but small enough to not effect the part. This helps when you get into sketched bends as you can just select the center of both cut-extruded holes; making no need for construction lines in your sketched bend. Hopefully this helps. I have attached some images for reference.

Regards,

Matt

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Adrian Velazquez Sep 25, 2013 7:43 PM

Sam, your SketchBend (Sketch2) has excess geometry, just have the actual bend line and not all the extra reference geometry.

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Sam R @ Adrian Velazquez on Sep 25, 2013 8:53 PM

Thanks Adrian for the advice. You're right that excess geometry is often a problem that I've experienced before.

But in this case, it hasn't affected the part at all. I removed or converted to construction lines everything but the bend line. However the features are still greyed out.

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Adrian Velazquez @ Sam R on Sep 25, 2013 11:54 PM

Convert it to SheetMetal first (in the flat), then try the SketchBend Feature.

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Bernie Daraz Sep 25, 2013 8:58 PM

I haven't done the sketch bend in a long while, I believe it cannot be a construction line. Also the part is not Sheet Metal yet, right?

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Sam R @ Bernie Daraz on Sep 25, 2013 9:47 PM

thanks. I do feel silly. My previous experience with 3D cad was that the file had to be sheet metal or not. But SW just converts it. My bend line is not a construction line, just the reference geometry which defines it.

Once converted to sheet metal, the functions become accessible. However I get an error msg reading 'Sketch contains unsupported entities for this feature.' Given that there is only one line which isn't construction, I don't know what that would be referring to.

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Lon Eding Sep 26, 2013 8:21 AM

It definately does not like the arcs, regardless of whether they are construction or not. The SolidWorks Help file on Sketched Bends in the first bullet point says "Only lines are allowed in the sketch." Only after deleting all the arcs and attaching the line you dimension from to other geometry using coincident relationships would the part form up properly for me.

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Sam R @ Lon Eding on Sep 30, 2013 2:06 PM

thank you Lon;

can you tell me if I need to remove all of the arcs on the origional part? or just from the bend sketch? The former would be very challenging as you can see. I will try just removing arcs on the bend sketch first

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Lon Eding @ Sam R on Sep 30, 2013 2:21 PM

No arcs are allowed in the "Sketched Bend" sketch. Other sketches may have them. If you ever need arcs to figure out where your bend line needs to be, figure it out in an earlier sketch with construction lines and arcs, and then use the "Convert Entities" command to bring just the straight bend line into the "Sketched Bends" sketch.

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Matt Sparks @ Sam R on Oct 3, 2013 8:18 AM

Regards,

Matt

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Bernie Daraz @ Matt Sparks on Oct 3, 2013 8:35 AM

Matt,

I've done that too over the years, some customers would not allow it though. Some had appearance specs on the edges which forced us to the lasers on occasions as well. Some tumbled for a day to clean up requiring some holes to be reamed after that.

A trick I have used is use the nest to support the bent edge, though this part nest would 'trap' the part in the bend process. For that I just leave a note on the router to "use a .144 spacer on the backstop". That will allow a straight bend. We kept an out of tolerance set of gauge blocks on the shop floor just for that. The ".144" would be whatever is required to effect the bend correctly and of course, varies per job requirement.

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Sam R Oct 3, 2013 9:23 PM

Thank you so much for the replies. With your help I was able to resolve the problem

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11 Replies

Adrian Velazquez Sep 25, 2013 7:43 PM
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Correct Answer
Sam, your SketchBend (Sketch2) has excess geometry, just have the actual bend line and not all the extra reference geometry.
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- forum help.png72.9 KB
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- Sam R @ Adrian Velazquez on Sep 25, 2013 8:53 PM
  Mark Correct
  Correct Answer
  Thanks Adrian for the advice. You're right that excess geometry is often a problem that I've experienced before.
  But in this case, it hasn't affected the part at all. I removed or converted to construction lines everything but the bend line. However the features are still greyed out.
  Like • Show 0 Likes0
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  - Adrian Velazquez @ Sam R on Sep 25, 2013 11:54 PM
    Mark Correct
    Correct Answer
    Convert it to SheetMetal first (in the flat), then try the SketchBend Feature.
    Like • Show 0 Likes0
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Bernie Daraz Sep 25, 2013 8:58 PM
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I haven't done the sketch bend in a long while, I believe it cannot be a construction line. Also the part is not Sheet Metal yet, right?
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- Sam R @ Bernie Daraz on Sep 25, 2013 9:47 PM
  Mark Correct
  Correct Answer
  thanks. I do feel silly. My previous experience with 3D cad was that the file had to be sheet metal or not. But SW just converts it. My bend line is not a construction line, just the reference geometry which defines it.
  Once converted to sheet metal, the functions become accessible. However I get an error msg reading 'Sketch contains unsupported entities for this feature.' Given that there is only one line which isn't construction, I don't know what that would be referring to.
  Like • Show 0 Likes0
  Actions
Lon Eding Sep 26, 2013 8:21 AM
Mark Correct
Correct Answer
It definately does not like the arcs, regardless of whether they are construction or not. The SolidWorks Help file on Sketched Bends in the first bullet point says "Only lines are allowed in the sketch." Only after deleting all the arcs and attaching the line you dimension from to other geometry using coincident relationships would the part form up properly for me.
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- Sam R @ Lon Eding on Sep 30, 2013 2:06 PM
  Mark Correct
  Correct Answer
  thank you Lon;
  can you tell me if I need to remove all of the arcs on the origional part? or just from the bend sketch? The former would be very challenging as you can see. I will try just removing arcs on the bend sketch first
  Like • Show 0 Likes0
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  - Lon Eding @ Sam R on Sep 30, 2013 2:21 PM
    Mark Correct
    Correct Answer
    No arcs are allowed in the "Sketched Bend" sketch. Other sketches may have them. If you ever need arcs to figure out where your bend line needs to be, figure it out in an earlier sketch with construction lines and arcs, and then use the "Convert Entities" command to bring just the straight bend line into the "Sketched Bends" sketch.
    Like • Show 0 Likes0
    Actions
  - Matt Sparks @ Sam R on Oct 3, 2013 8:18 AM
    Unmark Correct
    Correct Answer
    Sam, I opened your model and made a new sketch (Sketch3). This is a little trick we use at our sheet metal shop to configure bend lines. It not only marks where to bend the part in our press breaks but helps the operator as there is no lay out needed. The cut is large enough for our laser to cut but small enough to not effect the part. This helps when you get into sketched bends as you can just select the center of both cut-extruded holes; making no need for construction lines in your sketched bend. Hopefully this helps. I have attached some images for reference.
    
    Regards,
    Matt
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    - Bernie Daraz @ Matt Sparks on Oct 3, 2013 8:35 AM
      Mark Correct
      Correct Answer
      Matt,
      
      I've done that too over the years, some customers would not allow it though. Some had appearance specs on the edges which forced us to the lasers on occasions as well. Some tumbled for a day to clean up requiring some holes to be reamed after that.
      
      A trick I have used is use the nest to support the bent edge, though this part nest would 'trap' the part in the bend process. For that I just leave a note on the router to "use a .144 spacer on the backstop". That will allow a straight bend. We kept an out of tolerance set of gauge blocks on the shop floor just for that. The ".144" would be whatever is required to effect the bend correctly and of course, varies per job requirement.
      Like • Show 0 Likes0
      Actions
Sam R Oct 3, 2013 9:23 PM
Mark Correct
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Thank you so much for the replies. With your help I was able to resolve the problem
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Looking for help with Sheet Metal bend

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