I need to machine a bunch of rough-cut pieces of rectangular aluminum tubing, which are precut in sort of a trapezoidal shape. Here is a photo of a couple:
The interior and exterior mill finish of the tubing is fine, I only need to machine the rough cut edges (the pieces are a little over-length to allow this) and add a slot in the top and two holes in the bottom. The result should look like this:
If I use the STL file for the desired result with the stock material defined as a rectangular prism that encompasses it, there will be a whole lot of machining of “air” wasting time. I tried to play with keep-away regions, but didn’t really get a result that I wanted.
I thought that if I defined a solid that just had surfaces corresponding to where the sloped-edge trimming, the two holes, and the slot is, maybe that’d be better. So I came up with this:
I’m sure that’s an improvement because it won’t be trying to cut down to the inner bottom of the tubing, but still it’s going to waste time machining a lot of air. Even if I change to a mostly rectangular STL for the cut geometry, so that only the edges, holes and a subset of the notch region is specified, there still would be a lot of air-machining just to do the holes.
Is there a way to define the STOCK material as the rough-cut piece to avoid all this?
What you’re looking to do is possible a bunch of different ways, but is probably easiest using a tool like Fusion360 with the integrated CAM. In Fusion360 you can specify your stock as another solid body in the file, so you could model the “raw” stock as-is, along with your model, and go from there. I can post some screenshots of this if that interests you. If you haven’t checked Fusion out yet it’s free for hobbyists and small fry like us who are using it as a part of organizations who make less than 100k per year in revenue That’s a problem I hope to have in the future so I can afford to pay the $100 per month for the software as an official enterprise!
Troy, there is no way in MeshCAM to define other than a right rectangular prism stock.
To do your workpiece I’d:
Do the holes by drilling. MeshCAM is good at that actually.
Use 2d STL like your last screenshot, but plug the holes too. Since you’ve already rough-cut the ends, use finishing only, machine geometry only, zero margin, don’t machine top of stock. Use the direction of parallel finishing that goes along the slot plus waterline, with a crossover point so that the sloped surfaces are finished by the waterline. Use a fine waterline stepdown because it will be cutting through the top wall of the tubing at the slot (unless you rough-cut the slot also with the saw).
@UnionNine & @Randy thank you! I need to do some studying, but I think I get the gist of either.
If I do it as Randy suggests, is there a way to combine the drilling and slotmaking and finish into one NC file so that I can put the blank in and walk away, come back and repeat, or would I need to do them as separate ones on each?
Troy, if you want to machine the holes rather than literally drill them you can use Machine Region to roughly outline the two holes in your first STL. Do a waterline + pencil finish on the holes using your preferred cutter. Since you’ll be wanting to use a ball-end cutter on the slot due to its round bottom, and if you want to do the holes with the same cutter, you’ll need to set max depth deeper than the actual workpiece by the radius of the cutter, since MeshCAM controls the tip of the cutter. Write out the gcode for the holes.
Of course, if the holes are the diameter of your cutter you can just use the drilling routine but physically use the cutter to plunge the holes.
For the holes, you’ll want to verify that the ER chuck won’t hit the extrusion walls when you machine the holes.
Then go back and delete those Machine Regions and roughly outline the slot with a new Machine Region. Process it like I mentioned above and write out that gcode. If you haven’t pre-rough-cut the slot with your bandsaw it would be a good idea to do a rough cut on the slot before the finishing to remove the bulk of the material.
Then make a second STL with both the slot and holes plugged, and process it with the same ball-end mill, as I outlined above. This will machine only the slopes.
You’ll end up with 3 gcode files. It won’t really matter which order you stick them together but just concatenate them with a text editor. You’ll need to do some cleanup by removing some lines where one file ends and the next begins.
You’ll delete the lines in bold. Basically at the junction between two files remove the lines from where you would turn off the spindle, to where the next file makes its first move. Since you’re using a single cutter you don’t need to turn it off between the segments, and the tool is already defined the first time so you don’t need to re-call it and re-start the spindle.
Thanks @Randy! This seems to make sense to me, I’ll give it a whirl.
The holes are larger than my tool, and I have already checked that the collet nut will clear the sides as it goes around enlarging the hole, so I think this will work.
That’s a problem I hope to have in the future so I can afford to pay the $100 per month for the software as an official enterprise!