[native34]

Does anyone using an RF 40 Round column mill please help me with proper feeds and speeds milling steel to be effective i seem to be breaking and burning up alot of End mills and not getting any progress also what depth of cuts are you taking i seem to be haveing alot of problems with these two areas

[SCzEngrgGroup]

RPM is determined by tool diameter, and material, by calculating SFPM - Surface Feet Per Minute as follows:

SFPM = (PI * ToolDiameter * RPM) / 12 or,

RPM = (SFPM * 12) / (PI * ToolDiameter)

This is usually rounded to:

RPM = SFPM * 4 / ToolDiameter

SFPM is a function of the tool material and the work material. For mild steel being cut with HSS cutters, SFPM should be around 80. For aluminum, 400 SFPM is a good average. If using carbide, double or triple those numbers. So, if you're cutting mild steel with a 1/2" HSS endmill:

RPM = (80 * 4) / 0.5 = 320 / 0.5 = 640 RPM

Feed rate is a function of RPM, the number of flutes on the tool, and the "chip load", which is the nominal thickness of the chip each tooth carves out:

FEED(in IPM) = RPM * #Flutes * ChipLoad

Chipload is a function cutter diameter, and for roughing cuts ranges from perhaps 0.0004" for very small endmills (1/16") to perhaps 0.008" for large ones (1"), and varies linearly for sizes in between. So, for a 1/2" 4-flute endmill, assume a 0.004" chipload, and you get:

FEED = 640 * 4 * 0.004 = 10.2 IPM

Depth of cut should be as much as you can get away with, which will be limited by spindle power, machine rigidity, and coolant used.

Now, you're not likely to reach this numbers on a small mill, due to the limited spindle power, limited rigidity, and inadequate cooling. So, start by setting the calculated RPM, pick what you feel is reasonably modest depth of cut, and start by feeding at perhaps half the calculated rate. Increase feed rate until finish quality starts to degrade. When you reach that point, back off on the feed rate perhaps 10%. Now increase depth of cut until the machine starts shaking, or the spindle motor starts laboring, then back off a bit.

There are no canned numbers, as every job is different, and you have to learn how to "read" the machine. Some rules of thumb:

Keep chip load as high as possible. If you find you have to reduce feed rate well below the calculated value, then reduce the RPM to keep the calculated and actual feed rates reasonably close. Running high RPM with low chip load will cook tools faster than anything.

USE COOLANT!! You will never come anywhere even close to the calculated numbers without coolant. A mist system will work wonders, with very little mess.

Here are some typical numbers I use on my knee mill, running mist coolant:

1/2" 4-flute HSS endmill cutting 1018 steel: 700 RPM, 5 IPM, 1/2" DOC
1/2" 2-flute HSS endmill cutting 6061 aluminum: 3100 RPM, 12 IPM, 1/2" DOC

Regards,
Ray L.

[philbur]

I ran an RF40 clone for more than eight years. What is your maximum spindle speed, what method are you using for feed (manual, power or cnc) and what diameter cutters, number of flutes and cutter material are you using.

Phil

Does anyone using an RF 40 Round column mill please help me with proper feeds and speeds milling steel to be effective i seem to be breaking and burning up alot of End mills and not getting any progress also what depth of cuts are you taking i seem to be haveing alot of problems with these two areas

[Hirudin]

RPM is determined by tool diameter...

Thanks for taking the time to write that up, it'll come in handy!

[native34]

"I ran an RF40 clone for more than eight years. What is your maximum spindle speed, what method are you using for feed (manual, power or cnc) and what diameter cutters, number of flutes and cutter material are you using."

Philbur

My max spindle speed right now is 2500 RPM. I have a VFD and i am getting a 3 Phase motor to allow for about 3000 - 3500 RPM but this won't be until early next year. I am using CNC for power my cutters are mainly 3/8" - 1/2" four flute HSS EM Flat and Ball i also use Some Cobalt 1/2" Roughing bits they look like a corncob. I have also tried carbide but i don't seem to get very good results with them. I mainly cut CRS but i would also like to cut Aluminum.