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Cut on Reducer not showing correct on flat pattern.

Question asked by Manindra Singh on Oct 2, 2017
Latest reply on Oct 4, 2017 by Frank Ruepp
  • Comment • 12

Hello, i am creating Y duct piece. It have cut on it, but after opening it flat both cut have different shape.

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as you can see in above image, cut on both side have different shape.If you do unfold command its show both cut shape same.

I have designed same type parts with different dimensions, they didn't had this problem.

I have also attached model file. If there is problem with modelling , please tell me.

Frank Ruepp
Frank Ruepp Employee Oct 4, 2017 5:15 AM
Correct Answer

Hi Manindra, Hi Dennis, Hi John,

 

I had a look at the model and I tend to agree that the behaviour of this sheet metal part is something to report to our Support Team.  I can't see a reason why a symmetrical folded part turns out with an asymmetric flat pattern.

But I would like to add a few comments:

  1. This part seems to be a legacy part that was created with SOLIDWORKS earlier than 2013 since we did a major architectural overhaul with SOLIDWORKS 2013.  This overhaul had become necessary since we cleaned up some issues we were eyperiencing with the initial implementation of multi body sheet metal.  So I strongly recommend to create new (sheet metal) templates and use those for new sheet metal parts so that the new architecture gets used rather than copying old files with possible issues.  You can identify old and new architecture by the features in the tree:
    Old parts have several independent sheet metal definitions and several flat patterns in the tree:
    Whereas new architecture parts have a common sheet metal definition nodes and flat pattern nodes in the tree:
  2. I don't want to blame the issue you are seeing on some architectural changes we did in the past but when I create your sheet metal body from scratch with the new architecture I am not seeing the asymmetric flat pattern (checkout the green body):




  3. Personally I don't like the formed lofted bend feature for geometry that can be created by using ordinary sheet metal features since the formed lofted bend algorithm is different from the ordinary math we are using in order to determine the flat pattern geometry.  Means for ordinary sheet metal parts we are using simple math (linear and circular entities are added up) to calculate the flat pattern in opposite to the formed lofted bend algorithm where we are "approximating" the flat pattern geometry (please don't take "approximating" literal since usually the differences between folded and flat body are usually insignificant (in case of a cone there is actually no difference at all since we do not offer the bend deviation command on the flat pattern).  Therefore I have created a second sheet metal body with a regular cone and the Insert Bend feature (which I personally like a lot since it is the first sheet metal feature ever available in SOLIDWORKS and therefore usually works very reliable as long as you follow some sheet metal guidelines).  Please check out the gray body in its folded and flat pattern state:


    Way back before there was base flange or lofted bend you would have to create your sheet metal tubes or cones like this.
  4. With regards to Dennis' question I am not sure what the difference between unfolded and flat pattern is.  But obviously there is some difference between both features since in some cases you can unfold some sheet metal bodies which cannot be "flat patterned".  In the past I have stumbled over some rare cases where you could unfold the sheet metal body but could not get a flat pattern feature to work.  In those cases I also used a manual configuration where the part was unfolded in order to display the flattened state.

 

I have attached my part in 2016 format in order to comprehend my steps.

 

Kind regards

Frank

SOLIDWORKS Product Definition Team

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