How to calculate the RPMs and Speeds using as slitting saw on a mill?

HMF

HMF

Site Founder
Administrator
Joined
Sep 22, 2010
Messages
7,223
When using a slitting saw with, say, a 4" blade, on a milling machine, how do you figure the rpm's and cutting speeds? Is it the same as an endmill?
What is the formula to use to calculate the speed so that you have the proper torque?

Thanks!

:thumbzup:

Nelson
 
I'm not 100% sure so perhaps the experts will chime in, but I would think this would be sorta like a bandsaw's speed regarding inches per minute. Meaning as you change diameters on a slitting saw the surface speed will either increase or decrease with a constant RPM so I would think if you took the slitting saw's diameter times 3.14156 to obtain the circumference, then multiply or divide that by the RPM to get your surface speed. Match this surface spped to the material you are dealing with and I think it would work out.

But then again, what do I know?
 
I think November has it correct. Here's a good explanation of working the numbers backward to get the desired RPM from Sherline's site:

Using the correct cutting speed is an important part of using slitting saws correctly. You must realize that when you exceed the cutting speed with high speed steels, the dulling process can be instantaneous. It isn't you get shorter tool life, you get "no life"! This can be expensive in time and money because slitting saws usually cost so much you don't have spares.

The diameter of a slitting saw is much larger than that of a mill cutter and it has many teeth. This means the speed of the cutting surface will be fairly high even at low RPM compared to an end mill. For example, the Surface Feet per Minute cutting speed (SFM) for high speed steel is about 67 SFM*. For a 2" diameter slitting saw with 110 teeth cutting 12L14 steel, the calculations would be as follows:

RPM = (SFM x 12) ÷ (Tool Diameter x P)

RPM = (67 x 12) ÷ (2 x 3.14159), or 804 ÷ 6.28318

RPM = 128 RPM
Click to expand...

-Ron
 
You'll get a straighter cut if you climb cut, even if you are going against instinct. Just watch your locks to drag enough to control the feed.
 
RPM=CSx4/dia

which is a shorter way of saying the formula Ron quoted, and gets rid of the 12 inches per foot and the 3.14159 of Pii.

Next is the feed rate which is a certain amount per tooth.

I am looking forward to getting my new calculator, Machinst Calc Pro, which should be here sometime this coming week to see how it handles these calculations.

Walter
 
Jerry, it's when the cutter is rotating in the direction where it has a tendency to "climb" onto the work on it's own. It's a touchy thing, and if there is backlash (and on manual machines there always is), it can let the cutter jump into the work ahead of schedule..... and break. It's also (and properly) called down-milling, where the thickness of the chip actually drops, rather than gains in thickness, as in "conventional", or "up-milling".

CNC machines, and other machines with ball screws generally don't have so much backlash to have a problem with it, and so it is the preferred feed method. Cutting edges generally last longer, and a better finish results. Some more advanced manual mills have a hydraulic cylinder to damp backlash and can be used in that manner with no problems.
 
If you're not doing heavy cuts, you can snug up the locks and get away with it. It actually is a better way to cut, if you can do it.
 
Hi Just to add my $0.02

This website has a great description of backlash and the interaction of climb vs. conventional milling.

http://its.fvtc.edu/MachShop3/basicmill/backlashIS.htm

On RPMs I use the the following feed ranges in calculating for HSS tools the ones for carbide are much higher.

Material Speed FPM
Aluminum 200 to 350
Brass 300 to 700
Cast iron 60 to 80
Copper 400 to 500
Steel 100 to 125
Tool steel 50 to 60
Stainless steel 75 to 130

Like starlight_tools said I use RPM = 4*FPM/Dia to calculate.

Keep in mind the type of machine you are on is a big part of what you actually use for these values. I have access to a HASS mill that uses values much higher and a Bridgeport that uses the upper end of these numbers but my home machine is is on the low end or even a bit under. I think the big thing is can your machine handle a proper chip size at the RPM you are using. If the chips are too small they will not carry away enough heat from the cutting area and that causes all kinds of problems. :( Of course another thing to keep in mind is that some machines only have a set number of ranges. I think mine has like 9 or so. That means you only have so many to pick from so you can often just estimate the value in your head. Example the value for cutting with 4" silting saw in steel would be 100 RPM but on my mill 200 RPMs is my lowest range. So I set it at that lock everything I can down as best I can and put lots of coolant on it. I would make the cut with conventional milling since my mill is no where near rigid enough to do climb milling. However, the people that said climb milling is better are right if your mill can handle it.

Hope this helps,
Jeff
 
Hi Rick
You are spot on about chip and tool condition being the best guide. Its funny things we do without even thinking about it and then forget to tell others.

My $0.025

Jeff
 
Hi Rick, your right about cutting speeds, I have a variable speed column drill, (driven by cones) which is a dream to change speeds as you are cutting. I think its a skill that has to be learnt, watch the drill, the depth of cut, amount of pressure, watching for burning of the drill bit, listening to the machine drilling, even smelling the machine as its cutting, and feeling when the break through is about to happen. differant materials are drilled at differant speeds, A little hand held calculator would come in handy, just put in (material to be drilled) (size of drill) = cutting speed #@clap2@& come on ! you could knock one up
 
You must log in or register to reply here.
Back
Top