PDA

View Full Version : Lathe turning speed various material



kram350
04-10-2018, 10:34 PM
Big time novice here: I know there are specific speeds to turn or mill various materials. I usually turn and mill aluminum and steel. I have no speed read out so I guess based on finish and chip condition. I was thinking about getting a hand held tach to read RPM, but not sure how to convert to FPM which seems to be the standard for feed rates? Any advice on this? Thanks in advance

Fasttrack
04-10-2018, 10:55 PM
One could write a book on the subject... And in fact, people have! This is one of those broad questions that is almost too broad to cover in a forum. I'll start by suggesting that you find a copy of "Machinery's Handbook". This will be an invaluable resource, especially if you don't have internet in your shop. It has speed and feed tables for many different materials (my 1945 copy includes speed/feed tables for granite and frozen rubber, among more common stuff). It also has information on many other fields like fasteners, lubrication, bearings, strength of materials, how to calculate various things like FPM from RPM, etc.

As for that last bit, it's not too hard. Let's take a piece of steel rod in a lathe as an example. You know the RPM of the lathe. Now imagine a string wrapped around the circumference of the circle. If it doesn't overlap at all, how long would that string be if I laid it out flat? It would be the diameter of the rod times pi. During one revolution, that piece of string has come completely off the rod. So now you know that for every 1 revolution, the surface travels a distance of the diameter times pi. To get FPM, then, you just multiply RPM times the circumference:

FPM = RPM * Diameter x 3.1415926535

(Assuming, of course, that the length units are the same... i.e. to get feet per minute, you need the diameter measured in feet)

Brian H.
04-10-2018, 10:56 PM
The formula you need to know is this:

RPM = (4 x CS) / D

Where CS is the Cutting Speed, in Surface Feet per Minute, and D is the Diameter of your workpiece at the cutting tip (if doing lathe work), or the diameter of a milling cutter.

For example, if I were taking a modest roughing cut in mild steel (1018 or equivalent) where my lathe tool was positioned to cut a diameter of 1.25", I would pick a surface speed of maybe 150 SFM if using a high speed steel tool. Plug those numbers into the formula, and we get RPM = (4 x 150) / 1.25 = 480 RPM. Note that the SFM values given in reference books, like Machinery's Handbook, or in tooling manufacturers' catalogs are general suggestions and will vary depending on the material, the rigidity and power of your machine or setup, and the tool geometry.

To go the other way, from RPM to SFM, the formula becomes (RPM x D) / 4. Working from the previous example, we have a cut diameter of 1.25 and RPM of 480. (480 x 1.25) / 4 = 150 SFM.

Hope this helps!

rohart
04-10-2018, 11:02 PM
Assuming you're using HSS - high speed steel, the kind you sharpen up yourself:

Ally - faster than you'd think; steel - slower than you'd think;

Small diameter - faster; large - slower;

Steel - coloured chips mean you're a bit fast.

With a carbide tool - three times as fast as with HSS and coloured chips are OK.

Fasttrack
04-10-2018, 11:02 PM
The formula you need to know is this:

RPM = (4 x CS) / D

Where CS is the Cutting Speed, in Surface Feet per Minute, and D is the Diameter of your workpiece at the cutting tip (if doing lathe work), or the diameter of a milling cutter.


This is an approximation that assumes the diameter is in inches, the "CS" is feet-per-minute and approximates pi as 3. In that case, my formula can be reduced:

FPM = RPM * (Diameter inches) * (1 foot / 12 inches) * pi

Let pi = 3 then

FPM = RPM * (Diameter inches) * (3 foot / 12 inches) = RPM * (Diameter inches) * (1 foot / 4 inches) and if we get rid of units, replacing them with the symbols Brian H. used, this becomes:

FPM = RPM * D / 4

tom_d
04-10-2018, 11:14 PM
The formula above, RPM=(4xCS)/Dia. is the way to go. The number 4 in the formula comes from rounding off 12"/pi when we convert diameter measurement in inches to speed measured in feet per minute. As for the Cutting Speeds, a general rule of thumb is; 50fpm for the tough to cut things like hard tool steels, 75fpm for high alloy steels, 100fpm for mild steel, 150fpm for brass/bronze, and 200fpm for aluminum. This is for turning and milling operations. Cut the calculated rpm in half for drilling and one quarter for reaming. Note that these numbers are for using a HSS tool, and an approximate starting point only. You will need to adjust depending on machine and part rigidity, type of cutting fluid used, etc........ If you are using carbide then take the calculated feet per minute number and multiply by three.

