Can this be done in SolidWorks?

"John" a écrit dans le message de news: Xns998163096F2DEabrahamnonecom@212.242.40.196...

yes.

"Jean Marc" wrote in news:46b2e9cb$0$29155 $ snipped-for-privacy@news.free.fr:

Hi Jean,

Basically what I do is:

Base-flange/tab. then I select a plan. Tools > Sketch tools > sketch picture. Here I open picture of a guitar to use as referrence. Then using Spline I outline an M like shape (only one side of the guitar), fix relations and exit sketch.

Finally using Features > Extrude Boss/Base I give it a thickness of 2mm and hieght of 150mm.

Now how do I flatten it? The Flatten button is disabled.

Thanks, John

Suppress the last feature.

TOP

Use the Insert> Sheet Metal> Base-Flange feature instead of an extrude to create. (If you selected the Base-Flange feature before sketching, you should be able to click the "I'm done sketching" icon in the confirmation corner and the Base-Flange interface should interface should reappear in the property manager.) Then you can unsuppress the Flat-Pattern feature to see the part in flattened form.

"Abraham" a écrit dans le message de news: Xns998174C74D8C1abrahamnonecom@212.242.40.196...

If you use this method, you have to insert bends first.

Then 3 or 4 new features are added: sheet metal / unfold/ fold/ ... If you suppress the "fold", then you have your flat.

There are 2 ways to make sheet metal: one where you decide first it's S.M., and one where you insert the features at the end. You should be able to find example of both on the net. Not hard to figure out when you have an example.

Good luck, it's vacation time for me.

JM

"Jean Marc" a écrit dans le message de news:

Meant before being able to flatten. In this case the S.M features are at the end.

engr-D wrote in news:1186139579.792513.106260 @g4g2000hsf.googlegroups.com:

When I click "I'm done" It says "The sketch contains an entity with unsuitable geometry".

However if I use something else (i.e. 3 Point Arc) instead of Spline it goes well and as you said I can flatten it.

Thanks, John

Have you tried using a lofted bend? Sketch the profile on the Top Plane (for example). Then create a plane more than your 150mm above and parallel to the Top Plane. Duplicate the curve on the new plane and loft between them. You can make two cut extrudes to give the taper. See if that will work. If not, I know the method is close, but may not be exactly correct in the steps. I used it to get a flat pattern of an elliptically formed piece of sheet metal with an angular cut on one end. It worked well. Also, try looking in Help under Lofted Bend (in 2007 at least). Also, you can't use a closed contour, that is, leave a small gap between the ends or it won't unfold.

Bruce B.

I don't think SW will flatten a spline curve.

TOP

Abraham wrote in news:Xns9981A86F17C96abrahamnonecom@

I just read on the net:

"Flattening in SolidWorks requires that bend faces are limited to cylindrical, planar, conical shapes."

Cheers, John

TOP wrote in news:1186153809.018793.280260 @e9g2000prf.googlegroups.com:

Ok, here is the software that can do that: Rhinoceros

Cheers, John

I tried this method. It doesn't work if you cut the taper after you loft the bend, as SW is unable to flatten it. You have to make your second plane at the angle that gives you your 120mm and 150 mm heights at the ends.

Jerry Steiger Tripod Data Systems "take the garbage out, dear"