What's new
What's new

Feed speeds on horizontal mill

applescotty

Cast Iron
Joined
Jan 23, 2004
Location
Wellsville, KS
Guys,
I've been playing with speed and feed numbers for my horizontal mill. The problem I'm running into is my feed rate. My mill is capable of 0.003, 0.005, 0.006, 0.007, 0.010 and 0.014 inches per spindle revolution. This works out pretty well for end mills, but doesn't seem like it will work for larger cutters. Say I've got a 4" cutter, with 18 teeth. If, for example, the feed per tooth (this is the same as chip load, right?) for a particular material is supposed to be 0.004 inches per tooth, then my feed rate would need to be 0.072 inches per revolution. This is five times faster than my top feed rate. At my fastest feed rate, with an 18 tooth cutter, I can do .00078 inches per tooth.

So, my question is, will that work out okay? Am I going to dull my cutters quickly running at the slower feed rate? Or do I have this all wrong?

Scott
 
Scott:

Don't know what mill you are referring to, but the old small B&S discuused here recently in Antique section would make .003" to .150" per rev.

To answer your question, it sounds as if you will indeed tend to wear out an 18 tooth cutter.

John
 
run the cutter w/ every other insert removed, or every second, etc. it'll increase the chip load on those remaining (the kennametal guy told us that when he was trying to sell us new tooling where I used to work as some of our machines were pre-insertable tooling era and under-powered or too slow)
 
John,
My mill is a Fox mill: My Mill

While I have not measured the feed rates, the sales literature I've got for it lists the values I've stated, and I have no reason to not believe it.

So, back when this was new, what was done? Did the cutters have less teeth? Did carbon steel cutters require less feed per tooth?

Scott
 
Oh, man...and I thought my Burke looked ancient...

8*)

Personally, I'd not get too carzy over following the numbers - with my old Burke I basically feed at whatever sounds right.

With this old stuff you are going to drive yourself nuts trying to work the "optimum" tool rates and the like.

Do what makes the machine sound happy - and when it's unhappy trust me it's blindingly obvious...

Alan
 
scott-

your mill and my mill have basically the same table drive arrangments coming off the machine spindle.

yours looks like it has an additional gear set at the back of the table drive. i think it will function more like a hi-lo selector. your feeds step 3-5-7 and 6-10-14.

i started figuring out my geartrain by making chalk marks on the pulleys and turning the spindle by hand to count and see what was going on.

computing the chip load/feed rate is confusing.

i have the brown & sharp treatise on milling. in there, the cutter speeds for carbon steel tools is smaller than for hss, almost half.

the section on feed rates, about a page, says basically commercial finish is obtained with 0.03 to 0.05 per rev, finer finishes are obtained at 0.015 to 0.020/rev.

there is a caution that really small feeds can result in cutting edge not cutting but sliding over the work which will sound like chatter.

more text is given to climb milling vs conventional milling and how inchs/min are more convenient to understand.

inches per minute make more sense to me right now. i think once i get my mind over horizontal, in/rev may make more sense.

i am working on inputting the niagara cuttter manual charts so i can manipulate them.

http://niagaracutter.com/millingcutters/index.html has sfm and feed charts.

i think alan's suggestion of whatever sounds right is propably the best advise. however, i have never heard a horizontal mill cutting so i am a bit hesitant.

i think what is intimidating to me right now is that there are too many variables and i need to eliminate some of them to better understand what is going on.

so i think that if we stick to 3-5 though per rev, which is about 6-10 inches per minute we should be ok.

dennis
 
If it does not do the "rrrrrrr...rrrrrrrr" thing it isn't happy. The "rrrr" is really a combination of a growl and metal cutting noise. and the pulsing is because the cutter isn't *exactly* centered on the arbor.

Slow RPM and boost feed if you don't get there. For some reason, small mills always have cutter-dulling high RPM. Fine unless you get into something that work-hardens.......DAMHIKT

My little 5 x 18 Lewis works MUCH better now that minimum RPM on the spindle is about 30.

Makes those 4" cutters much happier in tool steels.
 
Your mill was designed at a time when high speed steel was king. Carbide was probably unheard of or "unobtanium" at the time. I doubt the designer ever envisioned inserted tooling. Your trying to put a supercharger on a lawnmower. Nothing wrong with your machine it's just that its designed for a different style of tooling. You'll never be able to climb cut (over about .003" depth of cut) so don't try unless you are going to replace the screws. Face it there are limits and only so much you can do. If you do want to increase the feed rate there is an easy fix.

First find a used Ridgid Drive or pipe threader, the hand held type. They are common, powerful, and have forward and reverse.

Next get a speed reducer. NOT one of those router speed controls for $20, it will last about 30 minutes. Bronco makes a good one but you may find used ones.

Make an adaper for the Ridgid drive to the feed table. Use the variable speed for feed. You got everything you need. Simple and if you want to thread pipe your all set. We must have a hundred of them here. We use them to drive bring bars (they will pull an 1/8 inch cut on a 24" daimeter with a 4" bar) We drive taps up to 6"-8 (with a multiplier of course) I have even seen them used to turn fan shafts. For the boys coming here for scraping I will have a few "field" machines setup including the lathe.
 
