Hi all
I have a stamped sheet metal piece.
It's not a part converted into sheet metal, I started from a plate so I have bent base sheet in my tree.
Now I would like to cut out a shape in the sheet metal (a rectangle minus the bottom side) the red line in my drawing and fold it according to the red dotted lines.
I searched in sheet metal tools, on forums and found no answer. Could someone tease me?
Thank you so much!
I didn't understand everything...
Can I attach the file I'm looking at?
Either you have to remove the material in a U-shape and then insert a fold, but I don't think it works since the edge is not straight.
Or remove material in rectangle and use swept folded sheet metal but you will have to tinker to have the right unfolded
Thank you Bart for your responsiveness.
The customer is very sensitive about the distribution of these files and I can't afford to pass them on. And it's a shame, it would have been much simpler.
I work in real life, from these parts and I modeled them to give it a new laser cutter path.
The goal is to pre-cut tabs that will then be folded.
I have tried to do what you recommend. But the winding function does not work on a sphere and the projected curve function does not allow material to be removed afterwards. I'm a little lost.
With the 3D Sketching tool, is it possible to create a fully constrained drawing along a face? A bit like drawing with a marker on the real object?
Thank you!
The pink line has nothing to do with it? if?
I think.
Without the part it's complicated...^^
Basically, it's a stamped part where you add a bent tab after stamping, right?
Good evening
Why not add this shape to your stamping tool??? It would make your life much easier... If you want to make the tongue by folding you will need a special tool for it, in concave shape because otherwise your sphere will be deformed by the vee and the punch which have a straight shape.
@Bart
Yes, the pink line has nothing to do with it, it's a selected edge.
I've sketched something out so that you understand better.
@GT22
Your tip is pretty good. The problem is that my shape will probably arrive almost at the top of the dome. So extrusion may mess up. I would have to be able to roll up or project a sketch and extrude in a "normal" way in relation to my surface (to simulate a 5-axis laser cut).
@AC Cobra
It's not stupid at all. Especially since I can select faces to remove during stamping. I'm going to try that.
Thank you.
to have a normal casi extrusion on the surface
make your piece surface and thicken after cutting
@+
That's why I suggested it to you, it's much easier to make and especially since the piece will fall apart. ;-)
Did you succeed by adding this bent tab to your shape tool as I had proposed to you???
@GT22
Excellent idea. It's true that for that I would have to go through surface and then thickening.
@Bart.
It's great! I don't need it to be foldable at all. The goal is on the one hand to do my calculations and my design and then to send the customer a new route for his laser cutter. The unfolded state is not necessary at all. Is the tongue based on a constrained sketch (copied from the hollowed out area) or completely redone?
@Cobra.
I admit that Bart's track seems simpler on my side for the design. I could come back to it very simply. Changing the stamping form will certainly be effective but perhaps a little too drastic. In any case, if I come to this method, I will obviously keep you informed.
Thanks guys!
I created a plane tangent to the "dome", then I did a "normal" rectangular material removal.
I then created a parallel plane offset from the vertical edge created by the previous material removal. This plan will be used to create the profile sketch to be scanned. It is offset by the value of the notch you want.
On this shot, I create the sketch of the tab, and then I use the swept base boss feature to create the tab. (For the sketch, I used the shape of the dome using "Convert Features to Have a Tangent Curve"
I add a removal of material through the first shot at the beginning to carry out the second notching.
I then use the "combine" function to bind the two bodies together.
And that's it. =)
After to make it configurable, it's something else...
EDIT: Sorry, I hadn't recorded the song and was a bit lazy to redraw it..... ^^
Hello
I think you should make this cut before stamping, you would no longer have a problem with flattening.
Otherwise you haven't tried projecting your cut sketch onto a plane, extruding it without merging and using the intersect or combine function?
Well, I succeeded by tinkering with the bart technique.
Thank you very much for your time.
@ you to validate the answer @ Bart as the best
thank you @+ ;-)
