Hey guys, for some reason solidworks wont allow me to produce a flat pattern of a model i created through sheet metals. Ive never encountered this error before and dont know where i have gone wrong..
Any help is muchly appreciated.
Kind Regards Daniel Pratt
Edge Flange 3 is causing your problem. Either adjust where its bend begins, or adjust Edge-Flange 2.
Edit Edge Flange 2 & 3 and select trim side bends. Then the part unfolds fine.
I see your problem. The right hand view is zoomed in on the corner with the issue. This applies to the opposite corner as well. See the image below:
You have an edge that is shared between two bends. The common edge is only .0022 in long but SW will not allow any overlap of bend areas. You can get around this by using a corner relief or cutting away the problem area manually, or use one of the recommendations above.
Daniel,
Part of your problem is the way you have constructed your sheet metal model. In the screen shot below you will see that the flange position icon selected (material outside) is the one where your sketch locates the inside flange material coherent with your sketch line. This causes your bend to begin inside the adjacent bend.
If you select the flange position (bend outside) to begin the bend at your sketched line, this removes the edge that is shared by two bends.
By making this change in several of your blends, you will see that your model unfolds very well.
I have attached a modified model.
Stan
HERE IS A MODIFIED PART THAT WILL FLATTEN
My SW license is stuck in another computer rendering in photoview.
So I opened up your part in e-drawings, and to me it looks like your problem might be in the corners of this flange, see image. check if it isn´t there, otherwise you probably don´t need to wait long until someone else can have a look by opening it for you in SolidWorks.
Hope this