JTiers-
How did you get your spindle speed down that low?
Electric speed controller? mechinical gear drive?

I am having a tough time getting pulley combinations to get low enough? I am getting 120-250 rpm motor side input to get the spindle to turn at a reasonable 30-150 rpm to use 2-6" diam cutters.

dennis
 
cruzinonline,
I'm definitely not trying to "put a supercharger on a lawnmower". The cutters I have to use are HSS. I really am trying to use it within it's capabilities. It's just that I don't quite understand what it's capabilities are. The slow (and small) range of feeds is what's confusing.

The sales literature for it states that "the machine is an ideal machine for light tool work, as well as for medium class of manufacturing work." So, it wasn't a specialized machine.
So, if it was a general purpose machine, why are the feeds so slow?

Scott
 
Jim,
The feed per revolution is independent of the spindle speed. Even at 30 RPM, I'd still only be able to feed at a maximum of .00078 inches per tooth.
Scott
 
No disrespect, what I meant was todays inserted tooling was not around when this fine piece of iron was designed. If there was carbide, it was mostly brazed stuff. The turbocharger reference was the concerning slab mills that were designed to be used on machines with 30-50 or more horsepower. Yours looks a little under that. We have a fine horizontal mill with a 6" spindle, 24' of horizontal travel, feed rates out the wazoo, but just try and put a 6" slab mill on it and push it the recommended feed and speed. The machine can't handle it. 20th century machine 21st century tooling.

Another way to look at this is volume. I have no clue what the actuals numbers are (someone here does) but there is a finite amount of material that can be removed vs horsepower. For example, your machine is limited to a feed rate of .014 per rev. Now, if you were pushing a 1/4" slitting saw, 1" depth of cut, and you were running at 72 rpm you would travel about 1" per minute and remove .25 cu. inches of material per minute. Ona 1" saw you would be pulling 1 cu. inch per minute, and with a 4" wide saw you would be pulling 4 cu. inches per minute. The point is there is only so much material your machine is capable of over a given amount of time. I believe your feed rates were designed with current tooling, based on machine power, average types of materials for the time and all the other normal parameters and standards for that time period.
 
cruizinonline,
No offense taken. What I meant was that I'm really just trying to figure out what tooling, speeds, etc I need to use for my machine to work properly. Based on the calculations I've done with current speeds, etc, my feed rate is too slow. That means that either:

a) You can run HSS significantly slower than the recommended speeds without greatly accelerating the wear on the cutter;
or
b) the cutting material commonly used on this machine was not HSS, and could handle running at the slower speed;
or
c) The Fox Machine Tool Company didn't know what they were doing.


Anyways, thanks guys for all the input. What I probably just need to do is get an arbor for the machine (which is why I've been playing with the numbers, instead of actually trying to mill something) and see what happens.

Scott
 
Per slowing.....I swapped countershaft pulleys to slow it down. It has a backgear also, so the combination did the job. It ruins backgear unless I have an endmill in teh spindle. With a roughing endmill, it runs me ragged cranking in CRS, I need a drill motor to go that fast.....

The problem with feeds may not be one. Usually the cutter will cut only on half or a bit less of the teeth anyhow, due to eccentricity. Only a few are taking a full cut, the rest a smaller, or none.

I don't have a functioning power feed, so I crank it. Works for me, lots of one-off cuts aside from gears and splines.

Yes the HP is a big factor. And the HP that can go through the flat belt drive, which probably has no back gear.

But, shallow cuts put a premium on sharp cutters. Dull ones rub.

As long as it is not squeaking, and you don't go too FAST on rpm, it should be fine.

per Qs, my opinion:

a) Yes

B) Carbon steel cutters will rub-dull too, but toolsteel workpieces definitely need a slower speed and feed

c) They made design choices, and probably didn't expect to work much aluminum......

You are going to have problems with larger cutters, speed, and the flat belt direct drive, I suspect. To get the HP in, you need belt speed, which means spindle speed, and that can be a problem for larger diameters.

But, to get a speed that won't burn up a cutter in something more resistant to cutting, you have to have a slow belt speed because of the 1:1 linkage to spindle speed.

To solve your problems the easiest way, can you put a handwheel on the table feed? In your shoes I sure would if I could. Then you can feed by feel.
 
on HP vs volume- the only thing i have seen is from the niagara cutter handbook. this was from the gang milling section.

http://www.niagaracutter.com/techinfo/millhandbook/styles_apps/build.html

"As a general rule, one horsepower is required to remove one cubic inch of steel per minute. A simple analysis can be made to determine the cutter diameter, size of cuts, and the speed and feeds permissible - dependent upon available horsepower and equipment. "

this seems reasonable, but i don;t know when this was written or what was assumed.

applescotty's machine and mine are lightweight machines and not too rigid. they being belt driven machines, i would expect that we propably have 50-60% loss on the transmission system.

i think cruizin is right on with his analogy.

as fas as cutter wear goes, the number of cuts a tooth will take is a finite number and the cutter does not care of you are taking 2 thou ot 10 thou, it only had so many cuts in its life before sharpening.

my diamond is dbl belt drive, so i have more potential for putting power into the spindle.

dennis
 








 
Back
Top