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Flattening sheet metal parts made with edge flanges

Question asked by Kenneth D'Angelo on Oct 11, 2011
Latest reply on Aug 29, 2012 by Ausdell Hadaway

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I have a simple u-shaped part made with a sheet metal base flange and two edge flanges. When I flatten the part it gives a length of 64.589mm. If I make a part with the exact same profile made from an extruded part converted to sheet metal it gives a flattened length of 79.594mm, which is the correct length.

Looking in the knowledge base, S-017112 describes the same problem (2007) and the answer given is incorrect:

Answer:

Flat pattern length is calculated by - < All flat portions length>+<bend allowance for each bend>. Do not consider the original length of the flanges since the bend radius portion length is also included in the length mentioned in the flange feature.

This is incorrect because it does not consider the centerline length of the bend radius. The part comes out way too short.

In the attached files is an assembly with two identical parts on top of each other. When they are flattened, they are no longer identical.

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Deepak Gupta Oct 12, 2011 12:10 AM

Welcome to SolidWorks forums Kenneth.

Quick question: What is the K factor as it'll play a major role in calculating the flat length.. Do a manual calculations and verify.

You might also find this post helpful for your future reference

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Wayne Tiffany Oct 12, 2011 9:30 AM

The 001014 part is the wrong one and it's because you have a custom bend allowance set for each of the bends. Go to the bottom of the PM and uncheck the box and let the k-factor control the bends. Then you get the same flat as the other part.

Now, might I ask why you are overriding the radius and bend allowance on each of the bends instead of setting the default in the Sheet-Metal1 feature and letting that propagate throughout? Even in the Part2 file you made the base geometry with one radius and then forced it to change later.

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Ausdell Hadaway Aug 29, 2012 2:56 PM

Hi Kenneth,

First off, let me say that the two models aren't quite actually identical, namely the inside radius of one is 3.175mm while the other is 3.180mm and the flange lengts were also off slightly as well. Nevertheless, the major issue is with the difference in bend allowance that you have chosen for both parts.

Given the two flat lengths, 79.594mm is more correct. As Wayne mentioned, pt#001014 is wrong because you have a custom bend allowance. You should note that SW doesn't care about the values you enter for bend allowance when the part is in the bent state. Instead, the geometry of the bent shape you see in the graphics is generated based on the flange length and bend radius values/options you entered for the bend.

However, when you ask SolidWorks to generate a flat pattern from the bent shape, the values you enter for bend allowance then do come into play. SW essentiall adds all the flat segments (those up to the bend lines) to all the bend allowance you defined for each bend to generate the flat pattern.

I made the bend radius and flange lengths for both parts identical so that we can properly compare the results. I will note that there is still a slight difference 19.380 vs. 19.377 for the middle segment (there is something else slightly off between the geometry of both parts). Nonetheless, the images attached should help clear up what SW does using the values you inputted for the bend allowance.

Hope this helps clear things up.

AMH

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Deepak Gupta Oct 12, 2011 12:10 AM
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Welcome to SolidWorks forums Kenneth.

Quick question: What is the K factor as it'll play a major role in calculating the flat length.. Do a manual calculations and verify.

You might also find this post helpful for your future reference
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Wayne Tiffany Oct 12, 2011 9:30 AM
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The 001014 part is the wrong one and it's because you have a custom bend allowance set for each of the bends. Go to the bottom of the PM and uncheck the box and let the k-factor control the bends. Then you get the same flat as the other part.

Now, might I ask why you are overriding the radius and bend allowance on each of the bends instead of setting the default in the Sheet-Metal1 feature and letting that propagate throughout? Even in the Part2 file you made the base geometry with one radius and then forced it to change later.

WT
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Ausdell Hadaway Aug 29, 2012 2:56 PM
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Hi Kenneth,

First off, let me say that the two models aren't quite actually identical, namely the inside radius of one is 3.175mm while the other is 3.180mm and the flange lengts were also off slightly as well. Nevertheless, the major issue is with the difference in bend allowance that you have chosen for both parts.

Given the two flat lengths, 79.594mm is more correct. As Wayne mentioned, pt#001014 is wrong because you have a custom bend allowance. You should note that SW doesn't care about the values you enter for bend allowance when the part is in the bent state. Instead, the geometry of the bent shape you see in the graphics is generated based on the flange length and bend radius values/options you entered for the bend.

However, when you ask SolidWorks to generate a flat pattern from the bent shape, the values you enter for bend allowance then do come into play. SW essentiall adds all the flat segments (those up to the bend lines) to all the bend allowance you defined for each bend to generate the flat pattern.

I made the bend radius and flange lengths for both parts identical so that we can properly compare the results. I will note that there is still a slight difference 19.380 vs. 19.377 for the middle segment (there is something else slightly off between the geometry of both parts). Nonetheless, the images attached should help clear up what SW does using the values you inputted for the bend allowance.

Hope this helps clear things up.

AMH
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Flattening sheet metal parts made with edge flanges

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