View Full Version : Travel speed question?

04-21-2006, 08:36 AM
I was just reading another thread that had a question about feeds and speeds.
Reminded me of this one I've been meaning to ask...just in case I ever get to use my mill again :D
How do you guys figure the feed rate with power feeds?
Do you time it with a watch and mark it on the dial of the power feed?
If so...wouldn't this all change for each size of cutter...ie...a three inch end mill would cut slower than a 3/8" so wouldn't this throw your calculations all out of whack?
Do you make a whole pile of feed/speed marks on the power feed dials for each tool or what?
Or do you have many sheets of info printed out with your findings?

04-21-2006, 10:01 AM
Torker thanks for asking. Maybe we can get one of the experts to come over here and answer the question. I also would like to know what they do.


04-21-2006, 10:44 AM
In my case I used enough older mills with mechanical feed systems that you get to be able to tell roughly by eye when you go to a mill with electric variable feed. With larger cutters you can also use a vernier and measure the thickness of the chips, this should measure the same as your chip per tooth if the feed is set right. (Works well with carbide face mills and the like that throw larger chips.)


04-21-2006, 11:39 AM
I for one need a cutting speed 101 course.

I am not able to understand the speed charts that I look at. Some of the formulas want the end mill in the small sizes to run at thousands of rpms. This kills any cutting tool that I have seen.

I run my lathe from 200 to about 800 rpms and this works fine for me. Slower for threading. I have a Millrite mill and run this on the middle groove on the stepped pulley. Motor turns approximately 1200 rpms. Don't know the real speed of the spindle.

Anyway don't understand the charts. Surface feet per minute or cutting speeds.

I love my tools. :)

04-21-2006, 02:23 PM
Ha, I'm glad I'm not the only one!
I read posts from guys all the time who rattle off cutting travel speeds and I've always wondered just how we do this. Especially if you have no power feed. Why am I thinking that most do it by the "seat of their pants" and don't have a real answer to my question?
Or is it just as good to guage travel speed by the way the chips look? Or by how red the endmill gets (kidding)?

J Tiers
04-21-2006, 04:53 PM
Actually, I don't think the travel speed" really matters.....

The chipload per tooth does. The RPM does.

There might be all sorts of chiploads for same table speed. Depends on the RPM.

Assume 4 flutes, 250 rpm, then there are 1000 flutes (teeth) per minute. If you advance the table at 2" per minute, than you get about 2 thou per tooth chipload.

So, I would choose a cutter RPM based on the material and cutter diameter. Then I would choose a table speed to keep the chipload "reasonable".....

In actual practise, the mill has no power feed (yet) so I just go by the cutting sound and "feel of the crank".

That works for anything except a roughing endmill. For that, I just crank as fast as possible..... it's never fast enough...... :D

04-21-2006, 06:49 PM
I'm no expert, but I'll throw in my $.02. First go back and read the post by J Tiers if you missed it. That's how I do it. Here's my guesstimates on speed for different sized cutters:

For cutting mild steel with an HSS end mill, 280/cutter diameter - or as close as I can come with exceding that number on my step pulley mill :) Same for lathe work with mild steel and HSS cutters, but use 280/work diameter. I double or tripple the RPM and decrease the feed per tooth by the same factor (in other words table speed stays the same) and take a very light cut for finishing.

Everybody was taught a different number, so don't get too worked up about 250 vs 280 vs 300. The 'tan chip' rule is also a really good guide for mild steel. Tool life is also a good guide.

I go three to 4 times as fast for HSS and aluminum. I go 2 to 4 times as fast for carbide and mild steel. I slow it down to about 2/3 speed for stuff like annealed 4140 and then watch the color of the chips. If I am cutting 4140 with HSS and the chips come off tan and then turn blue a second later, I'm happy.

That's just my off-the-cuff speeds that I start with instead of digging out Machinerys handbook and the calculator every time I set something up.

All that stuff is what I do. Everybody does something different. None are wrong unless they are wearing out their cutting tools prematurley or loafing so slow that they never get anything accomplished.

For table speeds it goes like this
desired chip load = (number of flutes X rpm)/table speed
Jteirs did the math. I won't do it again...

Calibrating the table speed is another question altogether. I have an old Gorton Mastermil 1-22 and the tube type Dynadrive for the long feed on the table has survived and still functions. As you may guess, it isn't exactly stable with tubes in the servo circuit - even with NOS tubes. I use a stop watch and two marks on the table (or my DRO since I finally got it working) to find out how fast it is moving. Then I go into the circuit enclosure and tweak a pot inside the Dynadrive until the actual speed somewhat matches the indicated speed on the dial. You may want to put a piece of tape on your power feed and mark apropriatley if you don't know where to tweak.

Disclaimer - I'm not a professional. Macherys handbook take precedence over anything I just wrote.

04-22-2006, 12:40 AM
The formula I was taught for RPM is:

RPM = (4x cutting speed)/diameter

Diameter is the 'rotating part' so the diameter of the workpiece when on a lathe, the drill or cutter on a mill or drill press.

Cutting speed for Mild Steel I was always told was 100, this is a 'base value' to work from. From there, aluminum or brass would be 2-300, cast iron maybe 60-70, tool steel or SS would be maybe as low as 30-50. These values are for HSS tooling.

So, as an example, drilling 1" holes in mild steel RPM = (4*100)/1, which works out to 400 RPM. (Sounds fast, right?)