It's not unusual for older machines to be lacking in spindle speed displays so if you can get an estimate with some sort of tach that's great. If the machine has step pulley speed adjustments then measure the diameters and chart out the speeds available. No matter what you do the machine will never have the exact speed required. That, and factoring in all the other variables is why these cutting speeds are approximates to be used as a starting point. Start with the calculated number, then find something close on the machine.

danlb
04-10-2018, 11:24 PM
There are lots of charts online that will tell you what the SFM should be for specific metals. The SFM ranges are quite broad. That's a good starting point. Printed out one of the charts and stuck it to the backsplash of the lathe and another to the column of the mill.

A handheld contact or optical tachometer is a great idea. Once you get the speed for each setting, you write them down and take the batteries out of the tach. You won't need it for a while.

Dan

J Tiers
04-10-2018, 11:42 PM
Big time novice here: I know there are specific speeds to turn or mill various materials. I usually turn and mill aluminum and steel. I have no speed read out so I guess based on finish and chip condition. I was thinking about getting a hand held tach to read RPM, but not sure how to convert to FPM which seems to be the standard for feed rates? Any advice on this? Thanks in advance

No need for a tach if you have speed via belt position on pulleys.

All you need is to know the motor speed, typically 1725 rpm or 3450 rpm in the US. Now for each belt setting, turn the motor (or the spindle, which ever is easier), and count the number of motor turns per spindle turn. Then divide the motor rpm by the motor turns you found, and you have rpm, as close as you need to know it.

If, for instance, the motor is 1725 rpm, and the number of turns was 4 1/2, the spindle speed is 1725/4.5 = 383 rpm. Call it 380, or even just 400, and you will be fine. Put those results for each setting on a chart kept by the machine, and you can choose a setting easily once you know the speed you need.

BTW, you can use any slower speed with most cutters. The slower the surface speed, the sharper the cutter wants to be, so the finish will often not be as good with carbide cutters at slow speeds, because carbide is often not very sharp.

If you have speed set via a knob and dial, as with many small import machines, a tach could be more useful. I think some of them go from slowest to fastest in one turn of the knob, so even labeling marks on the dial might be fairly inaccurate.

Richard P Wilson
04-11-2018, 01:17 AM
Don't forget the published figures are for industrial machines and tooling. Depending what machine you have, the smaller, lighter home shop machines might not cope and need slowing down. I haven't bothered with published figures for many years, its what sounds right, looks right and feels right. What Rohart says in post 4 makes a lot of sense

CCWKen
04-11-2018, 08:47 AM
And all those formulae fly out the window if you don't consider chip load and/or feed rate. Even more reason to use the "post 4" formula. :D

enginuity
04-11-2018, 09:15 AM
Don't forget the published figures are for industrial machines and tooling. Depending what machine you have, the smaller, lighter home shop machines might not cope and need slowing down. I haven't bothered with published figures for many years, its what sounds right, looks right and feels right. What Rohart says in post 4 makes a lot of sense

This is exceptionally wise advice. It really depends on the equipment. Monarch 10EE? I'd start with the posted industrial figures. Chinese or Southbend bench lathe? Much much slower.

I work on both ends of the spectrum - program and setup highly rigid CNC turning centres and also run small bench lathes.

If you have small hobby type equipment you should find yourself running on the slower end of your lathe for most things. If you have a backgear you'll be surprised by how often you will use it.

The good news is most cutting tools, including most of the fine grain carbide (which is pretty much all carbide these days) doesn't mind running slow, provided you have adequate feed (chip load). In manual machining feed is where the art and experience comes into the equation - you need to look at the chips and feel the forces in the machine to determine how things are progressing.

J Tiers
04-11-2018, 09:47 AM
This is exceptionally wise advice. It really depends on the equipment. Monarch 10EE? I'd start with the posted industrial figures. Chinese or Southbend bench lathe? Much much slower.

I work on both ends of the spectrum - program and setup highly rigid CNC turning centres and also run small bench lathes.

If you have small hobby type equipment you should find yourself running on the slower end of your lathe for most things.

Sort-of.

You can run as fast as the machine will allow. No reason to slow down just on the basis of the machine name, or place of origin.

Slow down because you get chatter, or the power of the motor will not allow a decent cut, etc etc. I run slower because the belt on the Logan slips if I run fast and take a big cut.

