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I find a Bug in weldment cutlist, same body shows different and incorrect length when patterned

Question asked by Charlie Fan on Aug 6, 2015
Latest reply on May 26, 2016 by Mark Greenwell

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As shown above, three posts on the right is patterned version of the left one.

The post is consisted of a cylindrical weldment structural member, and a block as pin top, which is extruded right on top of the post body.

We want the total length of the post, including the pin top, to be displayed as cutlist length automatically.

The result is interesting, the one on the very left worked just as we expected, however the ones on the right, which is patterned body, shows a wrong length. How can this be? it is exact pattern of the body, how can they have different length in Cutlist?

I also attached the part file so please kindly take a look and suggest some solution. This bug occurs in the 2015 sp4 as well.

Deepak Gupta Aug 7, 2015 8:58 AM

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I would treat this as a bug. It should be same for all bodies. Also they should be under same cut list and not different. Though there is a way out to get the correct length in this scenario just checked and found that the method is not working in this case.

See the reply in context

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Weldment.SLDPRT.zip76.8 KB

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Glenn Schroeder Aug 7, 2015 8:26 AM
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I don't know if I'd qualify that as a bug or not. You're trying to combine bodies created with the Structural Member function and a Boss-Extrude, and expect the cut list properties to be accurate. They don't work that way. The first cut list item is giving the length of the first Structural Member only, even though it was combined with the Boss-Extrude. The other three are showing the length for the combined patterned bodies. As an alternative workflow I'd suggest using the Structural Member function to create the full length of material needed, then use an Extruded Cut to remove the unwanted material.

And if you don't mind a little unsolicited advice, I'd highly recommend you start fully defining your sketches. If you don't I can almost guarantee you'll get unwanted results at some point.
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- Dennis Bacon @ Glenn Schroeder on Aug 7, 2015 8:30 AM
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  I agree Glenn. To me that is expected behavior.
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- Charlie Fan @ Glenn Schroeder on Aug 7, 2015 9:09 AM
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  Glenn, I tried revolve cut. It also has error. we just want the cone shape pin top. How to achieve that in extrude cut???
  
  Can you just have a bit more try please?
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  - Deepak Gupta @ Charlie Fan on Aug 7, 2015 9:20 AM
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    You could add a chamfer to get the cone shape pin top. But this would also result in same error of length.
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    - Charlie Fan @ Deepak Gupta on Aug 7, 2015 9:26 AM
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      Yes, revolving and revolving cut, they all get wrong result when patterning. I just don't understand why this has never been discovered before. If this problem can be fixed, people will be able to make any shape structural member(no longer just tubes) and still got the right cut length, it is important that they fix it.
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      - Deepak Gupta @ Charlie Fan on Aug 7, 2015 9:33 AM
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        There are few SPR on similar issue i.e. wrong length. So please report this to your VAR and let them take care of it.
        
        For you to get the correct length displayed, use the bounding box.
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  - Glenn Schroeder @ Charlie Fan on Aug 7, 2015 9:31 AM
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    To get the shape you had originally, just edit the sketch for your Structural Shape to the total needed length. Then delete your Boss-Extrude, but don't delete the sketch. Edit it, adding a circle that's co-radial with the outside diameter (the Convert Entities sketch will do that for you). Now use this sketch for an Extruded Cut.
    
    Charlie Fan:
    
    Glenn, I tried revolve cut. It also has error. we just want the cone shape pin top. How to achieve that in extrude cut???
    
    Can you just have a bit more try please?
    
    If you do want a cone shape instead of the rectangular shape, that will need to be a Revolved Cut. The first screenshot below shows the sketch used. To get the cut to work you'll probably need to have the upper left sketch point a tiny fraction away from the centerline (0.0001 would be enough). I'd attach my model, but I'm using SW2015, and you wouldn't be able to open it.
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    - Charlie Fan @ Glenn Schroeder on Aug 7, 2015 9:35 AM
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      Hi Glen,
      
      Everybody knows how to get the cone on the post!!!
      
      It will still get the wrong cut length, can't you just try it a bit more???? pattern your body and take a look and see what happens.
      
      I ALREADY TOLD YOU THIS ALSO HAPPENS IN SOLIDWORKS 2015 SP4. HOW CAN'T I OPEN YOUR FILE?
      
      Please kindly read my post carefully, I BEG YOU PLEASE!!!!!!!
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      - Glenn Schroeder @ Charlie Fan on Aug 7, 2015 9:56 AM
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        Okay, I have several apologies to make. I assumed that using an extruded cut to remove material would solve the problem, but it doesn't. Apparently there is a bug. I even tried patterning the Structural Shape first, then creating the extruded cut, then patterning it. That produced the same results.
        
        I do see that you said it was also happening with SW2015, but the Older Version warning icon threw me off.
        
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- Charlie Fan @ Glenn Schroeder on Aug 7, 2015 9:17 AM
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  Hi Glenn, The first cutlist item is the correct length of the entire post, which is 650;
  
  The second cutlist item is the wrong length only include the cylinder which is 600, it forgets the pin top.
  
  It is not what you have written, can you change your answer a bit?
  
  Please notice the three on the right is EXACT BODY PATTERN of the left post, since they are the same body, how can they have different cut length???
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Deepak Gupta Aug 7, 2015 8:58 AM
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I would treat this as a bug. It should be same for all bodies. Also they should be under same cut list and not different. Though there is a way out to get the correct length in this scenario just checked and found that the method is not working in this case.
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Dennis Bacon Aug 7, 2015 11:40 AM
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I'm sure there is a good reason for wanting to pattern the structural member but of course you could pattern the sketch then add your structural members then do your cut revolves, bosses, or chamfers. The cut list evaluates correctly then. With only one cut-list
Edit: Looks like it only works with the chamfer. I give up.
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Scott Harvey Aug 7, 2015 4:07 PM
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I feel like you are not using the weldment tool the way it was designed for. I don't understand what your trying to build in this part file but it looks like your making an assembly not a weldment. However it got the first length right so the programming is in there and probably could be tweaked.

In 2015 and above, with "Automatically create cut lists" turned off select all 4 bodies in your cut list after the pattern and choose make cut list item. Problem solved. Sometimes SW doesn't guess right. Probably why they made this enhancement in 2015 because the coding may be too difficult. Who knows.
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- Deepak Gupta @ Scott Harvey on Aug 7, 2015 4:45 PM
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  Scott agree with you but I would still treat this as a bug.
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Lulu Tanase May 26, 2016 7:57 AM
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I've found this bug, too.
The length of a mirrored chamfered body is miss-reported. It is shortened with the length of the chamfer (cutlist items 9 and 10).
(Solidworks 2015).

If I suppress the chamfer, the error disappears.
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- 3139275.SLDPRT.zip335.7 KB
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Mark Greenwell May 26, 2016 9:30 AM
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Charlie,

This is how I have done it, Using normal feature I extruded the tube 600mm long then, combined bodies with another sketch for the top piece.

I then went into the Weldments environment and converted into a weldment ( just clicked the weldment icon).
Then I added the bounding box,

This now gives me 4 parts all the same size and the cut list length in the drawing is correct (although you would have to edit the info as it shows made from plate).

Not exactly the way you wanted but another option.

Regards

Mark (SolidWorks 2016 sp3)
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