Surface Speed

Am I the only guy here that has never learned or used surface speeds ???

I've been a machinist since 1982, and never once was taught anything about it. I was always told that the speeds and feeds outlined in the charts were written by people that didn't really actually run machines. Everything I had ever learned about feeds and speeds was by sight, sound and feel of the cut.

I suppose I would need to know much more about it if I ran a CNC, but I've never had a problem judging what speeds and feeds to use on any given part, and I've never been told I'm going too fast or too slow.

I'm as you rockfish

I use all my senses.

machine noise and vibration or surface finish tells you when your not doing something right.

All the best.mark

I do use surface footage as a guidline probably because I was taught that way but I'm still using it today 23 years later. I don't use it all the time but when I'm cutting some strange material I make a note of the best speed so I can use it next time I come across the material. It does come in handy when runing a CNC in a production mode and I always teach my apprentices how to use it and leave it up to them if they want to use it.

I was taught the hows and whys of figuring speeds and feeds; but rarely bother. Experience will tell you what will work best.

I don't run production parts, a lot of the stuff I do is repair or one-offs. It's tough to identify material types when you're doing repair work anyway. Maybe you know what the part SHOULD have been made from; but ....

As far as my home shop work goes, economy takes presidence over speed, and besides, I rescue a lot of material from the scrap box (was that 4140, 1018, etc.) for stuff that isn't fussy. Running a little slower cuts down on my cutting tool expenses.

Kevin

I start with the reccommended numbers and depart from there as conditions indicate.

One thing to remember: the people who publish those tables have to satisfy the very smart and capable people who use them. If their numbers are BS then their products that don't fulfill the numbers are likely to be thought of as BS. You can bet that Kennametal, Union Twist Drill, and other major tool manufacturers refine their performance tables to a high degree. Their bottom line depends on their customer's faith and their product's performance.

I tend to trust published figures and those little carbide slide rules for initial feeds and speeds as modified by my personal experience. I recall working out feeds and speeds and depths of cut for face milling big steel plate fabrications. The calculator gave HP figures as well. I applied the calculated data to the machine. After the cut was established I looked at the motor load meter amps and usualy I was withing 5% of the predicted figure.

I used to machine largish K-monel castings. Nothing Kneeametal, GE, or Iscar could come up with seemed to hold up in this abrasive stuff, fancy coatings or not. The insert would go dull in 10 minutes and thereafter you had about 30 seconds before the end of the tool evolved into a solid friction welded mass of busted carbide and smeared metal, stuck to the tool shank.

It wasn't until the Kyrocera saleman gave me a couple of inserts that my productivity took off. Using that insert to the Kyrocera specs for high nickel alloys I could cut sand cast K-monel at ally steel speeds and feeds. Plus I got good finishes and flat faces.

The lesson here is sometimes your usual suppliers don't have a solution but eventually you find someone that does. All the petty annoyance suffered listening to salesmen paid off on that one transaction. Out of maybe 50 tons of castings yielding maybe 10 tons of chips we destroyed a dozen tools in the first few days until we were led to the Kyrocera insert. For nearly a full years after that the only expense was inserts.

If you can't do stuff by the numbers your process is controlling you.

The MetCut Institute in Cincinnati, Ohio has spent a great deal of time in researching and investigating proper speeds and feeds for optimal metal removal. Their books are an invaluable reference resource that should be on every serious minded machinist's bench. The "gut instinct" approach works but it is definitely not optimal. Most guys that run by the gut instinct method are usually running things far too slow. You put a guy that has learned how to properly calculate cutting speeds and feeds next to the gut instinct guy and the difference in efficiency is night and day. For the home hobby machinist this doesn't matter. But if you are trying to make a living at this it is a real good idea to take the time to learn the proper method for calculating cutting speeds and feeds. The fromula is fairly simple and if anybody replies to this post of mine I will gladly explain it to you.