But I run as fast as the machine allows mechanically, in cases where that is called for by the material of the work and cutter.

enginuity
04-11-2018, 10:01 AM
Sort-of.

You can run as fast as the machine will allow. No reason to slow down just on the basis of the machine name, or place of origin.

Slow down because you get chatter, or the power of the motor will not allow a decent cut, etc etc. I run slower because the belt on the Logan slips if I run fast and take a big cut.

But I run as fast as the machine allows mechanically, in cases where that is called for by the material of the work and cutter.


You are right - you need the right speed and feed for your machine. It may not be the slowest setting.

But I've found with most people starting out on their bench lathe they run way too fast. Maybe it is because they are thinking about working with wood. Or maybe there is another reason.

The industrial suggested speeds will generally be way to fast for bench equipment (except for perhaps very small work), not because the machine is not capable of the speed, but as you say due to chatter.

I tell people start off slow and work your way up. Generally there is less chance of ruining your tool, and is also a safe practice from a work holding standpoint. When in doubt, reduce the speed.

RB211
04-11-2018, 10:09 AM
For HSS, you want shiny chips. For carbide you want colored chips. No math required. If your doing Cast Iron with HSS, and the tip instantly wears away, going too fast.

MrWhoopee
04-11-2018, 10:49 AM
You are right - you need the right speed and feed for your machine. It may not be the slowest setting.

But I've found with most people starting out on their bench lathe they run way too fast. Maybe it is because they are thinking about working with wood. Or maybe there is another reason.


I believe they are suckered in by the term "high speed steel". I had to convince a newbie that 400 rpm was too fast for a HSS tool in a 3 in. diameter fly cutter in steel. Once he slowed down to about 100, the whole thing worked much better. CSx4/dia. is a very easy formula to remember and will get you close enough to start making chips (instead of resharpening your tool).

J Tiers
04-11-2018, 11:09 AM
The formula is too much like work.....

with a 4" diameter part the RPM equals the SFM, so if you need 100 SFM, use 100RPM.

For 2" diameter, use twice the speed. 1" use 4x. 1/2" use 8x speed. f you have an 8" diameter part, use half the speed, so 50 RPM to get 100SFM.

DONE.

It's the same information, but done by simple proportions.

BCRider
04-11-2018, 11:28 AM
Everyone here has been really helpful with formulae to calculate things. But if you look around on the web, or in the Machinery Handbook, you'll find charts with diameter vs RPM that provide you with the SFPM. HERE IS ONE (http://www.tapdie.com/html/sfm_to_rpm-_surface_feet_per_minute_to_revolutions_per_minute .html).

Similarly there's lots of different versions that give you SFPM for different materials from doing a web search for "cutting speeds for different metals".

Now one thing that the speeds for metals never says is that these are the MAXIMUM suggested speeds. Consider that these charts are intended for use in industry where time is money and they want the most material removed in the least time. And they might well be using some great honking heavy machine. So don't be shocked if you find your home machine can and should be used at some lower SFPM cutting rate.

Similarly each material has it's own traits which you'll learn quickly. I've got some steel here from the scrap yard that I'm pretty sure is 4130 or StressProof or some other really tough alloy. I know that if I try to turn it too fast with my HSS cutters that it heats up and work hardens and then strips the end off my cutting tool. But if I slow it way down and keep the edge engaged so it doesn't rub then it cuts fine with the HSS. And by slow down I mean REALLY slow down to a fair bit less than the "hard steel" SFPM chart entry suggests.

Your selection of cutting speed will also matter to the tool life. Ever watch Keith Fenner on You Tube? I'm always a bit surprised that he does a lot of his machining operations at relatively low RPMs for drilling and milling even in relation to the tools he's using. But then I bet he doesn't need to sharpen then all that often. Since I've come to somewhat mimic that I've noticed that I'm not dulling my drills anywhere near as soon as in the past.

So do the math with the formulae above or find and print out the charts that make the most sense to you and have the materials you mostly use and stick them on the wall. And from there go with what works for you within the limits of those charts.

Stainless can also be another material that defies the suggestions. Or it may be that the chart suggestions can only be met with flood cooling. Some stainless I've turned needed to be run at WAY lower a SFPM than the charts indicated and on top of that I had to ensure that the tool didn't rub at all. It needed to dig in and stay engaged or it would work harden the stainless and then it was like grinding the edge off the HSS. So you'd think switching to carbide would be the way to go, right? Wrong..... I ruined two or three of the carbide tips for the clearly wrong sort of insert and brazed carbide tools I had at the time. The solution in the end was to run the darn stuff at about 1/4 the SFPM listed in the charts for stainless and STILL keep it well lubricated. But that's what happens when we pick out "Mystery Metals" from the scrap dealer.

