Hi modellers!
I have a sketch (imported from illustrator) that I've have wrapped onto a curved surface.
Now I want to use the wrapped sketch to trim the surface.
The problem is the fact that I'm only allowed to pick one outline for each trim. This means that I have to really many trims to get the surface I want.
Is there any way to do this proces more efficiently and speed up the proces?
I want all the centers of the circles cut out, like the three in the lower left corner.
Best regards.
In some cases, you can project those curves back to flat plane sketch and then extrude that sketch to remove material. In your case, this would work easily as the curved surface is less than 90 degrees.
Query-select the curve and see if it won't let you select the ENTIRE curve (composed of all of them). If not, as Nike says, Just do It. 
PTC isn't listening to Nike... You can only select a single closed loop in the trim tool. You get the option to select the Rule-based "All curves in feature" but it won't allow selection of a wrapped sketch with multiple closed loops.
On the other hand, you can extrude a thin feature and remove material, which, of course, has to be planar. I see room for improvement here 
Yep. Ran into this when doing text.
This is probably more telling:
You can select the loop of each letter when you Project the curves from the Wrap feature back to the sketch plane (when creating the Extrude sketch). This makes it a very simple process. Remember to extrude as a thin feature since solids and surfaces don't mix.
Thank you for your answers both of you
I manage to solve the problem by projecting the wrap back to the sketch plane and extrude the holes away.
If you have a surface that bend more than 180 degrees, you have to do it the hard way?
Thanks again.
I was waiting for that one.
You have to be careful with spinal bend not to scale the part along the bend contour.
If the surface was not one that lends itself to a "wrap", it would be a great choice.
Who, ME???
For the one he wanted, it seemed like it would work fairly well. It'd be interesting to do 2 on top of each other and see if there was any distortion.
I've found that the intersection of 2 curves is NOT exact in creo anymore, so if that curve is crucial, use a curve from the intersection of 2 surfaces. Dunno why there's the discrepancy now.......
Yeah, in Pro/E, there's a dozen ways to skin a cat (and sometimes you have to try ALL of them to find one that actually works...... ).....
That must be that "relative accuracy" where close is close enough ...and sometimes better 
...
Yeah, in Pro/E, there's a dozen ways to skin a cat (and sometimes you have to try ALL of them to find one that actually works......
So does trying those other 11 methods first count in the reduced mouseclick directive? 
Antonius Dirriwachter wrote:
So does trying those other 11 methods first count in the reduced mouseclick directive?
I think that's been superseded by the "must have ribbon" directive. 
Actually the screenshot was of a simplified problem.
What I actually need, is to cut the holes in a double curved surface. I don't think that sheetmetal and spinal bend would help me here. Maybe? Otherwise it's a great way to do it.Thanks for the suggestions.
I manage to solve it by extruding the wrapped sketch that was projected back on a workplane... and because you can't wrap a sketch onto a double curved surface I had to create a single curved "dummy" surface that immitated the double curved surface as close as possible.
The result:
It's still just a test and not the final part.
Thank you very much for your help. You just helped me gain some new CAD skills
Just for fun, I wrapped a series of circles onto a "developable" surface thas has curvature normal to the exis of the final part. So, the circumference of the circles is correct (unlike projected). then I did a spinal bend on it to get the compound curvature (like a revolved surface). As you can see, now the holes are distorted near the top (smaller end) where the spinal bend actually shrunk the material. I wrote a relation to force the developed length to be equal to the big end. I could easily have donw it the other way with the relations to make the holes near the top undistorted and have the material stretch (as would more normally be the case) to distort the bottom. But, this was quick and easy. Note: This is sort of cheating to create a Toroidial bend, with greater flexibility. I later thickened it and it worked at 1" thick no problem!
For you though, what I'd suggest is simply punching holes thru a surface, normal to a point on the surface corresponding to where the axis of the hole goes thru, then thickening the surface. This will give you distortion of the walls of the holes, based on the thickness. This will most likely give you geometry most closely matched to a real world production process.
Very nice! That's one I'll have to remember.
If the holes are more or less random, you could also Project a sketch normal to the face. The sketch would be the distorted feature that would closely approximate the position and round shape. In the sketch, the corresponding hole would be an ellipse. The closer you need it to be, the more the sketch plane will need to be normal to the surface at the hole's axis. I think that Sheetmetal holes will do this but controlling their location is enigmatic. But it is the most accurate I can think of as it does map the hole with K-factors in mind.
Yet, I think you, Esben, have already done a marvelous job on your part. So the correct answer is "NO" ...there is no easier way.
Thanks! I never thought to try and do that with a spinal bend. They teach you spinal bends for planar parts, but I thought, why not? It seemed to work just fine!. And, I think it ends up giving you something you couldn't get with a toriodial bend. I'm sure I can find a use for this somewhere.....
Yeah, it looks like he's got a model that will work. I can't speak the the sheetmetal thing since I don't use that module.
