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 wonât 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 Iâve 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 youâd 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. Youâve 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.
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 wouldnât 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. Itâs far from rocket science, there are good tutorials and people can help (like me). Itâs 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 canât 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 youâre 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 isnât too expensive.
Please understand that Iâm in no way slamming MeshCAM - Iâve used it for projects myself. MeshCAM is awesome! Itâs just not the best CAM tool for all kinds of machining requirements.
Hi spongefile, to add to what @Randy and @mbellon have said, Iâd offer the following:
-
Have you looked at Fusion360 yet? The CAM kernel is the HSMworks kernel, so itâs very good CAM software for an amazingly cheap price and/or free, depending on whether you qualify for any of their promotional rates. Itâs very easy to set up multiple operations with different levels of âqualityâ 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 youâre working with ball-milling, because different cutting methods will give you a better surface finish in different situations with less machining time than others.
-
That brings me to what I think youâre really asking aboutânot 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 âroughingâ strategies only where you donât need a smooth surface, and then put finishing passes only on what mattersâto do this in MeshCAM youâd 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 thatâs slower and less aggressive and which will leave a better finish. In Fusion360 or other CAM packages, youâd just add another machining strategy to the list to do the finishing and when youâre done setting it up youâre exporting just one g-code file that has all the machining steps back-to-back. For example, hereâs the machining tree of a project Iâm working on:
You can see that there are a bunch of different operations all running one after the other in each setup. -
The other point Iâd make about finish quality, is that if youâre 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. Iâve been tracking it for some time. The CAM allows for complex machining and wickedly fine finishes. Iâve 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 didnât have access to high end CAM. Itâs an excellent package supplies high end CAM approaches at an accessible price - albeit manually. I use it still because itâs approach makes sense for some jobs.
MeshCAM I use for simple jobs, jobs I donât 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, âprofessionalâ Fusion 360 lacks the ability to 4 and 5 axis continuous machining but thatâs 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.
Iâve 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, itâs 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, Iâm using Fusion360 almost exclusively and Iâm 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. Iâve 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 itâs 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.