Is it possible to set a starting depth in MeshCAM? This would be helpful for multi-step runs. Maybe I need a G-Code editor?
Starting depth?
MeshCAM starts with the stock and cuts out the object. It has to slowly machine in. Roughing first, then finishing. The roughing has a depth per pass and the stock to leave; the finishing… finishes up.
There is no “starting depth”.
Perhaps I’m not understanding what you want to do. Can you please describe it in detail?
Once we understand what you want to do, it is highly likely we can find a “trick”.
mark
Example:
Start job with max depth of 3 mm but one that I need rounded edges for the first 0.9 mm. I do a finish pass with a depth of 1 mm and then switch cutters to a corner rounder and run it at 0.9 mm depth. I now need to finish cutting out the full 3 mm depth. It would be great to be able to start at the 1 mm depth instead of having to run the job over from zero again.
There must be an obvious way to do this so I’m curious as to what the best method would be? I just sort of assumed there would be this option in CAM but maybe I’m looking at this all wrong.
I’m having a dense moment… I don’t see the example at all (my fault)!
I’ll study what you’re saying and see if I figure out what you’re trying to do.
Do you have and STL of the object you can post and we can examine? Seeing what you’re trying to mill would help.
mark
See my acrylic thread for an example of what I’m making…I posted a picture there. You’ll notice the corner rounding of 0.9 mm. I need to cut a 1 mm channel out of the stock first, run my corner rounding pass, and then finish the cutout. It requires three passes to do this which I’m okay with, but I would rather my third pass start cutting at 1 mm depth since an earlier pass already took care of the first 1 mm.
Make sense?
I’d rather not post the STL for this one.
@dyelton do your top machining (pass 1 and 2) and then for pass 3, just use the typical waterline+pencil finishing only, with a waterline angle limit of 89 degrees. That will effectively machine just the vertical surfaces.
Randy
My advice above assumes you have the top rounding modeled in your STL. But then I realized you might be using a square-edged extruded DXF and that “corner rounder” is a concave bit to add the fillet.
In that case, to do the vertical walls in pass 3 you would define a new stock that is the .9mm thinner than your part, lock the stock dimensions, uncheck “center Z” and set a lower Z margin of 0. That will place the stock flush with the bottom of your workpiece, and the workpiece will protrude .9mm above the stock. Just make sure your retract/clearance height allows for the .9mm of geometry above the stock.
Randy
@Randy Your last bit would work and I thought about doing it that way already…I had just hoped there was a way to make it so I would lesson my ability to mess things up if I didn’t get it right. It’s much better, IMO, to set your depth than to monkey with the stock dimensions, but I’m nitpicking.
I do have the fillet modeled but have it hidden when I export the STL. My walls are 90 degrees and I just run the corner rounder to give me what my model has. No point in the STL having the fillet doing it this way.
Thanks!
You might also be able to do this by manually editing your g-code. It’s surprisingly easy to do, since MeshCAM thoughtfully puts loads of comments in the code. Try this:
1). create a job in MeshCAM to cut to the full depth. If you need the first pass to land at exactly 1mm you will want to set your depth of cut to a number that divides evenly into 1mm, eg .25mm or similar.
2). open the resulting .nc file in any text editor. I personally like Textwrangler on the Mac, but any will do. Look at the code. Depending on how you are cutting that slot, do one of the following:
2A): If you are cutting that slot using a roughing pass, you can just use Find and go through the code looking for comments like this: (Roughing Level Depth: -1.00). Once you find your depth of -1mm, use Find to go the NEXT "(Roughing Level Depth: -X) " comment, select and delete that comment and everything forward in the document to the bottom, making sure to leave:
M5
M30
(END)
(OF PROGRAM)
Now you should have a g-code program that will stop at 1mm. Do a “Save As.” Now re-open the original document, and do the same thing, only this time delete the code from after it says “(Parallel Rough)” at the top, down to the depth you want to start at. Presumably 1.25mm in my example. Do a “Save As” for that document. Now you have a g-code file that will start at the depth you want.
2B): If you are cutting the slot with a waterline pass, it’s a bit more involved, but still pretty doable. Use Find to go to where it says (Waterline Finish) in the code. If you see something like this:
(TOOL/MILL,3.1750,0,19.0500,0.0)
M6 T102
M3 S7500
(Waterline Finish)
Make sure to keep those lines.
Now use Find to go forward and look at the lines that start like “G1Z-” You will see that the depth progressively gets deeper as you step forward through the document. Find the depth for your first pass, go to the NEXT depth, and delete it and everything forward, stopping before the bottom bits as in step 2A. Now just do the same stuff mentioned in 2A to create the two different passes.
3). TEST THESE G-CODE JOBS IN FOAM OR JUST AIR CUTS. You can also try to run them through a simulator and see if it catches any errors you might have made.
4). congratulate yourself on being awesome.
5). take it a step further. Generate code for a job that involves a tool change. Look at it and see how that is accomplished. Combine your three jobs into one file with tool changes built right in.
6). repeat step 4.
@Randy I’m curious if I am just using waterline and pencil finishing and have the full retracts box checked, does the full retract apply to everything or just waterline?
Thanks!
Donavon, in my experience roughing and parallel finishing and pencil always have full retracts, no matter how waterline is set. I think waterline is a special case, becuase on a concave (inside of bowl, say) shape there is no need for a full retract to clear geometry, but on a convex surface (the outside of the bowl) the safe way is to have full retracts to clear possible geometry. I always specify full retracts in any case but I always keep my retract height to less than .1", usually .05".
Randy