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lofted sheet metal

Question asked by Tony Schaffner on Jan 20, 2016
Latest reply on Jan 22, 2016 by Tony Schaffner

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Hello All,

I am looking for some help with the attached part. It is a lofted sheetmetal part and I cannot get one of the bend lines to take so to speak. I have an equal amount of vertices and as far as I can tell I have done everything properly but I cannot for the life of me get the last form line to generate. This is causing none of my bend lines to show when projecting a flat pattern.

I have been on this part for the past 10 hours and would surely appreciate any help you all can offer.

Thank you in advance,

Tony

Dennis Bacon Jan 21, 2016 5:29 PM

Correct Answer

I think I have this figured out Tony... The reason the bend lines weren't showing in your file is there is a twist in two areas of the loft. Non planer surfaces. What I did in my attached file is deleted some of your in-context relations in your profile (on one end) and made parallel relations to the corresponding lines on the opposite end profile. This altered the geometry slightly in two areas. See screenshot. Everything else matches up perfectly. I have attached an assembly file with 3 parts. Your original (not altered), An altered "formed" and an altered "bent". The altered "formed" has a Loft minimum (that's what SW does on formed lofts) of 2 bend lines for each bend. I suspect you could put the bend line midway between them. The one done with the bent option just has a single line per bend and no reliefs as in the previous one. In the screenshot the original is grey, Altered formed is rust and the altered bent is yellow.

I think this is what you were hoping to see.

See the reply in context

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L-0000077-002-1.SLDPRT.zip483.9 KB

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Dennis Bacon Jan 21, 2016 9:38 AM

Tony... If you can get away with it you might want to used the "bent" option on the loft. In order to do this I had to delete all your sketch fillets and do a trim corner (connected the lines). I still could not get the bent option available even after deleting the loft so I put your sketches in a new part and was able to start a new loft with the bent and formed options available. There are some reliefs cut into it which I am sure is undesirable. I don't have time to put any more thought into this at the moment (be back in about 5 hours) but hopefully you can get some ideas. I have attached an assembly file of your orig file and my new file together so you can see there is little or no difference. I think the issue is the bend radii in your file are not measurable and the bend lines cannot be developed because of that.

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L-0000077-002-1 New_db.zip967.5 KB

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Tony Schaffner @ Dennis Bacon on Jan 21, 2016 11:18 AM

Dennis,

Thank you so, so much. I spent all day trying to figure this out.

I am however still trying to understand why it has five bend lines as opposed to three where it makes its transition from rounded to flat. I am guessing that its because its not possible to get the correct "overall" angles with 3 breaks. Does that make sense to you?

Regards,

Tony

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Dennis Bacon @ Tony Schaffner on Jan 21, 2016 5:29 PM

I think this is what you were hoping to see.

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L-0000077-002-1-Newer_db.zip1.2 MB

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Tony Schaffner @ Dennis Bacon on Jan 24, 2016 12:48 AM

Dennis,

This is exactly what I was going for and I now understand why I was having the issue. I went back and did it again from scratch just to be sure i understood what you were saying and the "twist" was the problem for sure. I added the parallel constraints as you did and bingo!

Thank you very much for your help on this. This is my first time using the forum and I will most definitely be back in the future.

Thanks again,

Tony

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John Stoltzfus Jan 21, 2016 1:31 PM

Like you mentioned - one of the main factors in lofting is to have the same amount of points per sketch, also each place where the sketches meet they need a radius, and what I always did is use my bend radius, the only thing you need to adjust is the offset for the material thickness etc...

You should be able to tell SW how many bends you need...

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John Stoltzfus Jan 21, 2016 1:55 PM

Here is a part you can check - I couldn't open your file to diagnose it - but when I recreated it using your model, I did an incontext part creation and the one side there was a spline line instead of a sketch line, not sure if it would show up in your sketch or not. Lofting doesn't do well with splines, when it reduces the amount of points from sketch to sketch...

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Part2.SLDPRT.zip393.8 KB

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6 Replies

Dennis Bacon Jan 21, 2016 9:38 AM
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Correct Answer
Tony... If you can get away with it you might want to used the "bent" option on the loft. In order to do this I had to delete all your sketch fillets and do a trim corner (connected the lines). I still could not get the bent option available even after deleting the loft so I put your sketches in a new part and was able to start a new loft with the bent and formed options available. There are some reliefs cut into it which I am sure is undesirable. I don't have time to put any more thought into this at the moment (be back in about 5 hours) but hopefully you can get some ideas. I have attached an assembly file of your orig file and my new file together so you can see there is little or no difference. I think the issue is the bend radii in your file are not measurable and the bend lines cannot be developed because of that.
Attachments
- L-0000077-002-1 New_db.zip967.5 KB
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- Tony Schaffner @ Dennis Bacon on Jan 21, 2016 11:18 AM
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  Correct Answer
  Dennis,
  
  Thank you so, so much. I spent all day trying to figure this out.
  I am however still trying to understand why it has five bend lines as opposed to three where it makes its transition from rounded to flat. I am guessing that its because its not possible to get the correct "overall" angles with 3 breaks. Does that make sense to you?
  
  Regards,
  
  Tony
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  - Dennis Bacon @ Tony Schaffner on Jan 21, 2016 5:29 PM
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    Correct Answer
    I think I have this figured out Tony... The reason the bend lines weren't showing in your file is there is a twist in two areas of the loft. Non planer surfaces. What I did in my attached file is deleted some of your in-context relations in your profile (on one end) and made parallel relations to the corresponding lines on the opposite end profile. This altered the geometry slightly in two areas. See screenshot. Everything else matches up perfectly. I have attached an assembly file with 3 parts. Your original (not altered), An altered "formed" and an altered "bent". The altered "formed" has a Loft minimum (that's what SW does on formed lofts) of 2 bend lines for each bend. I suspect you could put the bend line midway between them. The one done with the bent option just has a single line per bend and no reliefs as in the previous one. In the screenshot the original is grey, Altered formed is rust and the altered bent is yellow.
    I think this is what you were hoping to see.
    Attachments
    L-0000077-002-1-Newer_db.zip1.2 MB
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    - Tony Schaffner @ Dennis Bacon on Jan 24, 2016 12:48 AM
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      Correct Answer
      Dennis,
      
      This is exactly what I was going for and I now understand why I was having the issue. I went back and did it again from scratch just to be sure i understood what you were saying and the "twist" was the problem for sure. I added the parallel constraints as you did and bingo!
      
      Thank you very much for your help on this. This is my first time using the forum and I will most definitely be back in the future.
      
      Thanks again,
      
      Tony
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John Stoltzfus Jan 21, 2016 1:31 PM
Mark Correct
Correct Answer
Like you mentioned - one of the main factors in lofting is to have the same amount of points per sketch, also each place where the sketches meet they need a radius, and what I always did is use my bend radius, the only thing you need to adjust is the offset for the material thickness etc...

You should be able to tell SW how many bends you need...
Like • Show 0 Likes0
Actions
John Stoltzfus Jan 21, 2016 1:55 PM
Mark Correct
Correct Answer
Here is a part you can check - I couldn't open your file to diagnose it - but when I recreated it using your model, I did an incontext part creation and the one side there was a spline line instead of a sketch line, not sure if it would show up in your sketch or not. Lofting doesn't do well with splines, when it reduces the amount of points from sketch to sketch...
Attachments
- Part2.SLDPRT.zip393.8 KB
Like • Show 0 Likes0
Actions

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