Hello All, I have part with two curves, please see attached which needs to be converted to sheet metal or flatten. how do I Flatten this part?
Thanks very much.
Gil,
Hello All, I have part with two curves, please see attached which needs to be converted to sheet metal or flatten. how do I Flatten this part?
Thanks very much.
Gil,
Gil... this is a double curvature shape, it can not be flattened unless you form it (stamp it). ...so, you would have to make it a formed part (from a formed feature) if you want it to be a sheetmetal part.... so much fun (sorry)
IF SW Corp would/could have a simple diagnostic to help users this...
I know everyone.. I'm not realistic.... it can only happen in our wildest dreams...... or, after they change the icons for color blind females?.............................
I see Paul is in good form tonight. "it can not be flattened unless you form it". I'll be scratching my head on that one for a while.
gil,,, You won't be able to convert this to sheet metal nor can you model it with the SW sheet metal tools. So,, if you do have "Surface Flatten" (SolidWorks Premium) you can use that to flatten it. I did that and was not happy with the results. I wasn't off by a whole lot but enough to bug me. What I did is offset your surface 1mm to the inside of the material (1mm) so I would flatten from what could be considered half a material thickness or a k-factor of .5 You might be better off to do a Face Curves and take measurements. Plot curves and layout the old fashioned way. You can compare it with my flattened surfaces.
Edit:.. Paul's reply is beginning to make sense now..
LOL!...funny, I had just opened this in Rhino3D to smash it flat.. and had the same conclusion.... the smashed shape does not add up..
Thank you all!
well, John is correct or at least he has something which is the closest way around this (the flat should be different for this, imho)... but I still can not get mine to flatten... I will ask him how he worked around this or did it and hopefully he can post his file?
I think you can use swept flange in sheet metal with minor modification to the sketch1
Convert to an open sketch, either inner or outer arc and rest of them to construction.
One end of the curve, modify to small straight length, tangent to the main arc
In the swept flange feature, select "Flatten along path" and add correct thickness
I am not sure, how far the flat pattern is true to the formed shape, but it works
I kept both original and flat pattern, for a visual comparison
See below
John,.. very interesting.. nice workaround.. although, that flat does not look right, imho..
I can make mine a sheetmetal part but I can not get it to flatten.. will attach how I'd go about using a sweep flange.. I tried in 2012 and 2016... can you post your file for us to see?
Paul,
I am not a sheet metal expert and the way I re-create the part may not be the perfect approach.
Here is the file
As I mentioned, I kept the original part as it is to compare
Hello John,.. we'll let Dennis be the expert, he has more sheetmetal knowledge than I.
yeah, that flatten is simpified (or conservative),.. it does not include the approx side trims and the arcs are also off... (still, nice workaround!)
I'll attach what I have to compare/overlay with the Rhino3D import using Squish (much better than Smash but still a approx flatten)
..maybe Dennis can compare/post with his new flatten?..
I then measured coord lengths and approx/overlayed my manual flatten sketch.. closer but still not exact.
(maybe I will try to splt the inside surface and outside to reduce the flatten approx).
Hi Paul,,, I was out at the pool relaxing and heard my name. I haven't looked at what you have yet but it should be interesting. Wanted to show what I had come up with a little earlier. John had got me thinking. My first thought was to do a swept flange on this but realized that the beginning arc and the ending arc were not the same radius. So I thought of sweeping it from the side like John did but was afraid I may be pursuing this to the gates of insanity and then hell so I dismissed that. Then after seeing Johns file I thought just maybe that might work. Unfortunately, as you know, the flat pattern does not come out correctly or as you might expect. So I did lay this out using face curves as a guide and this is what I came up with. I probably am wrong on the top and bottom radii. Still trying to figure that out. What are your thoughts?
I then extruded that and put it in an assembly in order to compare it to my "surface Flatten. I had mentioned earlier that I didn't like the results from that and now my fears are confirmed. I honestly didn't think it would be off by that much. Gonna be interesting to see what yours squish and or smash did. The magenta is my layout and the transparent is the flatten surfaces..
Edit:.... Actually the surface doesn't look that bad other than the overall vertical length. If I get the arc on the bottom correct it probably would match up better.
Your squish and my flatten appear to be an almost perfect match.
Hello Dennis.. ,.. (was just posting, here it is..squish=blue) agree, very close.. and,.. I noticed I had loose settings on Squish so, I changed the settings to rigid and preserve edges.. so, it not as close but still pretty close.
After reading more on Squish, it has it's limitations, just like the new Solidworks Flatten, they are not exact, only approximations.
And, the isoparm coord lengths from yours and my sketches confirm these are not exact but close.
Gil... this is a double curvature shape, it can not be flattened unless you form it (stamp it). ...so, you would have to make it a formed part (from a formed feature) if you want it to be a sheetmetal part.... so much fun (sorry)
IF SW Corp would/could have a simple diagnostic to help users this...
I know everyone.. I'm not realistic.... it can only happen in our wildest dreams...... or, after they change the icons for color blind females?.............................