Then I was taught that using old, or tired equipment, to cut that to around half. Without coolant, maybe another 25-50%, putting you down somewhere in the 1-200 RPM range, which I find works fairly well depending on the machine and the setup.

If you're using carbide tooling, then you can maybe as much as double the figures again.....

Is there a hard and fast rule? Nope....main thing is to keep the tool cutting edge cool so that it doens't 'burn out, or anneal from the heat. With carbide (particularly insert cutters on milling machines) I find that people go faster, often the correct RPM, but feed WAY too slow (and often too light of cuts), resulting in wearing the inserts out from overheating, rather than actual cutting wear. One thing that I've found is that the workpiece should never feel warm, let alone hot, to the touch. If it is, there's too much heat being generated in the workpiece and tool, almost all the heat will transfer to the chips if things are set up right. I can make blue chips on a mill with tool steel, taking 1/4" deep cuts, and still put my hand on the workpiece. If you can't, something's up.

Remember, when you have 6 or 8 inserts that you still need to get that feed per tooth right, if it's spinning at 1000 RPM and you're taking forever to go across a small piece, how is each insert getting a .002-.004" chip per tooth?


04-22-2006, 01:41 AM
Some very good info here! Thanks for taking the time guys!
I see a few things I've missed but I guess I've been doing it "mostly" right.
JT...lol! You gotta love roughers huh! I buy mostly Niagra roughers and they are hotrods :D
And thanks for the simple math lesson!
So it seems there is more to the "seat of the pants" travel speed than I'd thought. I just thought it was absolutely critical that I knew the correct travel speed. It does all connect though. To get the proper chip load...you can have the proper rpm and doc but if the travel speed is whacked then you can't attain proper chip load...no?
I really have to remember to measure the chips next time. Seems like a good idea to me.
Another thing...sounds like I'm one of the guilty ones with carbide. I use a 2" insert endmill a lot and I may be going through inserts too quickly because I don't feed it heavy enough. It uses positive rake inserts and even the good ones don't seem to last. Probably the best for my small mill though.
Oh the things that experience will cure! :D

04-26-2006, 03:00 AM
Still using the Harig slide calculator I bought in '80 for a class at community college. :D

All such charts & formula give a good staring point. Usually designed to maximise production in industrial setting, so you can back off some. Tubal Cain says max tool life is at about 3/4 recomended speeds.

04-26-2006, 10:31 AM
I use 3.82 times the surface speed divided by the cutter dia. to get RPM and then chip load times number of flutes times rpm to get feed rate.
The REAL issue here is to get guys to stop thinking in terms of RPM and start thinking in terms of surface feet....
As we all know ...a 1/16th cutter spinning at 12000rpm is doing the same sfm as a 1" cutter spinning at 3466 rpm
It's all about sfm...not RPM
I routinely cut 304 at 500sfm
I face most alum at 2200sfm with a 3" 6 flute face mill at 120 ipm. That's a .0033 chip load. at .1 depth of cut the load meter is running about 60%
I use carbide 6 flute half inch cutters on steel at 500 sfm. that's be 3820 rpm. 3/8 inch deep and 57 ipm about 80% load. nice and quiet. just throwing chips.
I realize this is CNC instead of manual but the concepts are the same. The table feed in ipm are the same co there is no need to have one scale for this cutter and another tor that cutter. Table feed is table feed.
Just think in terms of sfm instead of rpm

John Garner
04-26-2006, 01:42 PM
Russ --

Table Feed rate for a mill is stated in either Inches Per Minute (IPM) or Millimeters Per Minute (mm/m), and is easily calculated as [Feed Per Tooth x Number of Teeth on Cutter x Spindle Speed in Revolutions Per Minute].

The handbooks provide guidelines for Feed Per Tooth, you'll have to count the Number of Teeth on Cutter, and Spindle Speed is "machine actual", which should generally be less than the theoretical spindle speed you calculate from Cutter Diameter, Pi, and a handbook parameter for Cutting Speed (Surface Feet Per Minute or Meters per Minute) for the particular cutter material and workpiece material pair.

The best essay on the subject I've encountered was written by the late Robert Bastow: http://www.metal-club.org/MillingSpeeds.html


04-26-2006, 07:56 PM
Thanks again guys! I've read all your info, and the info from Johns page.
I STILL don't see a concrete answer to my question. Simpler to get a handle on it with a large machine with feed speeds and big horsepower that you can control exactly (like a lathe).
But in the case of a manual feed machine or a cheap powerfeed like mine, you are never going to get it exact. I thought it was a bigger deal than that. I think it all comes down to the last lines in Robert Bastows writeup.

04-26-2006, 08:10 PM
Russ,there isn't anything set in stone for feeds on a mill that uses a DC variable speed feed.You just figure your speed for the cutter your using,drop the feed in and ease into the cut,once the cutter is fully engaged you can ramp up the feed rate to a comfortable speed(no table or spindle vibration or chatter)once it's set for the cut your making it's just a matter of dropping the FWD/REV lever in and out on the feeder.

Older mills horzional or vertical that use mechanical feeds or single speed motor drives on a mechanical feed you then have to count chipload per tooth etc,but there are charts for that if you don't want to do it the hard way.However,as mentioned it's simply feedrate/tooth count.

04-26-2006, 08:34 PM
Thanks D. I'm pretty sure I have it close enough then. I don't burn endmills anymore and quit making dust as well. Just trying to put the whole "in the know" together.