If I had to guess at it I'd say that I mostly work to around 50 to 70% of the SFPM of the charts. And I think my tooling stays sharp for longer for that reason.

754
04-11-2018, 12:06 PM
Bc your problem with stainless and carbide is likely the wrong grade of carbide.

Richard P Wilson
04-11-2018, 04:04 PM
I believe they are suckered in by the term "high speed steel". I had to convince a newbie that 400 rpm was too fast for a HSS tool in a 3 in. diameter fly cutter in steel. Once he slowed down to about 100, the whole thing worked much better. CSx4/dia. is a very easy formula to remember and will get you close enough to start making chips (instead of resharpening your tool).

High Speed Steel got its name in the 1930s when, relative to carbon steel tools, it did allow much higher speeds to be used. I agree its a misleading name in the present day and age, but I still like it, and use HSS tooling a lot. It probably helps that I built up a good stock of 'Eclipse' brand HSS tool stock (A good UK brand from back in the day) so don't use any of the modern Chinese HSS which can be a bit variable.

Illinoyance
04-11-2018, 05:35 PM
https://littlemachineshop.com/mobile/speeds_feeds.php

alanganes
04-11-2018, 05:50 PM
Way back when I started getting interested in this stuff and there was very little of what we now call the Web, I stumbled on a short article in an old Popular Science magazine that I had that addressed just this discussion. It ended up at the same formula that had been brought up here already. While it leaves out lots and lots of the nuances involved, it so simplified things that even a machinist know-nothing like me could use it to good effect. I still have a copy pinned to the wall in my shop, it's been there since I had a shop. I suspect that I have posted this at some point in the past.

Now that we have the WWW, you can find it here, starting on page 106, it's called:

"How you can cut metal like a pro" (https://books.google.com/books?id=psqW_3WpLaMC&pg=PP1&lpg=PP1&dq=popular+science+magazine+%22cut+metal+like+a+pr o%22&source=bl&ots=h6vngEI199&sig=49zBxGeETDuMhNXSpJjux6jpFAw&hl=en&sa=X&ved=2ahUKEwiotcetk7LaAhXI5J8KHXn1AEwQ6AEwAHoECAAQK g#v=onepage&q=popular%20science%20magazine%20%22cut%20metal%20 like%20a%20pro%22&f=false)


Easily digested and works ok for the vast majority of stuff to get you in the ballpark if you otherwise have no idea where to start.

jdedmon91
04-13-2018, 10:14 AM
This is exceptionally wise advice. It really depends on the equipment. Monarch 10EE? I'd start with the posted industrial figures. Chinese or Southbend bench lathe? Much much slower.

I work on both ends of the spectrum - program and setup highly rigid CNC turning centres and also run small bench lathes.

If you have small hobby type equipment you should find yourself running on the slower end of your lathe for most things. If you have a backgear you'll be surprised by how often you will use it.

The good news is most cutting tools, including most of the fine grain carbide (which is pretty much all carbide these days) doesn't mind running slow, provided you have adequate feed (chip load). In manual machining feed is where the art and experience comes into the equation - you need to look at the chips and feel the forces in the machine to determine how things are progressing.

I agree most of the time I run 600 to 800 rpm and .008 per rev on my Grizzly. .060 depth of cut. I use modified tool holders because I have a lot of surplus inserts that I have collected over the years.

Most home jobs are not needing to be at max metal removal. It isnít like Iím turning a profit off my work


Sent from my iPhone using Tapatalk

BCRider
04-13-2018, 11:23 AM
Stainless ..... I ruined two or three of the carbide tips for the clearly wrong sort of insert and brazed carbide tools I had at the time.


Bc your problem with stainless and carbide is likely the wrong grade of carbide.

Oh, it most certainly was. Still is for that matter. I've yet to really effectively wrap my head around the whole carbide tooling thing. I won't get into it in this thread as I've posted about my trials and tribulations in other threads.

MattiJ
04-13-2018, 12:41 PM
(Metric) Cutting speed table I made and printed to A4 size to mount to shop wall:
https://www.dropbox.com/s/6ujdafhnn3fpe1l/cutting%20speed%20table.xlsx?dl=0

Everyone feel free to re-use and adapt to your own use.