Using the Nomad to machine 2D parts

Our intention is to use the Nomad to machine parts from a thin piece of ceramic stock. The ceramic is ~.030" thick, relatively soft and is self lubricating. The parts we typically machine are round and between 1" and 3" in diameter. Many times there is an array of holes around these parts. Some of these comments or questions are directed at the Nomad, Carbide Motion and MeshCAM. I’m hoping we can address them all here.

What we’ve found is, on the 3" diameter parts machined on the Nomad, the OD varies by .010" to .012". We’d like to keep this at .005" or less. Our tolerance is set at .0001 in MeshCAM when generating the G code. The feed rate is set at 4"/minute. We are machining the .030" depth in two passes. Is there anything else we can do to reduce the variation for the OD dimension?

Also, we machine an array of holes along the outside edge of these parts. What we’ve found is that if the hole diameter is less than .037" MeshCam doesn’t see them. We’ve had to change the diameter of the holes on our models in SolidWorks so MeshCAM can see them and then we spot drill them in the correct diameter. We export dxf files from SolidWorks 2014. Are we doing something wrong that is causing MeshCAM to ignore the smaller holes?

Generally MC failing to recognize holes is too coarse an STL (i.e. not enough “sides” to the hole). Try a smaller angle in your SolidWorks STL export settings.


First, I’d look at the part in MeshCAM to make sure it’s being exported from Solidworks at the correct size. After importing the file, click Geometry->Properties to check on the overall size of the model. Is it approximately 3" give or take a thou? If not, it could be the the STL is too coarse from Solidworks.

If that’s ok, can you create a 1" square (Bigger might be better to magnify the potential error) in Solidworks and machine it in something soft like wax and measure it. If it’s off by a similar amount, I can tell you how to apply a “correction factor” in the machine config to scale the units.

Regarding the holes, Randy it right. Be sure to increase the quality of the STL coming from Solidworks to get them recognized.


Thanks for the suggestions. Because the parts we machine, for the most part, will be 2D, we have been using dxf files (vs STL).
Going to the STL file conversion fixed the missing hole problem. Regarding our elliptical hole issue, we machined a part using an STL file. The part should be 2.030” OD and 1.610 ID. The dimensions in the Geometry/Properties window match the 2.030” max.

The actual part was:
2.032 OD in the X direction
2.039 OD in the Y direction
2.034 OD at 45 degree angle from either X or Y
1.606 ID in the X direction
1.610 ID in the Y direction
1.607 ID at 45 degree angle from either X or Y

We machined a 2.5” square. The Geometry/Properties were right on at 2.500.

The actual part was:
2.503 in the X direction (both top and bottom edges)
2.512 in the Y direction (both right and left edges)

The deviations from 2.500" are not the same which explains our ellipses. I’m guessing a single correction factor will apply to both X and Y?

We can change the X and Y independently so it won’t be a problem. I’ll type up a procedure for you on Monday.

Do you have a serial terminal program that you use or would you prefer to do it in Carbide Motion (slightly more complicated)?


1 Like

That’s good news. We will have to make the changes in Carbide Motion unless you can recommend a serial terminal program that would make sense for us to have.

Any progress on the X and Y correction?

Anything you can do to get us the procedure for adjusting the X and Y dimensions/units would be greatly appreciated. It would be extremely helpful for us to get this corrected so we can start making parts.

1 Like

Here’s a PDF (sorry for the formatting). If you can follow it, I’ll upload it to the website for others as well.

Calibrating the X and Y.pdf (153.8 KB)



Many thanks Rob.

I was able to adjust the dimensions. Now when machining a 3" square the machine is right on in the X direction and within .002" in the Y direction. I may try to tweak the Y to get it right on but thought I’d reply so you know this worked.
A couple of things that may be obvious but I’ll mention them. After you start CM and connect to the Nomad, The Load Project and Move Cutter commands are in the CM window. You can type L to open the log window and it opens up over the top of the CM window. You have to activate the CM window again to type in M and when you do this make sure you are either to the left of the Load Project command or to the right of the Move Cutter command. It is easy to activate either of these commands which takes you places you didn’t intend. When in MDI mode the commands are entered on the turquoise line to the left of send. You have to click above the line to activate it to type in the command. When entering the new factors I typed them in and they did not show up in the log window. You have to type in the new numbers and exit MC and then go back in and the new numbers will appear.

The adjustment I made is as follows:

Original 1” Machined Square

88.889 (factor used from factory) = 1.0012" 1/1.0012=.9988 88.889 X .9988 = 88.782 Final dimension = 1.000

88.889(factor used from factory) = 1.0048" 1/1.0048=.9952 88.889 X .9952 = 88.464 Final dimension = 1.0006

I replaced the 88.889 with 88.782 for the X factor and 88.464 for the Y factor.

