Different tolerances for different areas?

Does toolpath software exist where you can define very precise tolerances for one area of a piece (say, the area that needs to connect to another part) and then rougher tolerances for the rest of the piece so the milling process overall takes less time?

Tolerance per se won’t affect machining speed. In fact, on 3D contoured parts a tighter tolerance can possibly increase overall speed by making the toolpaths smoother.

But you can effectively change machining resolution on a part. Machine the whole part with coarse stepovers/stepdowns for the finishing, then use Set Machine Region to isolate the area(s) you want to machine more closely, and finish them with a finer stepover/stepdown. On a few 3D parts I’ve done this using a much smaller cutter for the selectively-detailed areas. .125" for the overall machining and .031 (or maybe it was .020) for the detailed area.


In that process, would you have two separate gcode files that you’d run one after the other? First the roughing, then the finer run with Machine Region isolations applied once the roughing has stopped?

Exactly so. Do the roughing and coarse finishing with one gcode, then go back and define the machine region, set up the finer finishing parameters and write a second gcode file with just the finishing. You’ve already imported the geometry and defined the stock and set the program zero so it is easy and fairly quick to play around with the machining parameters.

1 Like

Yes, SharpCAM can do that. Each cut can have a tolerance - offset from the ideal - so you can achieve what you are asking for. Speed wouldn’t be largely affected; finish is very tunable though.

It is common to do 2, 3, 4 or more operations on a feature adjusting the tolerance, feeds and speeds and so forth (e.g. hog (FAST rough), rough, surface finish, pencil finish).

SharpCAM is a higher end CAM program with a steeper learning curve than MeshCAM. It’s far from rocket science, there are good tutorials and people can help (like me). It’s takes a bit of getting used to… and then you rock!

I have a Nomad 883 Pro on order. One of the first things in my agenda is to write a Nomad post processor for it and have it picked up by the author for the next release (we cowrote a post processor for CAMaster machines). I will make the post public if I can’t get it in the official release.

By-the-by, many of the high end CAM programs can do this. The high end and super high end CAM programs look at everything you’re asking for and optimize the cutting for finish, minimal tool changes, minimal machining time and so further. Then they generate the G code. The generated G code is a sight to behold!

SharpCAM is somewhat unique in the it offers variable tolerances and an easy way to have multiple operations per feature at a price that is way below the big boys. Of course you have to set up the operations yourself; the automatic optimizations and reordering is why the big boys are big $$$$$ - and SharpCAM isn’t too expensive.

Please understand that I’m in no way slamming MeshCAM - I’ve used it for projects myself. MeshCAM is awesome! It’s just not the best CAM tool for all kinds of machining requirements.

1 Like

Hi spongefile, to add to what @Randy and @mbellon have said, I’d offer the following:

  1. Have you looked at Fusion360 yet? The CAM kernel is the HSMworks kernel, so it’s very good CAM software for an amazingly cheap price and/or free, depending on whether you qualify for any of their promotional rates. It’s very easy to set up multiple operations with different levels of “quality” by adjusting the step-overs/step-downs between different operations, or doing different parts of your model with different machining strategies entirely. This really shows value when you’re working with ball-milling, because different cutting methods will give you a better surface finish in different situations with less machining time than others.

  2. That brings me to what I think you’re really asking about—not really tolerances per-se, but finish quality. How do you reduce cutting time and go faster, and still get precisely what you need where you need it, right? You can take more aggressive cuts and just do ‘roughing’ strategies only where you don’t need a smooth surface, and then put finishing passes only on what matters—to do this in MeshCAM you’d want to create separate g-code files and then run them back to back, with a roughing pass going over the whole model but leaving a bit of stock behind that you clean up with a finishing pass that’s slower and less aggressive and which will leave a better finish. In Fusion360 or other CAM packages, you’d just add another machining strategy to the list to do the finishing and when you’re done setting it up you’re exporting just one g-code file that has all the machining steps back-to-back. For example, here’s the machining tree of a project I’m working on:

    You can see that there are a bunch of different operations all running one after the other in each setup.

  3. The other point I’d make about finish quality, is that if you’re doing curved surfaces you want to use the largest ball mill you can that will adequately fit into the crevices and things in order to flatten out the surface and have the lowest cusps. A larger ball mill with the same step-over as a smaller one will give you a better finish.

Hope that helps!


Yup, the fancy CAM packages one just adds strategies to features - the software deals with the complexities for you. UnionNine reinforced what I was saying - thanks!

MeshCAM is very good at what it does but it takes some really noodling to make it do 8 or 10 passes that are natural and relatively simple in the more complex CAM packages.

Fusion 360 is really, truly getting there as a major force in CAD/CAM. I’ve been tracking it for some time. The CAM allows for complex machining and wickedly fine finishes. I’ve played with it and been pleased.

Price wise it is hard to beat, even paying for it annually. They constantly update it. Traditional packages are initially expensive and have costs per year that are larger than the total cost of Fusion 360 per year.

I have SharpCAM because, at the time, the could afford or didn’t have access to high end CAM. It’s an excellent package supplies high end CAM approaches at an accessible price - albeit manually. I use it still because it’s approach makes sense for some jobs.

MeshCAM I use for simple jobs, jobs I don’t need to think too hard about. It is wonderfully simple and can make pieces with little thought and good finish.

I use Evolve for CAD (think Rhino on steroids) because I like it better than the CAD portion of BobCAD-CAM.

For me, “professional” Fusion 360 lacks the ability to 4 and 5 axis continuous machining but that’s about it. I can easily see dumping all of my tools and switching to it once I have a single package that can do all I need.

1 Like

I’ve been following this Fusion 360 thread: Fusion 360 for the Nomad

and am trying to figure out whether to jump into Fusion tutorials now, or wait till the workflow is more solid. So many comments in there now, it’s not clear to me whether there are still bugs after export or no, does it play nice with the Nomad natively or is it a bit toothpicks-and-glue.

I am CAMing in Fursion360 for the last month and it works fine with carbide3.cps post processor (GRBL).
I like it better than MeshCAM right now because Fusion360 is more complex. And I am complete CNC noob and like to experiment with all the strategies and chiploads. And it nice to have it in one package close with modeling functionality.


Hey, I’m using Fusion360 almost exclusively and I’m a newbie never-before CNC guy before I got the Nomad. I would say it works just fine 99% of the time as long as you remember to 1) post using mach3 2) turn off useg28 3) Turn off useradius 4) post in mm. I’ve only run into one weird bug that I never could track down in a single very long job where I had to end up going in and replacing a bunch of itty bitty vertical arc commands with linear moves. Aside from that one job it’s been rock solid.

For me the modeling part of fusion is also a joy to use, and being able to make a simple 3d pocket pass to cut your piece out all at once OR make a complicated set of roughing and then contour and parallel and pencil line and facing passes to get a better finish and then save all that work in the same project file as the model is pretty awesome.

1 Like