Creo 2, M230
I'm creating a sheetmetal part and I have opening that I want cut with a single laser cut to create a knock out, like this:
I can create a narrow extruded cut (which is how this image was done), but that would mean double the laser time when I only really need a single pass.
Ho do I create a simple, single laser cut pass like shown?
I'd create a single sketch which generates the centerline paths of the knockout cuts and then use it to create the 11 thin extrusions. That would generate the "hifi 3D model". Create a simplified rep that does not contain these slits and use this rep as the model for the drawing. Since the centerline paths would be shown on this drawing and the resulting edges would not be, programming the NC code should be straight-forward by exporting this drawing as DXF...
In fact, I might skip the "true 3D model" step.
This seems like a reasonable, if cumbersone, approach.
I was hoping for a sheetmetal feature that would enable this without creating 11 features. I had hoped the "sketched rip" would, but I think it requires the sketch to be tied to a part edge.
Yeah, quite cumbersome; copy+paste special is a must here.
This is a sketch scheme I think I'd use for keeping those gaps under control:
Two features - one with the entire path and then use that to make an interrupted set of curves in a second feature for the displayed cut. I would probably put points on the original curve where the attachments will be and then construction circles in the next feature so that only one dimension is needed to set the tab width.
The "real" problem is with the CNC software not recognizing that a narrow cut can be done with one pass or a punch. Similar problems occur with half-punches for knock-out features, such as are seen in electrical boxes. It's a special feature that is handled diffenently depending on the exact means of fabrication. The alternative problem is that if a single curve is used, how does the software know when a rip/shear is required and when a laser/waterjet narrow kerf is OK?
I believe so, which is why I wanted to avoid the two lines of a thin cut.
Have you tried using a Cosmetic Sketch?
(and give the cosmetic sketch a color which your laser recognizes as a cut-line.)
@dgschaefer did you find a solution for your problem/challenge?
I did, I guess. I carried on making a narrow sectioned extruded solid cut (section width of 0.002") and placed a note on the drawing that they should be cut with a single laser pass. Not ideal, but it works as would have the other suggestions here. @psobejko's solution is close to what I did, but not quite because I used a single solid extrusion vs. the multiple thin extrusions. The single feature seemed easier to implement and control.