Anyone also using CNC?

Longtime FF user myself using Sketchup for design and Simplify3D for slicing and gcode generation. I finally took the plunge and placed an order for a CNC router to enable me to make some things the FF isn't suitable for. If any 3ders here also have experience with CNC routers, I was hoping for a little discussion to help me wrap my head around the differences in how both machines build objects (or in the case of CNC...subtracts).

As far as I can gather from my research, gcode that is generated for a 3D printer isn't going to work on a CNC machine without some modification. I'm assuming this is due to the fact that a program like Simplify3D doesn't have inputs or settings for things like tool type or size. Not only that, but the toolpath is going to be a lot different because it has to move around an object that's already there (say a block of wood that's being carved) as opposed to 3D printing where there's nothing there at the start of the build.

One other question I had that I don't seem to find referenced anywhere in discussions concerning CNC machines concerns the original carving object size. I assume there has to be a way to tell the machine what you're starting with, but I can't find mention of this process so far. In other words, if I'm carving a 5 x 5 mm cube from a block of wood that is 10 x 10 mm, there must be a setting somewhere to tell the machine what I'm starting with?

Sorry for the off topic. I know I could post this on some CNC forum, but I thought it'd be easier to try here with other FF users first. :)

I own a FFCP and an XCarve CNC machine. They're both great and similar in a lot of ways. I would check out the XCarve forums (regardless of your CNC machine) to learn more about how they work and also to find answers to your questions. It's a very helpful and active forum.

Quote:

---

Originally Posted by GammaRays

I own a FFCP and an XCarve CNC machine. They're both great and similar in a lot of ways. I would check out the XCarve forums (regardless of your CNC machine) to learn more about how they work and also to find answers to your questions. It's a very helpful and active forum.

---

Will do. Thanks for the advice!

That's correct. The gCode generated by Simplify3D will not do a lot of useful things on a CNC. It is the same code language, but 3D slicing programs output different kinds of tool paths because of how 3D printing is typically done. The commands are the same between 3D printers and CNC machines, for the most part, when using gCode. However, there are particular commands you would only use on a CNC machine (spindle speed, tool change, etc.).

The CNC equivalant of S3D is one of a number of CAM (computer aided manufacturing) programs. Essentially, CAM = Slicer, when comparing CNC and 3D printing. You import whatever object you want into the CAM program and it decides how to move the CNC machine to give you your final part. Fusion 360 is a great CAD + CAM software package that you can get for free. I personally use a CAM plugin for Solidworks called HSMWorks, which I enjoy a lot. You can define your stock material size and can even use other parts as your stock. That allows you to machine a new piece from an existing part (for revisions to parts, or just recycling unused parts).

There are two general types of programming for CNC machines: conversational and manual. Manual programming is entering each line of gCode by hand, which may be fun to learn but is generally not needed. Conversational programming is just using CAM software to have it generate the gCode for you, like S3D does for your prints. You'll be able to define your stock size, tool size, how fast you want to cut, what kinds of tool paths to take, and a lot of other cool things.

Had a look at the xcarve site.
And they have software that might be useful for you: https://www.inventables.com/technologies/easel

I had no idea desktop cnc machines were so affordable

I had wanted a CNC for a long time and bought the XCarve as soon as it came out. Great machine, but it's less ready-to-go than the FF prints are, so it's safe to say you should expect to tinker and fix things often.

Also, the Easel software from Inventables will only work with CNC controllers that use GRBL software, which the XCarve machines do.

Thanks for the additional advice, GammaRays. It's helpful to be able to wrap my brain around how the machines work! Those xcarve machines look awesome, and I'm thinking I might just return the one I ordered and get one of those. After reading up more on the xcarve, it sounds like another problem with the Easel software is that it's not really suitable for cutting/carving 3D objects. A lot people recommend Meshcam for such projects on the xcarve, but it's kind of spendy. It sounds like there are some free options out there I'll explore first. One major feature I'll be looking for in software is the ability to import an existing STL file and be able to output it to the CNC machine. It doesn't seem like a tremendous amount of platforms allow that, but I have read that Meshcam will do it.

That's true, Easel cannot do 3D carving in any real sense. Fusion 360 is what you want to look into. It's an excellent CAD/CAM package that is free to students and hobby users. Also, if you have a university e-mail address you can get a lot of other CAD/CAM software for free.

I do a ton of CNC programming, from 2,5 axis to 5 axis. I use Creo Parametric, PowerMill, EZ-Cam and VisualMill. I would look into VisualMill if I were you, although cost might be an issue. Anything specific you need to know?

