Tool Changes, Z Axis Issues

I’ve been working with the Nomad for a few months now and have had decent luck, once I figured out how to work around some of the little quirks that come with Meshcam. I’m still having trouble when using different tools for the rough and finishing passes. I’m trying to mill some molds out of Teflon sheets and it works just fine when the tool is kept the same for all passes, but as soon as I try and use an 1/8th bit for the roughing and a .03 for the finish passes it destroys my piece. The zero point for the first bit is used when the second bit is inserted even after zeroing the second bit before milling I end up having the bit run into the material and have to shut the machine down. Is there a way to do this tool change and continue to mill the piece as designed or do I have to use the smallest bit necessary for the whole project? (Currently milling the molds again using .03" and milling time is over 44 hours estimated) Thanks in advance for any wisdom!

MeshCAM toolpaths always deal with the tip of the tool. The length of the tool doesn’t matter to the toolpaths. That is miorrored in the CutViewer Mill toollpath visualizing program, which doesn’t care how long the tool bits are.

In my Sherline days, I output and ran MeshCAM’s roughing and finishing toolpaths as individual gcode files, loading and touching down each tool separately to establish Z 0. On my Tormach, with pre-mounted tools and a tool table calling out the relative tool lengths, the controlling software adjusts for the individual tool lengths.

The Nomad is refreshing with its tool sensor. I just put in the called-for bit at a random length (just ensuring there is enough projecting from the collet for the depth of machining), and Carbide Motion senses the tool tip and resets the Z reference accordingly.

I have done testing on the limit switches and the tool sensor (which uses the same microswitch) and to the limit of my ability to measure, all are repeatable to .001". I am very impressed at the quality of components and construction of the Nomad.

I’ve been using MeshCAM for 10 years now and trust its output 110%. My experience with the Nomad is much more limited, but I trust its handling of toolchanges too.

I have a question about your wording

even after zeroing the second bit before milling

To me that sounds like you are trying to do something manually to adjust the Z of the second bit? That is not necessary, but I apologize if I miss your meaning.

Randy,
For the tool changes I’m simply putting in the new bit and tightening it down. After confirming with carbide motion that the new bit is installed the program moves over and remeasures the zero point at the tip of the bit and continues to drive the bit into my working material.

OK, sorry for my misunderstanding. I just wanted to make sure.

Carbide Motion doesn’t care or ask what tool you have loaded when you do the initial Move Tool to set the X0 Y0 Z0 relative to your workpiece. Of course, it is logical to use the actual first tool to do that, and that is what I do. But it could be a random tool also, or even a 1/8" dowel pin, since after moving all axes to the home switches, CM then measures whatever is in the spindle.

You could do a test with a scrap piece of material, using a different tool to do the initial X0 Y0 Z0 setup, then load the actual roughing tool when the gcode calls for it. That tool should properly start your roughing if CM is working as it should.

You could also put a piece of scrap stock on the table, put a random tool in the spindle and set X0 Y0 Z0 on the top of the rawstock near the middle. Then you could run a program like this, using random tools for T1, T2, T3, T4. This will have CM measure the tool, then move it over to X0 Y0 and then down to Z0, which should just be touching the top surface of the stock (maybe use the piece of Renshape that came with the mill or something else soft like blue foam insulation or balsa wood…) then wait two seconds while you look at it before moving back up an inch and then calling for the next tool. it doesn’t start the spindle rotating at all, just touching the tool like in the inital setup. Each tool should just kiss the stock if all is going OK. Otherwise it will plunge the different tools into the stock or come short

G20 (puts gcode into inches)
M6 T1
G0 X0. Y0.
G0 Z0.
G4 P2 (wait two seconds for observation)
G0 Z1.
M6 T2
G0 X0. Y0.
G0 Z0.
G4 P2
G0 Z1.
M6 T3
G0 X0. Y0.
G0 Z0.
G4 P2
G0 Z1.
M6 T4
G0 X0. Y0.
G0 Z0.
G4 P2
G0 Z1.
M30 (end of program)

It doesn’t matter which tool you put in the spindle at any step, since CM is just concerned with the tip of the tool. You could even just remove and replace the same tool at a different projection from the spindle, for that matter.

I read about a similar issue here in the forum and I believe the problem was the roughing pass wasn’t getting into some small areas. As a result, during the finishing pass the tool was plunging into material that was thicker than it thought.

A few things may help is this is the case - try leaving less material during the roughing pass and reducing the plunge rate and depth per pass on the finishing operation.