Hi there,
When I'm trying to flatten my ellipse models in sheetmetal it won't work. Is there a solution for this problem or is solidworks just not able to unfold or flatten ellipses?
Thanks.
Hi there,
When I'm trying to flatten my ellipse models in sheetmetal it won't work. Is there a solution for this problem or is solidworks just not able to unfold or flatten ellipses?
Thanks.
If it's of a solidworks part file it is not possible. If it's of a sheet metal file it is possible.
Thanks and Regards
Venkatesh S
Application Engineer
E G S Computers India Pvt. Ltd.
http://www.egsindia.com | http://www.egs.co.in | http://www.egsindia.blogspot.in
If you develop your sheet metal with a square shape then unfold and cut your shape then refold it will work for you, could you upload the part ?
Hi there John, Thanks for your help.
Sometimes I'm succeeding while flattern ellipses. But while trying with a simple ellipse base flange extrude the feature won't listen. I have the same problem making a swept flange with an ellipse functioning as my guide line. When I try this I get an error that says i only can use lines an regular arcs.
The uploaded part contains the swept flange error.
This upload contains the base flange flatten error
You only need one sketch for the shape, the circle and the line must be tangent
Thanks for your response John.
But when I'm trying to use the swept flange with an ellipse it won't work. And this is the exact guideline form I need.
If you make these pieces , you need to use sheet metal extension.
For example:
To make a dog mouth between two pipes.
First you make the model of the two pipes.
Secund you make the intersection between the pipes.
final piece you can to use for assembly template between two pipes.
Hi there Miguel,
Thanks for your response. I can't quite understand what you mean. Is the sheet metal extension a feature, or is it something else? And what is a dog mouth? I'm sorry i hope these extra question won't cause too much inconvenience.
dog mouth - intersection between two pipes.
I'm not sure what you mean by ellipse. I could't find one in your model. John is correct - For your profile you should have one sketch (make sure it has a tangent relation) and get rid of your base flange.
I have attached an assembly file consisting of your file and your file modified laid on top of each other so you can see there is no difference. In the _db file I suppressed your base flange and added a tangent line to the profile. Flattens like it should.
Samson is using an educational copy, therefore he can't open it, you could upload pictures ...
I didn't know that you can't open a SW file with educational. I did originally open it with 2015 and noticed it was an older version. Opened it in 2014 and it did not indicate older version. Samson, only lines and arcs can be use for the profile. If it would work with ellipses and splines it would be wonderful. Oh Well...
You can sketch a series of tangent arcs around an ellipse. I'm not sure if you want the profile or the path to be elliptical, or, maybe both.
Thank you very much Dennis. I'm able to open your solidwork files by the way. To bad that solidworks won't allow us to use an ellipse sketch as a guideline or profile. I want to use my ellipse sketch for my path. It's kind of hard thought to make the ellipse existing out of single arc lines. Could you maybe upload your last file, so I can check out your arc (ellipse) sketches? Thanks for helping me out.
I think this is going to be a problem for me. I can't get my series of arc lines that exact that I can call it an ellipse. Maybe someone has a solution for this.
You can use an ellipse and make it a construction line and the draw straight lines that somewhat follow the ellipse then add a large enough radius so you don't see the straight lines.
Follow what Dennis did
thanks for helping me out john!
On the attached file I sketched the ellipse then made it construction. Started with a 3 point arc coincident at 3 points with the construction geometry ellipse. Then used tangent arcs from there. You just sketch the arcs and drag the end around until you get an almost perfect match with your ellipse, accept that and start another tangent arc. This is fairly easy and as you see it becomes an almost perfect match to your ellipse. Also by changing the size of the ellipse your arcs will change with it.
You changed things up a bit Samson.. Used a Lofted Bend. Nice job. It works well. I sketched an ellipse in and you aren't off by much. I would suggest adding the ellipse in - make it construction - and making your arc points coincident with it.
thank for all the help Dennis!!
You can sketch a series of tangent arcs around an ellipse. I'm not sure if you want the profile or the path to be elliptical, or, maybe both.