View Full Version : Speeds & Feeds & Tools for Cutout Profile in Wood

06-15-2009, 09:57 AM
I primarily cut metal, but I have been messing around with doing some wood projects with my CNC Mill.

My question is, in 3/4 inch wood, mainly pine and oak, what is the best tool, depth of cut, and feed to use?

I've tried several straight style router bits in 1/2" and 1/4" at high RPM (around 25,000 RPM), and also 2 and 4 flute end mills at lower RPM (around 3,000 RPM). The best overall result seems to be the 1/2" two flute (two cutter) straight router bit at 25,000 RPM with about 1/8" to 1/4" DOC and 15IPM feed, but that wastes a lot of material. The 1/4" two flute router bit (same settings) doesn't allow enough room for the chips to blow out and I actually broke one of my bits.

With the end mills, I get a lot of overheating (discoloration on end mill) and burning of the wood even at lower speeds (about 3,000 RPM). Not to mention a horrible banshee-like squealing. The mills are razor sharp, not just using my old metal cutting bits or anything.

SO, long story short, I was just wondering what tool and settings most people use for cutout profiles.

06-15-2009, 10:27 AM
Hi I usually run a rougher then a finisher just like you do on Steel most of the time. For roughing I like to use an Onsrud #60-910 I run it at 20,000 RPM @ 680 IPM and it sounds GREAT. Then I follow up with an Onsrud 60-252 20,000 RPM @ 520 IPM and it hardly makes any sound. This will only work if you don't have any radii to cut smaller than 1/4 " Radius. If so you will have to use an even smaller tool for final finish.
The reason you are getting the squeeling like a banche (I'm familliar with that sound) is your cut feed rate is too slow and you are getting too much surface contact with the tools flutes. You need a heavy chip load like .024 to .034 per tooth. The use of bits designed for Steel generally will not work because there is not enough chip clearence designed in them. The bits I mentioned above are Down Shear Bits and intended to be used on solid wood using a Climb Cut. Good luck and others may pipe in on what they are using.....

06-15-2009, 02:49 PM
Thanks for the reply! I do the wood cutting on my CNC Milling machine. Since it was designed mostly to cut metal, the max feed rate is 80 IPM. I'm guessing that you use a gantry machine with much higher feed rates than are possible with my mill.

However, the information mentioned about the heavy chip load may be useful. I'll plug that into my tool calculator and see what kinds of variations I can come up with for feed and spindle RPM. Knowing that my max feed speed is 80 IPM, I should hopefully be able to figure out the ideal spindle RPM to get the .024-.034 inch per tooth cut.

With the regular milling head attached (and not my router attachment), max spindle RPM is about 3100 RPM. Not sure off the top of my head if spindle RPM or feed will be the limiting factor. My router attachment starts at 10,000RPM up to 27,000 RPM. So hopefully somewhere in there is a happy medium that is attainable with my equipment.

I assume you use a gantry type machine (If not let me know). I had no idea that such high feed speeds (680 IPM !!!) were possible in woodworking machines. Like I said, I primarily do metal, and have only had experience with the mills. Maybe it's time to look into a gantry machine too!

06-15-2009, 02:56 PM
One more question. I purchased a Freud 1/4 inch spiral upcut bit and was thinking of using that. My question is in regards to upcut vs. downcut bits. I'm pretty new to wood cutting (at least with CNC tools), so can you explain the intended purpose of an upcut vs downcut bit?

I had assumed that upcut pulls the chips up and out, and downcut would force them downward (like a roto-zip bit). If I don't make through-cuts, would the downcut bit tend to clog the cut? Or do I just have the whole upcut/downcut thing wrong.

I really should learn more about the wood cutting aspect I guess. I only started doing wood projects because I had people asking me more about doing wood projects than metal projects right now.... Any recommended website or books for Wood CNC?

06-15-2009, 05:41 PM
Actually, high end routers can cut over 2000ipm.

