Had to split project in 2: why can't I re-use x and y coordinates?

So, I’m just making a simple sphere, around 2.75" in diameter. The plan was to make two halves and then glue them together. As I went along though, it occurred to me that I will be exceeding the flute length/cutting length of my cutter. I’m using the #101 .125" ball nose cutter that came with the machine. Meshcam gave me a gcode that looked fine at first, but it doesn’t seem to take into account the depth limits of the cutter. After trying unsuccessfully to figure out a way for meshcam to cut out enough material at the top of the stock surrounding the part to clear the way for the cutter to reach the full 1 3/8" to the bottom, I decided to slice the part into two jobs: I’d cut out a lot surrounding the part on the top half, and just do the minimum on the bottom. I was concerned that I wouldn’t line the two jobs up precisely and this would create a noticeable seam, but then I figured if I just determine the new Z coordinate for the bottom half, I could just re-use the X and Y numbers I had for the top half, right? This would put me in the exact same spot as before. I just typed in the same numbers for X and Y at the set zero page in meshcam, confident that this would work… but no go. The cutter promptly began gouging the newly cut top of the sphere when I started the bottom half job.

I have a number of questions about this exercise: first, is this really as severe a limitations as it would appear? I took for granted that I could put a piece of stock in this machine and get full 3" Z cuts out of one job; hence the name ‘Nomad 883’. I’m sure this is indeed the case and I’m just flailing right now, so please someone, tell me how to do this! :smile: It seems like I should be able to cut out extra material surrounding the part in a pattern that narrows toward the bottom so that it clears the way for the shank as I go down, but I couldn’t figure out a way to do that. Also, I’m dying to know why my plan to re-use the X and Y coordinates didn’t work.

Think of a piece of stock, a cube 3" on a side, that is resting on the XT plane (the bottom of the cube is at Z=0). A 3" sphere can be embedded within. Now cut the stock/sphere in half at Z = 1.5.

No matter what the Nomad maximum (physical) Z is, you’re still limited by the total length of the tool when it is mounted in the collet for maximum working Z. For our example, we need a maximum depth of 1.5". We need a tool of the that length AFTER it clears the collet. It’s never a good idea to get too close the collet so the effective depth is a little bit less (or we need a tool that is a little bit longer).

As long as the flutes are cutting material and we’re not colliding with uncut material, we’re OK. When machining a sphere (via upper and lower halves), the flute length isn’t really a concern. One can always engage the stock.

We need to rough away the stock to “expose” the sphere half. We can do that via a layered approach where we remove stock a small amount at the time. A good general guide line is 1/2 the diameter of the tool.

The sphere half has to be “held still” so it doesn’t go flying after we machine around all it. MeshCAM has construction tabs (the red lines one can apply) to keep the piece connected to the stock. This means our stock needs to be bigger than the 3" so there is stock left for the construction tabs to connect to.

Now our imaginary block needs to ~4x4x3 (to grab in four direction) or ~3x4x3 (to grab in two directions).

With a flip jig, this is a perfect job for two sided machining. Top half, flip, bottom half. Cut the construction tabs, remove sphere, clean up the part.

Flipping a part requires the stock to very accurately known. One would get stock that is ~3.25". Machine the top flat (take off a bit), flip it, then machine flat again such that the remaining stock is 3.000" in thickness.

I’ve read what you wrote and I’m not sure I quite understand. I THINK I do and I will try based on what I understand. The Nomad is a 3 axis machine. One cannot machine under another feature in one machining session. In your sphere example, machining from the top, we can easily see how to do the top half. The bottom half, which is below the top half isn’t reach able. The machine doesn’t know the material is there so the trying to do the bottom half in the same machining session will try to go through the upper half to machine the bottom half - not a pretty thing (and likely to break a tool).


Thanks so much for the reply, Mark. I went ahead and did a few drawings - hopefully they will communicate better than my wordy post did. The one showing the Meshcam work around is what I wound up attempting (without success), and the other one shows what I got for gcode from Meshcam, and what I’d like to wind up with.

Thanks again!

Uploading blob.png…
Uploading blob.png…

Whoops, those pictures don’t seem to be uploading - I’ll try it again.