Ready to roll now!

We machined a test part this morning with the new X and Y factors. The part was a disk with an OD, ID and had an array of holes. We used a .035" end mill to machine the part.

The OD of the part from CAD - 1.295
The machined OD was 1.296" in the X axis, 1.292" in the Y axis

The ID of the part from CAD was 1.000
The machined ID was .995" in the X axis, .994" in the Y axis

The diameter of the holes in the array were to be .042, the actual was very near .037"

It appears there is an error in the offset for the tool. I double checked the data for the tool in MeshCAM and everything was in order. This may have contributed to the dimensional error when machining the previous test pieces.

Is there a way to correct this?

It’s unlikely that MeshCAM got the offset wrong unless you made the tolerance much bigger that the normal .001" value. If you have memory, you can move it down to .0001".

Internally, MeshCAM is more accurate than almost any milling machine.

  • Make sure the tool is defined correctly in MeshCAM (one more time).
  • Measure the tool just to make sure it didn’t get switched at some point. Is it .035"
  • Make sure you run a waterline pass. If you’re only running parallel passes then the outer dimension could be off by up to the stepover value.
  • Slow down the cut a bit. There could be some flex in there causing the dimensions to be off. This is an issue even in our 8000 lb Haas mill
  • Regarding the holes, I’m not sure how round they’ll end up being given the tiny arc that the tool must follow to cut it. It might be better to try to drill them since they’d be within .002" of final size and probably be more round.

Finally, it’s unlikely that every part will be exactly the designed dimension. We’ve generally told people that .003"-.005" or so is about what to expect although you can do better depending on time, material, tooling, etc.


1 Like

Thanks for your reply. My answers to your bullet points:

  • I checked the tool definition again and it is correct.
  • The tool measures .035".
  • We machine the part using the waterline pass and pencil cleanup.
  • We’ve run the program twice for the same part where, when we run the program the second time, nearly no material is being removed. There should be no flex on the second pass as it is not removing material and the dimensions were
    virtually the same.
  • The reason we had the program interpolate the .042" diameter holes was to check the accuracy and the offset issue. We used a gauge pin to check the diameter. We can and will spot drill the array of holes.

If I tell MC I am using a .030" tool and insert a .035" tool the parts are machined correct dimensionally.

More questions:

In MC, after creating the toolpath, I turn off the waterline finishing to look at the pencil finish toolpath and they are superimposed on each other. There is no offset. Is that correct?

Given we are machining ~.040" thick material, in MC, is there a stepdown number we should be using in the waterline options? Could this stepdown number affect the pencil clean up? Our stepdown is currently set at .030. How about the number for the maximum depth per pass in the tool definition? We are currently using .030". We are cutting at a max depth of .055".

What tolerance value were you using?
Can you post a photo of the part?

What material are you cutting? That is a big factor in determining the stepdown to use. If the stepdown and max depth match up, then the pencil may overlap the waterline. (Exact behavior depends on the geometry).

The values in the tool definitions are just there for convenience to automatically copy them over when you change to a new tool.

We have the tolerance set at .0001

We are cutting boron nitride. This part is 1.295" diameter.
The material is pretty easy to machine and self lubricating.

I believe we could cut the full depth of .035" but we have chosen to set the stepdown at .030" thinking the second pass would be more accurate.

The stepdown is .030" and the max depth is .055". Should the pencil toolpath be ~.002" to .0025" offset from the waterline toolpath?

Should the pencil toolpath be ~.002" to .003" offset from the waterline toolpath?

Any thoughts/suggestions as to what we might try? It would be helpful to know if the pencil toolpath follows the waterline toolpath or is it offset some as a finish cut?

Can you tell us what settings you would use to cut the part?


The pencil path should be within the tolerance value you defined for the toolpath (assuming a vertical wall).

I can’t find much about the machining parameters of that material but if I call it “Hard Plastic” and load some info into GWizard I get the following:

.035" cutter: 10000 RPM, .025 depth, 4 inch/min
.125" cutter: 10000 RPM, .03 depth, 7 in/min

The cut above assumes a flute length of .2" for the smaller cutter. In both cases, the speeds and feeds are limited by the flex of the cutter, not the spindle power.

Again, I’m assuming it’s something like ABS or Delrin so you can adjust if you think I’m way off base.


Thanks for the info. I wasn’t sure if CM was somehow omitting the pencil toolpath and leaving the part slightly larger (if the pencil path was offset from the waterline path). So now I’ve tweaked the units in CM a bit more and the parts are now within .001" both X and Y.The material is pretty soft so I’ve backed off on the spindle speed to 8000 RPM. The feed and depth numbers we are using for the .035" cutter are 4"/min and .028 depth which are very close to what GW gave you.