Hey all. Thanks for the help so far. My machine arrived and is all assembled and I cut my first path today. Using a piece of junk pine, quarter inch 2 flute upcut bit. Is this mess a result of the bit or speeds and feeds?
Hey Scott,
depends on what you wanted to make. If it was a battlefield, nice! 
An upcut bit can cause wood to tear out. Especially for plywood and veneered wood, but also for wood in general, there exist downcut bits or bits like this one which has very steep upcut spiral angle of 15°, which is a compromise between the ability to evacuate chips and trying to minimize tearout at the surface:
Also when milling wood, you want a high rotational speed of the spindle.
3 Likes
Hey Scott,
can you please in the future use the “Reply” button to reply.
LOL! Yes, a battlefield! Hey - I didn’t burn the bit or the wood, and no crashes so I’m calling it a succesful maiden voyage!
FWIW, it was solid pine (not ply or veneer). It was the Myers SRF4-250UP that came with the starter kit. I was running Makita low speed which I believe is around 10k, using 200ips feed, and 0.25 cut depth.
- If I’m initially profiling pine, is bit or settings my main issue?
- Does that answer change for MDF?
- Do either of those answers change for 3D cutting?
Lastly, is there a go-to reference for speeds & feeds and the like for various materials? I don’t want to be pesky with all these questions if I can find the definitive guide. So many of the answers I find when looking have little or questionable feedback.
Thanks!!
Hey Scott,
FWIW, it was solid pine (not ply or veneer).
Yes, I know. Anyway you have a lot of tearout which is not uncommon with an upcut bit.
It was the Myers SRF4-250UP that came with the starter kit. I was running Makita low speed which I believe is around 10k, using 200ips feed, and 0.25 cut depth.
- If I’m initially profiling pine, is bit or settings my main issue?
- Does that answer change for MDF?
- Do either of those answers change for 3D cutting?
Lastly, is there a go-to reference for speeds & feeds and the like for various materials? I don’t want to be pesky with all these questions if I can find the definitive guide. So many of the answers I find when looking have little or questionable feedback.
Yes, the WWW is full of the information you demand for. You could search and find a list of speeds and feeds calculation table for different materials to start with. Please understand I can’t offer a CNC for beginners course at the moment. Usually you got to take a greater amount of time to learn this, especially if you are not already a skilled woodworker who just switches from a manual router / table router to a CNC machine.
1 Like
I swear that’s what I did. Obviously, something went sideways. Sorry!
What a weird forum… Why in the world would any group let people edit posts made by others!!!
I don’t think it typically does. I see I can edit @Aiph5u’s posts in this thread but not yours.
This is the first time I’ve seen this behavior on this or any other forum. Perhaps there’s something special about his account settings.
I’ve checked some other threads with other posts and it’s just @Aiph5u who seems to be affected.
I’m not asking you to provide all the answers. Just throwing it out there for anyone interested in weighing in.
And yes I’m well aware of the WWW. I see lots of forums with “RTFM” or “search the forum”. I’ve done that, but I see lots of replies that say “RTFM” and “search the forum”. See my dilemma? The other issue is finding answers that don’t have followup by the OP, so I don’t know if they were good answers or not. I only say this to respond to your answer.
I do have moderate woodworking experience as well as a background in 3D modeling and CNC programming, so none of this is completely foreign to me. I’m just casting out a net in case someone has a 1F or another resource for this stuff. I have no trouble spending the time learning - I just want to learn the right stuff! One thing I’ve found in my brief experience with 1F is that there’s a lot of info out there but it’s poorly organized.
Thanks for your help!
Scott
I’m glad to hear that’s not normal behavior! What a bizarre “feature”.
And if it’s just @Aiph5u … he has my condolences!
Hey Scott,
I use mainly books. The profession “Zerspanungstechniker” in my country, which means something like “Milling, turning and sanding machinist”, takes three years to get the degree. I use the books for this training for the tables for speeds and feeds, together with books for the “Machinery engineer” and “Electrical engineer” studies for the spindle / VFD matter.
But I know that there are many good web pages and video-based courses on the web, but I think others have a better overview of these resources.
I know that my CNC parts supplier, Sorotec.de, has a Speeds and feeds calculation table in english. They also have a Table for what type of bit to use for which material.
