sheetcam.com

Hello,

Is there a variable available to the post to determine if the entity being cut is an inside offset or an outside offset? In the Operation dialog, I know you can specify Inside Offset, Outside Offset, or No offset. SheetCAM is very smart to have the operation set to outside offset and still recognize the need for an inside offset.

Cutting Rules has an option for "On Inside Corners" or "On Outside Corners" but i am needing the entire path, not just the corner.

So, is there a way for the post to know if sheetcam is making an inside or outside offset?

Thanks,

David

I believe I have a YouTube video to help you solve this.

https://youtu.be/EaPys9ovKKw

That works prefectly fine for a single part or a part with only a few holes. Our problem is we typically have multiple parts with numerous holes already nested on a sheet that is imported into SheetCAM. This would be excessively time consuming to do in our case.

Oh, I usually just burn single parts that I nest and array using sheetcam. So, if you assign inside and outside to the single part and then array them it uses the same info for all parts. Sorry I couldn't help.

No problem, I appreciate your thoughts. Worst comes to worst, i will have to set all inside paths to a different layer and do that, it would just be a huge time killer. Our laser machine is set up for production and we try to nest as much on a sheet as possible. I could have parts from a few different customers nested on one sheet.

Just a thought - you can move just inside contours to a different layer pretty quickly. In edit contours mode right-click->Select all inside contours. Right-click->move to layer

That will work, thats an easy simple step. Now i just need to get the post to determine which layer it is on. Is there any function that can be used to set a variable based on the layer of the operation or some sort of that? Im trying to avoid having a different tool for inside and outside paths. That would result in an unworldly number of tools.

The end result i am trying to get here is somewhere in the g-code before the toolpath is written, there needs to be a line that says "#501=107" for all inside paths and "#501=108" for all outside paths. But i need that to not be hard coded because the 107 and 108 could change anywhere from 102 to 110. Id prefer that be a custom tool parameter.

I ended up using another post variable to be set using "set post variable" operation to tell the post which contour I am working with in combination with the right click select all inside move to new layer step. It works, thank you for the ideas Les.

Its still not the ideal process, but it works and makes it so sheetcam will work with out laser. Maybe one day you might be able to add a "On Inside Contour" and "On Outside Contour" function set, but this works for now. Thank you Les!

Hey Les, I hate to but I've got to go back to this one. I have ran into a situation where my workaround will not work. Hopefully you can come up with something or I can convince you it'd be worth the time to add these functions.

I drew a part in AutoCAD. The part is a U-shaped bracket with two mounting holes. I have nested 280 of these parts on a sheet using NestFab. (MyNesting may work through the plugin with SheetCAM, but NestFab does not. The file extensions are different.) I then imported the resulting nest DXF file into SheetCAM. The outside path is on one layer and the holes are on another layer. The issue is, All of the holes are cut first then the outside paths are cut. We actually need 300 parts cut, so either i will have to make a separate program with a separate nest or waste a sheet cutting a lot of unnecessary holes.

Do you know of any way to cut this on a per part basis instead of SheetCAM seeing it as one giant part?

I see the option in CutPath in the Operations box to keep parts together, but that does nothing if the holes are in a separate operation.

Any thoughts?

In edit contour mode delete the sheet outline. Now right-click on the job and select 'break up manually nested drawing'. You already have 'keep parts together' selected in Options->job options so it should now cut each part in sequence.

Dude, you're the man Les. You have a solution for everything. Thank you!