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Flat Pattern not working properly

Question asked by Thomas Warner on Sep 16, 2014
Latest reply on May 23, 2019 by K. M.

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When populating my drawing with views,the flat pattern does not unfold.

I have had this issue with SW 2014.Checked the Property manager,and it shows the flat pattern as the selected view.

Still,all the rebuilding and control q I try no unfolding is performed.Open the part and it unfolds fine.

If I leave it in the flat pattern,my formed views are incorrect???? It is designed in a top down assy that has many other references,so leaving it unfolded disrupts the design intent.

Anyone else have this problem with SW 2014 SP2?

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Roland Schwarz Sep 16, 2014 9:33 AM
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Try making your own flat pattern configuration and using that in your flat views.

There is a difference between "Unfold" and "Flat Pattern". Sometimes an Unfold feature will work but the Flat Pattern will have difficulty. Be sure to check the actual Flat Pattern feature by unsuppressing it in the model.
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- Thomas Warner @ Roland Schwarz on Sep 16, 2014 9:48 AM
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  Thanks Roland,
  But it just seems like a huge amount of un-needed work. The model flattens fine,using both the flatten command,and suppressing the flat pattern feature in the tree.
  The assy contains 11 parts that will all need to have their own unfolded configuration added?Come on Solid Works.!
  I have had this issue with SW 2014 and have yet to make sheet metal work well in SW 2014 drawings. Unpredictable as to what I will get from my next model.
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  - Thomas Warner @ Thomas Warner on Sep 16, 2014 10:14 AM
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    Ok I went thru all the added exercise of adding a configuation,unfolding the part using the unfold command,and the view in the drawing has lines from the bends,instead of a nice flat part as it should. This type of view when converted for CNC g-code produces many short little lines that leave burn marks from being laser cut,IE stop and starts in the cut path.
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    - Ian Worrall @ Thomas Warner on Sep 16, 2014 10:17 AM
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      Try RMB on the drawing view & select "Tangent Edges" > "Removed"
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    - Jan Forkovic @ Thomas Warner on Sep 16, 2014 1:18 PM
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      Hi
      Try to use merge faces.
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      merge faces.jpg525.4 KB
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    - Rushabh Shah @ Thomas Warner on Sep 16, 2014 1:49 PM
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      if possible, and if you dont mind, than upload your solidworks files. might get your answers. as i have been working a lot on sheet metal, and face a lot of problems, especially for multi-sheet metal (even different thicknesses) into single part file.
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Tyler Hamm Sep 16, 2014 11:26 AM
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I'm assuming that you chose this when you added your flat pattern view in your drawing.
Make sure the drawing added this configuration when you selected the flat pattern view.
Then, double check that the flat pattern feature and the flatten features are unsuppressed in the feature tree of the Flat Pattern configuration.
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Jody Holm Sep 17, 2014 8:59 AM
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Yes. This is a bunch of crap! Suppress this, unsuppress that, make your own configuration, make a macro. Come on solidworks, just because you put an icon on the interface doesn't mean your done. IT HAS TO WORK! Tom, I am suddenly having the same problem. My flat pattern view was correct until I made a couple changes to the part (none to the bends) and now I can't get it to unfold in the drawing. The part unfolds in the model as yours does. If I try to re-drag the view into the drawing the "flat pattern" view now shows up folded in the view pallete. Very irritating.
Now, because I am pressed for time, I'm going to have to save the part under a new name and bring that new model in, unfolded, so I don't screw up the rest of the folded views. This is sloppy and non-associative and definatly the wrong way to do it! Hopefully somebody has the real answer to this problem and not some cobble job work around.
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- Thomas Warner @ Jody Holm on Sep 17, 2014 10:12 AM
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  As I would agree,sheet metal functionality has degraded in SW 2014,added features that should populate in the flattened/un-folded state remain at the end of the feature tree instead of modeling into the flat state. The problem I encountered with flat pattern not portraying properly in drawings was after a revision to the part also Jody.
  I have battled this many times and just finally had to ask(Hey guys,What am I missing here?) So close all assy's with references,open and flatten part,drop into a drawing,and all other views are incorrect now,and all the detailing and dimensioning work I have done is wasted. So make a new part file,inset part,break refs,and create a new part.Flatten and insert into drawing. If I revise my part,the flattened state will not reflect any changes made.Its maddening and quite dis-appointing. I have my work arounds for it.As we all do for certain other maladies in modeling software glitches. I am just hoping for some improvements in Sheet metal from SW 2015! After 20,000 hours behind the mouse,modeling in SW I just had finally had enough and came to the masses with my anguish!
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Tyler Hamm Sep 18, 2014 4:39 PM
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I've blown up many drawings using the DefaultSM-FLAT-PATTERN configuration to make changes in my models and then not making sure that the configuration is flattened.
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Jim West May 29, 2015 3:00 PM
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I just had and solved this problem. One of the Edge-Flanges I was adding for some reason had supressed elements inside the Edge-Flange feature. When I unsupressed these features the whole part started unfolding correctly.
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- John Stoltzfus @ Jim West on May 29, 2015 3:02 PM
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  Another thing that seemed to take care of it for me in the older versions and I would still bring the part in the drawing the same way and that is......
  
