Bit Choice for Routing Hardwoods with CNC

Experienced hands provide tooling advice. August 30, 2005

We need to rout cutouts in 3/4" thick solid oak and hard maple on our Weeke BP60, similar to a cabinet end panel's toe space notch. What type of router bit is recommended (HSS or carbide, style, etc.)? Can I expect to do this in a single pass? Mirror finish is not necessary, but the cut edge should be fairly clean. Suggestions on feed rate and spindle speed would also be appreciated.

Forum Responses
(CNC Forum)
From contributor E:
Try using solid carbide up/down compression. Slow your machine down and take smaller bites. We run alder twice as fast as the maple.

From contributor M:
I would use solid carbide up or down cut finisher depending on your machine set up. Keep the rpm's around 12-14,000 and feeds 175-350 ipm depending on the species. Contributor E is right about the quality of Vortex. Here is the website below.

Vortex Tool

From contributor A:
Another thought is Onsrud's Hogger series. Another options is Courmatt's Ruffer series – it cuts solid wood easier but leaves a series of lines. In some cases we can leave this (as in the case of a toekick type notch or rough in pocket we are quite happy with this finish), and other times we use the Hogger/Rougher as a stock removal tool when we plan to follow up with a profile pass . We have used these tools for cutting decorative corbels several inches thick, and take the cut to a pump sander and remove the small lines very quickly.

From contributor B:
We cut our pod held hardwood curved mouldings at 150 to 200 ipm with a spindle speed of 18,000 rpm. 18,000 rpm is a bit fast for that feed rate, but we run at that so we won't blow the mouldings off the pods. As a result we go with HSS downcut spiral 3/8" bits rather then a corresponding carbide bit. I've found we get about 40 mouldings out of the HSS and about the same out of carbide. HSS stands up to the heat buildup better the carbide.

From contributor J:
I've started using 1/4" spiral and use multiple passes about 1/4" deep per pass. There is a lot less pressure on the vacuum hold-down and a whole lot less chipping.

From contributor B:
I neglected to add that we cut 15/16" to 1 1/8" material in one pass with the settings stated above.

From contributor C:
We use 3/8 carbide downshear at 13k rpm/300-350 ipm in hardwood. I usually write to take 1/4" deep passes. The bit is loud (high-pitched). I've tried varying speeds and changing collets/holders to no avail and have just been living with it.

From contributor T:
One thing I've learned is to use bits with just enough cut length for the material you are cutting. I sometimes cut 1 3/4" material so I ordered bits with 2" cut length. These are not good for cutting 3/4" material.

From contributor S:
For solid woods we use my favorite tool, a 30mm insert cutter with 30x50 inserts. At 15000 rpm and 8-12 mpm (200-300 ipm) we cut 3/4" deep. We usually cut 1.5" thick stock, so two passes usually does it. We’ll go with three if we’re worried about pod power. The tool might seem like overkill, but we get good tool life and great cut quality every time. With 30 mm diameter there is no deflection so it's quiet. This tool is the tank that goes through anything.

From contributor S:
If I need a small radius I follow the 30mm with a 3/8 compression or a 1/2" hog cutter like mentioned before. The serrated hog cutters cut fast if you can live with some lines in your finish cut.

From contributor G:
We have developed a slow helix ruffer that leaves a finer edge finish than our fast helix tools and there are virtually no lines at all. Depending on your part size (toe kick 4x4) feed speeds will be slow. We go with 250IPM @ 12000Rpm's in a single pass. Maximum feed to date is 200IPM @ 24K cutting MDF, PB and ply's, 1" and under. On 1 5/8" Plywood (hard) firms are achieving 1600IPM @ 22K, all with no lines.