Quote:

---

Originally Posted by Sebastian Finke

I do a ton of CNC programming, from 2,5 axis to 5 axis. I use Creo Parametric, PowerMill, EZ-Cam and VisualMill. I would look into VisualMill if I were you, although cost might be an issue. Anything specific you need to know?

---

Thanks, Sebastian. It's fascinating to think of some of the other design "doors" that will be opened by jumping in to CNC. It's a little intimidating to think, however, that most of the CNC machines that I can afford (including the one I purchased, and even the X-Carve) are definitely not "run straight out of the box" like the FF is. Software seems a lot more complex as well. That being said, I downloaded trial versions of Fusion 360 as well as Meshcam. Fusion 360 made my eyes glaze over and gave me a headache after 30 minutes of playing with a couple of imported STLs. :D Meshcam is nice in that it essentially has an "idiot" option for people like me. Input your stock and tool size and it will pretty much do everything else automatically for you. Once you get the hang of things there are also manual control/design options. Not bad, but also a $250 price tag for the luxury.

One other thing I'm still trying to understand about CNC has to do with "roughing" and "finishing" settings/tools. I'm to understand this enables you to use a bigger tool at the beginning to take out lots of material faster and then the finishing tool and settings are used for the finer detail. So how is this accomplished? Does the machine basically pause and retract at some point so you can change out your tool?

The way you handle a roughing and finishing pass depends a lot on your machine. Generally, the less you spend on your CNC the more work you'll put into doing this. It also depends on the software you use to generate your gCode. But, for your case, the machine will likely pause and retract for the tool change, like you mentioned.

A major difference between a print job and a CNC job is that a 3D print job is an all in one job. It almost always begins your part and finishes it without stopping. CNC jobs are usually done in segments. When I make an aluminum part, for instance, I do all of the CAM work in HSMWorks to go from my stock to my finished part. However, this entire job is broken up into different subsets. One subset may be finishing the top of the part, another could be drilling holes, and one could be chamfering (smoothing cut edges with an angled cut). Depending on the software and CNC you have, you can run each segment one at a time, at which point your CNC will return home where you can change out a roughing bit for a finishing bit. On inexpensive machines with free software (XCarve + Easel), the machine will automatically return to its home position after doing the roughing and wait for you to put in the finishing bit; then you tell it when its ready to start cutting again. There are some simple (but not precise) ways of changing bits, and expensive (very precise) ways of changing bits. For most hobby cases, you can get away with changing a bit and then adjusting the z-height manually to deal with the difference in tool lengths between your roughing and finishing bit. This way your machine will know the new height of the new bit and can continue cutting the original part. More expensive machines use automatic tool changes, where you tell the CAM software which bits to use and it will physically change out the bits from a reserve of bits that you setup near the machine.

Everything GR says and...

Roughing and finishing are processes. You can use the same tool if you choose it often more a case of settings i.e. speeds and feeds used for a particular workstep. For example: you can use a 10mm endmill in a roughing workstep by using a larger stepdown and stepover and maybe a higher feedrate and then do a cleanup cut by decreasing the stepdown, stepover and feedrate.

Not always that simple though as you do also get dedicated roughing and finishing tools. The bulk of my milling experience is for injection moulds. Here we would often use a 32mm Mitsubishi AJX tipped cutter to rough cut a cavity block with 2mm offset. The block is then sent off for hardening. After this the block is then semi-finished with the same cutter to 0.5mm offset but using a different grade tip. The block is finish off using a Mitsubishi ARX tipped cutter.

With wood that would probably no be necessary though.

On the hobbyist level, there are lots of options for CNC machines and CAM software. Many run from STL files, although they aren't universal in the CNC world as they are in 3D printing. But most old-line machine shops are unfamiliar with them, and mesh file formats in general. CAM programs that can handle STL files include VisualMill, MeshCAM, and DeskProto.

Industrial CNC mills (or Vertical Machining Centers) generally have automatic tool-changers, which select and load a new tool at a tool-change prompt in a single G-code program. On the hobbyist level, it's more common to write a separate G-code program for each tool, and to change them manually (re-zeroing the tool tip) when the program completes. So you might run a program for a 1/4" ball endmill, leaving a stock margin of .05", and then follow up with a finishing pass using a 1/16" ball endmill using finer step-overs, to get the fine details.

Andrew Werby
www.computersculpture.com