@pjhof, there are a couple of ways you can do this::smile:

  1. Use a longer endmill. :smile:

  2. Do the sphere in two jobs: first set Machine Whole Stock and set a Max Depth that is high enough that the collet won’t hit. Just run the roughing from that job to clear out the bulk of stock. Go back and reset Max Depth to the bottom of the stock, set Machine Geometry Plus with a small margin and rerun the job, just for the finishing passes. The remaining material around the base of the sphere is probably small enough that you can get by without roughing. The job will end up looking like the left drawing in your last picture.

You are correct–MeshCAM does not have the ability to take the collet into account when making toolpaths. It’s up to you to work out the maching strategy.


Thanks Randy,

No disrespect to Meshcam, BTW. It’s just that as a novice, I’ve been using the Carbide Auto
Toolpath option, so I thought that since I was using the proprietary machine and bit, it wouldn’t give me the option to do anything that would cause this type of issue.

So it sounds like you’re recommending what I tried in my ‘Meshcam work around’ drawing, more or less.Is it true that I could use the same numbers for X,Y,and Z when it’s time to set zero the second time around? If I’m wrong, I don’t know how I would get to the same spot again…

How about my first drawing? Is there a way to make that happen?

Thanks for your patience!


Pete, the only way do the first drawing concept, with the sloped roughing walls, is if you draw the geometry like that including the rawstock and machine it as part of the workpiece itself. But you could do that as long as you have accurately measured your rawstock ahead of time. I have actually done that in the past for a different reason.

About the option I described, you would do the two operations to a single workpiece while it was still clamped in the machine. It is not uncommon to make two or more MeshCAM setups to progressively work on a workpiece. Since you are doing roughing and finishing (but from two trips through MeshCAM) without changing the Program Origin, you can run them one after another without doing any re-zeroing or resetting.

In fact, the Nomad is accurate enough in homing, and retains its user-set coordinates when you power down, that I have machined some on a workpiece, shut down overnight, and resumed the next day without doing anything new in the way of setup. The proper coordinate zeros were still in place, Carbide Motion measures the tool anyway at startup, and the new machining aligned perfectly with the previous machining.



A-ha! So I was making it more complicated than I needed to; I can’t wait to take another crack at it.

Same goes for your suggestion about the first drawing: that’s an interesting way to come at it, which is very doable and I’m eager to try.

Thanks a lot!


Pete, I think I misunderstood your second sketch. I thought you literally broke the model into two slices (to later be glued together), but you were trying to apply two MeshCAM slices to the one job? That would present a couple of difficulites. The lower slice would need Retract Height high enough for the tool to retract up past the geometry MeshCAM didn’t know was there. And I think that even with Don’t Machine Top of Stock selected, the ball-end mill would wrap up around the top corner where the geometry came to the top of the stock. That’s just a geometric thing becasue the upper part of the sphere isn’t there for MeshCAM to stay tangent to.

But other than that, I think you could try that method. If you have zeroed the Z on top of the actual stock and know how thick the MeshCAM slices are, you could reset the Z zero by going into Set Zero in Carbide Motion, clicking in the Z readout and typing in an edited value.

But that’s all theoretical–I think just doing two jobs as I suggested above would be much more straightforward.

But…it never hurts to go through mind experiments and poke the envelope–something useful might turn up.


@pjhof, thanks for the pictures. Now it makes sense.

@Randy has this under control. he also advocated a longer end mill. :smile:

I was advocating doing a half sphere from the top, machining away all of the stock but the sphere and the construction tabs at the bottom. Not even having slopes.

All one needs is a long enough effective end mill. Without an end mill like that, slice the job in CAD into two halves - slicing - and machine away all of the stop except for the construction tabs at the bottom. Repeat, as necessary, until all of the parts of the sphere are done. Cleanup and assemble.

Thanks Mark, I’m about to take another swipe at this bad boy.

Randy, I actually did adjust the retract height & selected don’t machine top of stock, so I was feeling pretty good about myself, but alas, it was hubris :smile:. I think it might have worked had I only altered Z and nothing else.

I’m going in…