With 1/4" tools, chips will tend to pack in the cut whether you're using an upcut or downcut, due to the small kerf. If you need a really clean edge on top, use a downcut, as an upcut may chip. wood grain and species can play a role here as well. If using vacuum holding, an upcut can pull the part up, where as a downcut will push the work down.

I find that I rarely use downcut's, as most times upcut's give an acceptable quality edge, and they tend to last longer, as they run cooler. Be sure to get some bit cleaner and clean any buildup off the bits often, as it'll create heat and dull bits faster.

As for your situation, try the router at 10K rpm, 80ipm, 1/4"-3/8" depth of cut.

06-16-2009, 07:25 AM
Jerry is providing some good info here. About what I was going to input. Yes My machine is a Gantry type with a 5 foot by 14 foot table. It's max feed rate is 800 IPM but it is 8 years old and the newer routers can cut, as Gerry said, over 2,000 IPM. You are probably using a vice or clamps to hold your wood blanks as you have no Vacuum. So you won't be able to cut the part free like I can. I used to run Mori Siki Milling Centers with 40 Tools and cut metal but wood is way more fun. You will have to experiment with the machines' capabilities to get good results.

06-16-2009, 11:43 AM
To hold down the parts, I am using standard hold-downs, t-slot bolts, and step blocks, but I have found the "Tabs" feature in Aspire v2.0 is incredibly useful for my setup.

I create the 3D tabs 1/2" high by 1/2" wide (on 3/4" thick material), then use a laminate trim bit in my router table to trim off the tabs. It works incredibly well.

I had been playing with creating my own gantry router machine. I had been looking at the K2 site and realized that most of the parts required are well within the reach of my Novakon NM-200.

Thanks for the info gentlemen, you have given me some ideas to play with for my wood projects. Trying to get the feed per tooth dialed in will be my first task. In metal, you slow down when there's a problem, it just didn't occur to me to speed up for wood :-)

06-16-2009, 12:02 PM
Actually, since I've been getting good info on this thread, I have another question regarding a key-hole slot bit.

My specific project is a red oak coat rack. To save on mounting hardware costs, I used a keyhole slot bit on the back of the coat rack to make a way to hang the coat rack on the wall.

Each 18" long coat rack has 5 keyhole slots (to provide a variety of mounting options for the customer). After about 3 parts (or 15 slots) the bit snapped off at the minor cutting diameter. The cutter was 3/8" (bigger diameter) and 3/16" minor diameter.

Basically, the bit plunges to 3/8 deep, moves 3/8" in the Y direction, moves back, and withdraws. Feed is set to 5 IPM (except on the withdraw). This was done in my router at 23,000 RPM. Can you make any recommendations?

Perhaps my lack of knowledge about feed rates in wood caused this problem as well, but I don't know if the bit snapped due to excessive heat, buildup of chips, or maybe it was just the cheap Skill brand bit I was using. I don't normally use cheap bits, but it was a one time production of about 30 parts, I thought it would work. I purchased some replacement bits from Grizzly, and don't really want to snap those as well, so if you have any suggestions, I would appreciate it. I have included my (truncated) GCode below.

( Home Position - Set Feed Rate)
N80 X0.0000 Y0.0000 F5.0
( First Keyhole )
N90 G00 X1.0000 Y3.0000 Z0.2500
N100 G1 Z-0.3750 F5.0
N110 G1 Y3.3750 F5.0
N120 G1 Y3.0000 F5.0
N130 G1 Z0.2500 F15.0

06-16-2009, 01:44 PM
Probably combination of cheap bit and too slow. Not sure if what you got from grizzly would be any better quality wise. I've never used a keyhole cutter myself, but you should be able to run it at your max of 80ipm. Pretty much any wood cutting with an 1/8" bit or larger should be easily capable of 100ipm. One thing you mightwat to consider is to predrill where your plunging. Plunging is incredibly hard on router bits, and creates a LOT of heat.