1 Like
Awesome. That gives me a place to start. Thanks!
Usual preface, I’m with PreciseBits so while I try to only post general information take everything I say with the understanding that I have a bias.
Just to clarify what you are seeing here is not tear out (mostly) but a lack of shear. Tear out is where there is a material failure for the force being applied to the material and a piece “tears out” instead of cuts. This is a lack of shear where the unsupported material avoids getting cut by the tooling. You can increase the shear by increasing your RPM or using a cutter with higher rake or a higher helix. The higher helix will make the likelihood of actual tear out greater though as you will be shifting more of the cutting force up into the spindle direction.
Pine in general is notorious for being a poor finishing wood. It has a large and soft grain structure which usually requires more aggressive tool geometries to cut cleanly. You can cheat some by sealing the wood before cutting as that will make the top surface harder and easier to cut with less aggressive tooling.
There are no real go to feeds and speeds charts or tables out there. The problem is that all cutting is a combination of failure points that change for every user. The material, system and tooling all change which is that failure point and where the best feed and speed is. I’ll briefly go into each.
Every material will have a minimum chipload that will need to be hit to actually cut a chip out of it. If you cut under that minimum the chip can’t support itself and the tool will push or “rub” the material away instead of cutting. That can generate a lot of heat and is the reason that you will see burning or discoloration in the wood. On the other end you can get tear out where the cutting forces get so big that the material gets ripped out from the force on the chip being made instead of the tool cutting it. In wood this is especially user specific as even with the same wood the trees are variable and things like moisture content in the wood changes how it cuts.
On the system side you will usually be limited by the rigidity of the machine. As your cutting forces increase (more depth per pass, higher chipload, larger diameter, or larger stepover) you apply more force to the machine. Since everything is a spring this will start to bend the machine into the cut, how much depends on the forces and the machine. This is usually referred to as deflection and can effect both the finished dimensions and the cut quality. This happens in ALL machines and ALL cuts. There are other things machine specific like runout and hold down that can effect the cut but I’ll stop here for now.
Tooling I’ll be fairly generic on since I have a greater bias here. There are a lot of different features of tooling that are usually not spec’ed that can greatly effect the tool. 2 that I already talked about are rake and the helix. The rake of a tool is the attack angle of the flute and the more aggressive the rake the “sharper” the edge of the tool. That usually comes at the cost of making the edge weaker. A higher rake tool will produce less force, need less chipload to cut, and effect the cut quality in ways dependent on material. The helix is the twist of the flutes. As I mentioned before this changes the direction of the force and the tighter the twist the more the force change. Additionally, like for like the higher the helix the weaker the tool as flutes are functionally closer together leaving less mass. There are other things in geometry like flute volume, core, relief, etc but I’ll stop here unless there’s more interest.
The other common thing not listed in tool spec is the carbide grade. In a like for like tool this will effect how quickly it dulls and how strong and resistant to deflection the tool is. These are not the generic “grades” you see like sub-micron but things like Sandvik DH20, or Mitsubishi MF20. Both of those being under ISO K20. These go into things like transverse rupture strength and rockwell hardness. Again though I’ll stop here unless there’s more interest.
Hope that helps, let me know if there’s something I can expand on help with.
4 Likes
This is all very helpful. Thanks! I have just enough background to understand all this - at least in principle. This helps me to understand what the variables are and where I need to spend time experimenting.
I understand I need to learn about these variances as a general principle, but that makes me wonder about professionals who use this in production. I would think there is enough consistency that, for a given material in their shop, they know which tool, speed, etc to use for a given task … right? I can’t imagine needing to proof every time you cut. Would you say there are guides out there that give these starting points? (For example, I know I need to be aware of the factors on each cut, but I’m going to approach cutting P20 differently from 4140 or brass when selecting the tool, feed rate, etc. because there are guidelines. Wouldn’t the same general rule apply to pine vs mahogany vs plywood?)
Just thought of another question.
I grabbed some scrap pine for my first cut because it’s soft and cheap, and I have a lot of it. Given what you’ve said, I wonder if that’s a poor choice for me to start with. If not pine, what should I be learning on? MDF? Plywood? Maple? Please don’t say something like Purple Heart.
