Smoked bit routing red oak?

I’ve been routing skateboards with my x-carve and a Bosch Colt. I’ve run all kinds of different bits and feed rates, etc and have been happy with the results. Today I was perimeter routing a .75" piece of red oak with a depth of .150, speed of 30ipm with a half inch 2 flute straight cut.
It cut well with slight chatter going across the grain. I adjusted the speed of the spindle while it was running to find the optimum speed which was somewhere around 20k rpm.
Towards the end I could smell the wood burning and when finished the bit was black on the bottom half of the cutting edge.
Is the bit smoked? Where do you think I went wrong, speed, depth, feed rate or all of the above.
Sorry for the long explanation, but I really want to understand this. If it wasn’t cutting well or seemed to be struggling I would understand the bit being fried.

Thanks for your time

1 Like

With a Feed rate of only 30 ipm you would need an RPM of about 1,000 for an appropriate chip load. 20K RPM is way way to fast, no wonder it was getting so hot.

The recommended chip load for hardwood with a 1/2 inch bit is between .019 and .021. At your very low feedrate it is impossible for most routers to spin slow enough to do a decent job with the bit and material you are using.

The recommended chip load is only .009 to .011 for a 1/4 inch 2 flute bit.

So it would be better for you to use a 1/4 inch bit at at a feed rate of 100ipm and a spindle speed of 16,500 RPM

Here is a spreadsheet that allows you to enter your feedrate and it will show you the RPMS needed for a variety of chip loads. I made the spreadsheet to show the correct speed setting for a Dewalt dwp611 router but it also shows RPM

CNC Speed Calculator.xlsx (14.6 KB)


I agree with Allen, lower your depth, instead of .150 make it 0.05. per cycle. What it does, cycles several times with higher feed rate, basically it will cut it on same time but cuts cleaner and doesn’t burn anything.

Thanks guys. This is the best forum ever:-)

1 Like

do you think my bit is ruined?

Using the chart, one of the calculations I get for using a 1/4" bit with hardwood reads 325 ipm at around 16000 rpm.

Is that even possible to do with an x-carve, meaning are those feed speeds out of the realm of it’s abilities?

It never does them any good to get that hot. I would clean it good (knock the char off it) and put it away. Using a router for a spindle means you really should not be using 1/2 inch bits anyway. Most routers are not designed to spin at the slow speeds necessary for that size bit. I don’t own the Bosch Colt so maybe it can reach the lower speeds, I know the Dewalt 611 lowest speed is about 16,000 rpm

I would stick with 1/4 and smaller (unless you are surfacing the wasteboard)

I was kind of surfacing. I needed 1/2" 5x9 oak and I don’t have a planer. I then cut the piece out to my need size. I have only construction tools, nothing to cut straight:-(

Don’t feel bad. I have Dewalt planer, never using anymore. When you use to surface with X-Carve, you always do the same as we do. For surfacing you may want to buy 1/2" or 3/4" flat bit. It does very good job. All my products are OAK, mostly hard to find 1/2" wide enough. I buy 3/4" and bring it down to thickness I need.

I feel your pain. I do not have a planer either. I have been seriously considering buying a band saw so I can split the 4/4 lumber the lumber supply has.

me too! I have the exact same problem with my local supplier. Anything under an inch is not very flat.
The bit looks good, btw. Just had some charred wood on it.
Thanks for your help. I never understood the relationship between speed and diameter until I used your spread sheet. I had downloaded while I was waiting for my x-carve, but never had a reason to use it.
Sometimes having good luck is good, but you rarely learn anything.
Thanks again.

1 Like

Just for fun I ran the numbers through Gwizard.
Material= hardwood
tool =carbide straight flute
2 flute .5" dai 1.5" stick out
DOC= .150
WOC= .5
RPM= 11185 still to slow for a colt
feedrate IPM= 110
Plunge IPM=110
surface speed SFM= 1464
mfg suggested SFM 1500
Chipload= 0.0145"
deflection= .0001"

If you push the RPM to 16,000 You SFM goes to 2094 so you run the risk of burning your bit.

I looked at the spread sheet that was linked to and I am surprised at the low numbers listed.


i have been using G-Wizard for the past few days and all i have to say is WHERE HAVE YOU BEEN ALL MY LIFE!

its about 80$ a year but worth every penny. i’m going to be buying ti after my trial runs out.

my feeds/speeds have been amazing since i stopped guessing and started using GWiz

I have never tried and feedrates over 140 ipm

Hey Dave,
What’s surface speed SFM?

No offense, I work on that GWizard numbers, setting machine parameters, Only I can get close to X-Carve capabilities with Dewalt, which is no slow speed possibility what so ever is Rough Cut. Fine and Aggressive cuts totally out of heck.
Some others might like it, I didn’t. I’m the old shit always goes with instincts and live experiences. I have no extra money to break a bit or Belts. Maybe perfect calculations for other brand CNC equipment especially running on Aluminum. X-Carve starts shaking when I give those numbers. Poor guy.

SFM = Surface Feet per Minute and is related to tool circumference and RPM. Do a search on surface feet per minute and you should find lots of info on the subject.


These are the numbers that Gwizard gave me. I’m not saying that they would work well for a X-Carve. A 1/2" router bit is very big for a stock machine and Iffy in a highly modified machine.


I just put commends to AndrewBishop’s post. He was very happy with it, I’m not. Didn’t work at all. Failed all counts.

No problem. 1 thing I have discovered about this forum SW is if I hit the reply button of the post I’m referencing that my reply has the name of the person who’s post I am replying to in the upper right hand corner of my post.

I have been using Gwizard for several years now CNC machining metal both ferrous and non ferrous, also plywood and styrene sheet material. I have never broken a end mill using the feeds and speed that Gwizard has recommended. Now I have broken tools because of my screw up by running into clamps or getting my tool offset wrong.

Gwizard is not for every one that is for sure. I do think that it can help people that are just starting out in CNC and have not got the experience you have.