  Select all the views in the drawing view dialog box, Prior to selecting the Flat Pattern view
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Dennis Bacon May 31, 2015 9:57 PM
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I understand your anguish Thomas (wonder if you are still following this post). Looks like Jim and John are keeping this alive. I bet the guy who wrote the code for this went bonkers. I managed to do this without issues although I can see how they can occur especially in a top down. The view below is multi body sheet metal part. As far as the tangent lines in your drawing I would say remove them (a previous post indicated how to do that in drawing and by merging faces in part). Show sketches (from the view menu) if you want to show the bend line. The tangent lines are not included in the exported part (at least with the cad-cam software I have used. They probably do if exported to dxf. Personally I can't understand why anyone would want a flat pattern drawing but I suppose people have their reasons. If you set your flat pattern to simplify bends you won't get the splines or polylines in the bend area. Even with splines that convert to short lines, with any laser produced in the past 15 years you should not get burn marks providing the conditions are correct. It will just take a couple of seconds more per part like these to cut. Also most cad-cam software today has the ability to smooth the lines out into a couple of arcs (or more) automatically.

I had nothing better to do
Also, all dimension changes can be easily be done by altering the Layout Sketch. This updates all the parts and flat patterns at the same time. Of course any holes can be added, altered etc without unfolding the parts. No drawing issues!
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Kevin Peters Sep 9, 2015 8:53 AM
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I had this same problem and figured out what happened. The flat pattern feature became suppressed in the flat pattern configuration.

How to fix:
1) In the 3D model expand the Flat-Pattern feature
2) Right click the sub-feature labeled Flat-Pattern#
3) Select configure feature
4) Uncheck the box next to DefaultSM-FLAT-PATTERN
5) Hit apply and then ok
6) Save

The flat pattern view should now appear correctly on your drawing.
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- Jason Radcliff @ Kevin Peters on Dec 8, 2015 8:02 AM
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  This fixed it for me but how in the hell do these get changed!! all I did is went in on my base face and changed the width come back and rebuild and then had this issue. I am good now.
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- Tristan Pashley @ Kevin Peters on Mar 15, 2016 4:25 PM
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  That did it! Thank you so much!
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- Matthew Watts @ Kevin Peters on Jul 11, 2018 8:29 AM
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  Kevin,
  I had to go through a lot of threads before finding your technique, but it worked where every other one would not. So I just wanted to thank you for that!!
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- K. M. @ Kevin Peters on May 23, 2019 10:06 AM
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  Thanks for this! You solved this problem for me even now. Additionally, I had to un-check all of the boxes in that window. (see attached pictures)
  
  "Solidworks sheetmetal flat pattern not flat" is what I searched to find this thread, so hopefully adding that will make it easier for future users to find.
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Daniel Feldstein Dec 30, 2015 1:17 PM
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I've been having to learn how to build my sheet metal parts in ways that bend lines aren't interfered with in solidworks... interferences which do work in real life, but if I try to unfold on solidworks I get interference messages but it won't highlight in the drawing where the problem is. It tells me which bend line but not where along that bend line the issue is... I'm curious to know if 2016 has better information on where the problems are along a bend line when the model will not unfold. I do complex sheet metal designs so this has become a pretty time consuming problem.
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Bernie Daraz Dec 30, 2015 8:36 PM
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Thomas,

That is a one piece item to me. No way would I tie up the welders with all that welding and fixturing. One flat face at the top, 5 top flange bends, 5 bottom flange bends. Making all those parts to save on the scrap just adds value to the scrap.
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- Thomas Warner @ Bernie Daraz on Dec 31, 2015 9:08 AM
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  Thanks for the input Bernie. I made the assy as it is for simplicity at the brake press. No welding or fixturing. The bolts lineup all the components.It is an eleven pc. assy actually, fitted with felt runners and rubber to absorb shock to avoid breaking the glass. You see, it is a window frame for an ATV, with 1 fixed glass and 1 sliding glass window. Only 2 like it in the whole world. RH and LH.
  Made for a friend who broke out his glass on a hunting trip!
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  - Bernie Daraz @ Thomas Warner on Dec 31, 2015 11:53 AM
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    Thanks Thomas! Us production guys forget that sometimes we only make one or two! Happy New Year!
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Mahinder Dhahari Jan 3, 2016 7:49 AM
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Add BEND ALLOWENCE K Fector
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