Hey Scott,
much of the experience you need to get here is not CNC-specific, but about milling wood. First this is woodworking. So since woodworking is in a steady revival both in the DIY but also in the professional context, there are tons of books and videos and web pages on it. E.g. I have worked with wood since my childhood (we had a small woodworking workshop in our house) but in the last twenty years, I worked on wood exclusively with hand tools. No power tools, no machines. When I began with this, by using chisels and gouges, but also hand planes, it was the first time that I really “felt” how wood is to cut, and that you cannot do good woodworking without a relatively good knowledge about steel, and that you need a sharp edge to work on wood.
Woodworking with a router is different, and especially with the advent of High speed steel (HSS) you have sharp edges that do not get dull when they get hot (as hardened carbon steels do), so in cabinetmaking, the industrialization went on since the 1950s. But there are sectors where the nearly exclusive work with hand tools remains, e.g. violinmaking, but also carpenters know how to use a chisel.
Now the third step of evolution is from a hand router or router table to a robot (that’s what a CNC router is), and it brings a few new aspects to learn, but I think when you use a CNC to mill wood, most of the task requires the knowledge about how to use a router and its milling bits. The CNC brings aspects like a feed rate and other cutting parameters that can be much superior to what you can achieve with a hand router.
1 Like
I’ve worked with a lot of production shops and in general they do testing. They are looking for the highest production number and/or the best finish. So they will usually spec a tooling source and test for the best numbers. I know that may seem insane but the faster you can run a tool before you either exceed you machine, material, or effect cut quality the longer that tool will last (the higher the chipload the less impacts to the edge to complete the same length cut… on top of reduced heat). They are also usually controlling a lot of other variables too like shop humidity and material suppliers. Once they have those numbers though they can run for a while and potentially apply formulas for other similar materials.
In some cases you will find feed and speeds or chipload charts from a tool manufacture. Unfortunately even for production shops with 6 figure machines these aren’t very useful. Every tool manufacturer has to make a decision on how to make these. These vary from testing which makes them machine dependent, to formulas which are problematic for a multitude of reasons, to extremely conservative numbers which are leaving a lot on the table for tool life and cut quality. Ones for metal are a bit better as it’s much more consistent, has a lost of research, and often the tool is the limiting factor (assuming your aren’t deflection limited).
There’s some general rules of thumb that can be used for low end to prevent rubbing. As an example in soft material I would never cut with less than a 0.002"/0.05mm chipload for tooling over 0.0625". For 1/4" and above I’d usually double that as a minimum. For woods with similar grain structure you can also use their janka values for some off the cuff numbers.
For metals in almost all gantry machines you are deflection limited. So those become more of a force issue trying to hit something within the material minimums usually biasing on the pass depth and tool diameter. Some of that changes with adaptive as you are functionally using chip thinning for a higher pass depth.
Sort of, there’s a lot more variation in wood. The hardness (janka), grain size, and material integration change it more than most materials on top of the previous mentioned tree variation and moisture content. As an example you might be able to apply a set of constants in domestic hardwoods with similar grain structure using the janka values. However, once you start dealing with more exotic woods like rosewood or ebony that all goes out the window. Those woods integrate silica into them which makes it functionally cutting almost a composite.
MDF can be good as it’s much more consistent than woods. However, it’s also a lot more abrasive so it can eat tools faster (some worse that other depending on MDF quality). Maple is a good tight grained wood that finishes well and a lot of people use that for baseline info.
The other thing to keep in mind is that until you start talking about micro tools, exotic woods, or larger end-mill you have a lot of margin. While it might be necessary to run tests for the best finish or the most tool life you don’t need to hit that all the time and is probably counter productive if you aren’t going to be running the same thing over and over. Short version is after getting some basics down you can run a lot of stuff without “optimal” settings.
Pick some woods to work with that are decent finishing and start playing with numbers. Once you have a good idea of what works keep the previous post in mind for what and how things might change. If your wood is harder than you might need to reduce your chipload/feed to get the same deflection or you might be able to increase it if your issue was tear out. If you change tools keep in mind the rake and helix difference as those can also change how you are cutting and where you are putting the forces.
Let me know if there’s something I can help with.
1 Like
Again, very helpful. I’ll be rereading this as I work through my testing. Thanks!