Can this be done in SolidWorks?

Hello,

2mm thin sheet metal needs to be bent to match the side of a classical
guitar.

After it's been bent the length will be 340mm and the width (on one end
120mm and on the other end 150mm).

I need the flattened drawing.

Thanks, John

 

yes.

 

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.

 

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

 

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

 

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

 

I just read on the net:

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

Cheers, John

 

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"