Dennis,, I think this might work. Select your holes and on the sketch menu do a Convert Entities. Then right click the view and Hide/Show Edges and select the holes again. This will just hide the edges of the holes and not the newly converted edges. Then put what you want on whatever layers you want. You could probably also right click on the view and Convert View to Sketch and work it that way. Seems to work. I saved as DWG (no mapping) and it came into DraftSight like you would expect with the holes on pierce and edges on cut layers. Since the edges of the holes were hidden when I turned off my pierce layer the were no holes at all. If I hadn't hidden those edges it they show up which may lead to an issue.
Dennis, I knew of this option but I really don't want to convert edges into sketches on my SW drawings. If I go that route I might as well just do all the layering after exporting to a DWG. But it might be my only option.
I used to leave the perimeter the default and then for the holes we would have a layer called scribe and do it like Dennis Bacon mentioned and when the drawing was loaded into the Plasma Program it would treat the layers as intended...
I agree Dennis. I figured that is what you would say. I am going to hammer on this some more and see if I can come up with something else. So far it does not seem like it is possible to put edges on different layers. Hope someone can prove me wrong.
I don't know how to do exactly what you want, but....
At the part level, you could create a configuration that has the holes suppressed.
Then at the drawing level, have two views with the two different configurations, one labeled "CUT" and the other labeled "Pierce". You could even put the different views in separate sheets. See example below:
What the part looks like:
Select the holes feature, RMB and select "Configure Feature"
In the "Modify Configuration" window, add the configurations and select the correct suppression toggle.
Create a drawing and add the two views (put them on separate sheets or even separate drawings if you want).
Then select the "reference configuration" drop down box for each one:
I think that this might work for you.
I can't use configurations with this because I need all features to be shown on the DWG file. What I am trying to do is be able to model parts that are correct per the final process.
If you take the part you have drawn and leave it on the DEFAULT configuration in the DWG. I want to the perimeter to be on a "CUT" layer and then the holes to be on a "PIERCE" layer. So that way our cutting software can recognize what to do with certain features, so when with the holes being on the pierce layer the torch software knows to just pierce the location of the hole and not cut the perimeter. The pierce is then just helping them locate the holes rather measuring and marking. Then the print will determine for them which holes to drill.
So far the only option that works is Dennis Bacon's idea. I just would like not to do a "work around" to do this. But if that's my only option then I don't have a choice.
OK, here's an option then:
I think that this is an easier work around.
Create your part complete.
Make a copy of that part (or add the body to a new part to link them together, with a proper configuration).
In the copy, suppress all the features that you want on the second layer.
Then add both parts to the drawing, and put the complete part on PIERCE layer.
Overlay the two views (using the alignment feature).
Now you can swap layers, and it should trick the DWG into what you want.
Edit: the issue here is that a single part can only be on one layer, and that propagates though all the views. When you separate the two parts, you can put them on different layers, you just have to overlay the views.
If you want an example, let me know.
Just another thing you could try and that is when you're in the drawing view, find the sketch in the feature tree and convert the entities and add those line/lines to a layer, make the outer profile sketch a different color etc... then you can select the main body/extrude in the drawing view and hide it, that way all your new converted sketches will show and will move when you change the main part etc.... Then after you save the file as a dwg the layers will show like Dennis Bacon mentions above..