Probe Causing Z height Zero issue?

So I’ve had my nomad 3 for a week now, I’ve done several jobs in different materials. Im very careful to set my zeros accurately in Carbide motion.

I set Z above my stock with a piece of paper and I start the job. I have also tried starting the spindle and lowering the it until I see a touch into the material.

it seems that about a third to half of the time, I start a jew job after zeroing, it probes, looses its zero and then plunges deep into the stock breaking my end mills as soon as its done with my VERY slow plunge rate. for what its worth I did have it once do the opposite where it set zero about 0.5mm above my stock because it finally kissed the stock on the last pass of a 0.4 pocket.

Im trying to figure out what’s going on because tonight alone I broke $60 in endmils.

A couple points: 1, I tighten the collet nut very well. 2; I have the Z set to stock top on carbide create.

Any other ideas?

Whenever I set Z zero and am unsure of things I move the machine to Z+6mm and use a 5.5mm thick piece of acrylic to verify that it is where it ought.

To verify that the endmill isn’t moving put a mark w/ a permanent marker on the shaft of the endmill or a bit of tape or some other witness mark to verify that the endmill isn’t pulling out.

Post a .c2d file, generated G-Code, step-by-step notes on how you are securing your stock and setting zero relative to it and managing any tool changes and we’ll do our best to sort this out w/ you.

Have you cleared offsets before set zero?

I’m not sure what you mean by clearing offsets, its weird that it works perfectly sometimes, I zero all three axis before every job and re-zero Z if I change tools.

Do you change bits with the machine turned on but without being prompted by Carbide Motion to change the bit?

Zeroing will not compensate for changing a bit without being asked to change a bit.

4 Likes

No. Wednesday I tested this out with my 102 end mill. It never failed doing 15 simple circles in acrylic. Height was perfect.

Last night, I initialized the machine. Changed the tool, to my last 1/64 endmill, Zeroed it multiple times. Then loaded the program. Started the job and it plunged at least 1mm into the stock when it was supposed to start at .05mm depth or even slightly above the work piece. Obviously the end mill instantly broke.

You may think it’s the program. So I loaded in a 0.3mm ball bur I had. Zeroed that. And it ran right where I wanted it to. Albeit with a terrible finish

I’m now wondering if I need to zero after I chose my G code program. I got confident with the machine after Wednesday assuming previous dives were user error. So of course I didn’t record it.

I’m going to record every start from here on in. I have more 1/64 end mills on the way but I can’t keep watching them break from Z height dives. I may also start doing a test program of a quick circle 2-3mm above the work piece. Then load the actual program. I still think it’s something with the probing sequence. Not sure why it even has to do that after I set zeros.

Can you elaborate on this part? After initializing the machine, how did you change the tool?

I think there’s a misunderstanding of the probing routine and setting zeros. Your machine has no way of determining the physical length of the bit you have put into the machine. This is a fundamental concept you have to consider when using the machine.

It only knows the difference in length to the bit that was in the machine when the machine was initialized. Just the difference - not the length. If you make a change that corrupts this “difference to last time I measured” you will experience failures.

2 Likes

I plug my laptop in and hit the initialize. Loosen the collet after it says change the tool and put in the new end mill. Let it probe again. After that initialize sequence, I set zero in the jog tab with the end-mill I’m using for the job. I set zero with a piece of paper. With the new tool in and zero’d. I load up the program and hit start. I think the first 12 lines of code is the machine probing the tool, prompting me to make sure the tool is correct, and then probing again. I feel it’s this sequence that the Z zero gets corrupted. Not sure why It does this sequence anyway.

Again it’s not every time, Just sometimes but it seems to really do it more frequently with these 1/64 end mills.

There is still a little bit of ambiguity in how this is phrased. Is “new end mill” the “end-mill I’m using for the job” ?

Do you ever change the end mill without a CM prompt saying the equivalent of “put an endmill in now”?

If you are having trouble w/ endmills which are notably shorter than others I’d suggest starting w/ them and using the shortest endmill when initially setting zero so as to ensure that you aren’t bottoming out the Z-axis.

1 Like

Moving forward, when I have a job calling for a 1/64 end mill Im going to make a point to change to the 1/64 endmill, turn the machine off, turn it back on, initialize it, load the job, then zero the end mill and then start the job. Im also going to video all these starts.

These plunges are happening after I have changed the end mill and after I zero that new/changed (1/64) end mill.

What I’ve been doing if I have a 102 (or other) end mill in the collet, and need to change to a 1/64. I initialize the machine with the 102 end mill. Then after that process is completed, I change the 102 end mill to the 1/64.

Then I zero that 1/64 endmill with the jog function. Then start the job, I don’t always initialize the machine with the 1/64 endmill but I do always zero the 1/64 endmill that I’m using before I start the job. I assumed that would be satisfactory. I thought the initialization was for the machine to locate the limit switches and switching tools after the initialization would be fine as long as I zero the machine again with the changed endmill.

none of these plunge issue jobs require a tool change anyway. its the first line of code after it probes. It plunges too deep because its zero is off. But again I always zero the end mill with the jog function that Im using right before I start the job.

I know Im repeating myself a lot, its frustrating and hard to convey,

Thanks for all the replies.

It seems clear that you are changing the endmill at the wrong time.

It’s hard to say this again without sounding odd… but… NEVER just change the endmill. As in, NEVER.

There are only two times you can reach for those spanners and change the endmill.

One time is when the machine is powered off.

The other time is when Carbide Motion has a dialog on the screen asking you to do it.

You simply cannot do it at any other time.

4 Likes

This is SUPER critical input. Only change anything (Bit or Dowel) in the collet when prompted. Also, make sure that if you ZERO just Zee using the BitZero that you set the entire apparatus on the surface, not having it sit on the corner. I murdered a couple of endmills because I did not realize this. Do not use the bitzero with the dowel unless the Nomad asked you to insert a bit. If you zero with the dowel without being prompted then the Nomad doesn’t know how long the dowel is and the zero will be wrong when it goes and grabs another bit.

1 Like

I don’t know if you are changing tools, but if you are, I had similar issues: my Nomad would just ram into my stock. I then realized that I should change the tool only when prompted. The Nomad will do the tool length probing multiple times, and if you change the tool prematurely, it will get confused. It sometimes seems like you can change the tool already, because there is another probing cycle right afterwards, but stick to the prompts.

I don’t know if this helps in your case, it’s just a problem that I had.

2 Likes