[TTalma]

I am trying to find a decent feed and speed calculator for different types of wood.

I have been using a 2 flute downcut spiral bit on MDF and have had good results on the material with settings: 3/8" deep, 21000rpm and 200ipm.

Last night I cut a pocket 1/4" square with those settings and the bit was real hot, and discolored at the end. I had the stepover set at .24". The finish was good but the bit is basically ruined.

Does anyone have any good calculators, charts, etc. for routing in wood?

[wizard]

No calculator per say but a couple of things to consider.

1. a dull router bit will get hot. As will a bit with any resin build up on it.

2. I'm having trouble following this: "Last night I cut a pocket 1/4" square with those settings and the bit was real hot, and discolored at the end. I had the stepover set at .24". The finish was good but the bit is basically ruined." To cut a 1/4" square pocket you would need a real small router bit that can't do a 0.24" step over. Are you cutting a much larger pocket with a 1/4" cutter?

3. While an ideal number will vary with the wood in question, make sure you know what your feed per tooth is for the material you are running. Looks like you are running 0.0048 per tooth, calculator here: Milling Formula Calculator. If this is MDF I might try doubling that feed rate and use a step over that is no more than half the cutters diameter.

4. As for the cutter is it high speed steel or carbide? Generally both can be resharpened. In any event don't throw out old worn or broken, carbide or HSS! Even if they are beyond sharpening for their intended use they have many applications in a machine shop.

5. Finally this pocket, how tight was it. Down cut bits can have issues in pockets in that swarf can become packed in the pocket and cutter. This leads to heating. Actually you can break a bit this way. Depending upon what you are doing with these pockets you might want to try an up cut bit.

[TTalma]

Sorry the pocket size was: 2 3/4" wide x 1 1/4" long X 1/4" deep.

The bit was pretty new. I had cut out a few parts (longer run time than it took to make the pocket). After Cutting out the parts I could switch cutters, and it was only a little warm. I usually onion skin when I cut out a part, so my thinking is this is pretty similar to making a pocket.

[ger21]

Yes, what size bit, and what size is the pocket?
Different diameter bits require different rpm.

Feeds and Speeds in wood can be tricky. Do you want maximum tool life, or best finish? Depending on the specific material, they may be very different.

Also keep in mind that machine rigidity and power can play a huge role.
Most major router bit manufacturers list recommended feeds and speed. Onsrud has some very comprehensive charts.
But these charts are generally geared towards maximum tool life. Most hobby machines can not achieve anywhere close to these speeds.

If you are using a 1/4" bit, 21,000rpm is much higher than you should ever be running.
At 200ipm with a 1/4" bit, try 15,000 rpm.

Depending on the pocket size, you can also find that the machine never gets up to full speed, and is actually cutting much slower than the commanded feedrate.

[Gary-Wiant]

I dont have an answer but I do have a question. When calculating feed & speed how can you tell if & when the router will reach full speed? How can a new user calculate the proper feed & speed to be able to get good bit life and good finish, I assume there is a middle ground between the two.

Thank you
Gary

[skrubol]

Most decent manufacturers of CNC mills/bits will give speed/feed recommendations on their website.
If you're using hand router bits, no idea, I doubt you'll get the best results no matter what as they're light duty compared to CNC cutters.

[wizard]

I dont have an answer but I do have a question. When calculating feed & speed how can you tell if & when the router will reach full speed?

A CAM program may be able to give you an estimate if the cam program knows the operating condition of the machine.

Barring that you can do a bit of math to figure out how many inches of travel are needed to reach full speed. Then it is a simple matter to consider how much of the cutting can be achieved at full speed.

In the end how much time is spent at full feedrate is application dependent. Some users may not even see 1%.

How can a new user calculate the proper feed & speed to be able to get good bit life and good finish, I assume there is a middle ground between the two.

Thank you
Gary

When speaking about wood, it is best to experiment. Some woods behave badly when cut even different boards from two different trees can be very different.

[ger21]

When calculating feed & speed how can you tell if & when the router will reach full speed?

I would not even think about this. With any decent machine, it should be negligible.

The only exception might be 3D carving, where the machine may never be ableto get to the commanded feedrate.

[TTalma]

I do almost all of my cutting with 1/4" bits as in this case. My spindle is a Perske 2.2kw spindle. My VFD has a "spindle at speed" output which I use. I can only assume it's pretty close as I don't have feedback on the spindle. The machine is pretty rigid, Pushing sideways on the x axis will yield around .004" before the machine moves across the floor (It weights around 600lbs).

My goal in most cases is for a decent finish. Most of the time I'm not in a hurry so production speed is not an issue. Although I don't want to burn up a bit in a single use either.

I try to use bits made for CNC, but for some operations I can't find a CNC bit or it is cost prohibitive for a small amount of cutting.

Also Solid wood is hard to calculate density. I work with a lot of hand tools and do a lot of hand planing. The density of a board can vary quite a bit depending on growth rings, distance to a branch, etc.

[ger21]

When I cut hardwoods, I make roughing passes about .015-.02 oversize, making 1/4" deep passes at ±300-350ipm and 18,000 rpm.
Then a full depth finish pass at 150-175ipm.

[TTalma]

Ger, What manufacture do you use. Do you stick with one brand or do you buy whatever?

Also whiteside sent me an excel sheet for calculating feeds an speeds. I can share it, but I'm not sure how to post it to make it public.

[rallyx99]

Yes, what size bit, and what size is the pocket?
Different diameter bits require different rpm.

Feeds and Speeds in wood can be tricky. Do you want maximum tool life, or best finish? Depending on the specific material, they may be very different.

Also keep in mind that machine rigidity and power can play a huge role.
Most major router bit manufacturers list recommended feeds and speed. Onsrud has some very comprehensive charts.
But these charts are generally geared towards maximum tool life. Most hobby machines can not achieve anywhere close to these speeds.

If you are using a 1/4" bit, 21,000rpm is much higher than you should ever be running.
At 200ipm with a 1/4" bit, try 15,000 rpm.

Depending on the pocket size, you can also find that the machine never gets up to full speed, and is actually cutting much slower than the commanded feedrate.

Exactly what ger21 said! I suspect that you were rubbing more than you thought because of the factors stated above. You've got to think about how fast the machine is ACTUALLY moving through material and not what the feed rate is set to.

[ger21]

I usually use Vortex or Onsrud for my 1/4" spirals.

Amana Spektra are pretty good as well.
https://www.amanatool.com/46348-k-so...-down-cut.html