Joe

It is really not that hard to calculate and it is not even necessary to use a calculator. You can easily calculate RPM from a desired SFPM in your head. All you have to remember is at 4" dia your SFPM = RPM....close enough. You simply double or half from there. Say we know that we need 110 SFPM and we are turning an 8" part, what RPM? It would be 110 RPM @ 4" so slow it down 50%(half again as fast)so start at 55 SFPM. Now according to my Kennametal slip stick calculator it should be 53RPM, we're in the neighborhood. At the same rate, a 6"dia part is a third bigger than 4" so slow the RPM 1/3.....110-36 (a third of 100 is 33, plus a third of 10 is 3, so 36)=74RPM.
Say you want to turn a 1/2" drill at 80SFPM. It would be 80RPM@4", 160RPM@2", 320RPM@1" and 640@1/2"dia. Once again, according to a calculator it should be a lash over 600. Pretty good eh? No calculator needed! All that's needed is to remember at 4", RPM=SFPM.

I have found over the years that the speed/feed tables are a good starting point, the variable is the machine or fixture.

Over the years I have called most of the major tool manufacturers of inserts as well as drills and taps I have found most times they gave very good advice. Again it is only recomended as a starting point.

Jackmo

I'm guilty of the same seat of the pants technology.

In the last few years useing my new cnc's it has become definitely more productive to figure it out.

on the lathe you set the SFPM and the control figures the rest.

On the Hurco VM1 same thing, enter the sfpm the number of flutes and chip load/tooth and run.

The thing you have to do is determine the correct SFPM. FOR THE TOOL AND MATERIAL.

I think finding the starting information takes the most time. Calculation time is small.

Last year for example, I was turning 4140 pre heat treated steel way too slow. The kennametal Rep. stopped in to help, he calculated the correct speed and feed and detph cut. What he came up with was at first frightening and I asked him if he was certain of his numbers. He assured me that this is where the tool was designed to run. So with one hand on the E-Stop button I started it up. With teeth clenched tightly, I watch as the bit entered the cut. The sound coming from my "new" lathe was one of the nicest sound I could have imagined. The finish was like a mirror compared to my previously 220 grit looking thing. The opperation went from over 20 min/pc to about 3.5 min.

It's worth the time, figuring out the right speeds and feeds.

Wiz

The other day one of our machinists (?) spit a part off the table on a horizontal boring mill. I was called over to take a look and see if it could be salvaged, it could. Next I tried to figure out why it moved in the setup. FIRST was the way it was clamped. Heel and toe were about level and the clamp (bowed) was only hitting the edges of the part. I had him raise the heels and put pennies under the toe of the clamps. Next I looked at his settings. I asked what surface speed and feed he was running. He had NO CLUE what I was even talking about. I did some rough math and he was running a 2" rougher at about 300 sf and was feeding at 8" a minute. (the feed was metric and he didn't know how to convert) One clue was the bright blue chips on the table. Taught him some basic math, gave him a Machinists Practicle Guide, patted him on the butt and sent him on his way at 60 sf and .001 per tooth load with a spray mister. He has been in the trade about 5 years, we've had him for 2 of those years. It simply AMAZES me how little we train our people in the US.

The FIRST formula tought is.....

RPM = (3.82 x CS) / Dia


Cutting Speed is Ft/min
Dia is inches

It works for Rotating tool, and Rotating parts.
If the machine does not have the speed you want, use one slower than the formula's result.

If your lazy, use 4, it will be better than a guess.

Get a table of Cutting speeds and learn how to use it.

Piling on behind Ray, if you think education is expensive, try ignorance.

In the early '60's my shop cycled all its machinists (almost 500) through a two carbide tooling class. Year later I asked the supervisor who spearheaded it what the payoff was. He dug out his papers.

One of the things that sparked that carbide training class was the cost of damaged tooling. Most people were running it too slow. They reasoned that because carbide was harder tan HSS they were treating it like it wasn't supposed to wear on the edge. Naturally the brittle carbide of those days crumbled because the necessary heat wasn't present at the cutting edge. Another thing was people would get into trouble and reduce surface speed, feed, and depth of cut.

Mr Wortman told me the training paid off in reduction of damaged tooling alone in less then three months. This was before computers so increased productivity and reduced reject rates were hard to break out but in the heavy lathes and heavy too sections roughing stock reduction productivity just about tripled.

He figured that training cycle was about the best deal the taxpayer got since the Alaska purchase.

Not every part problem can be made to take advantage of carbide's full potential but the machine mechanics should at least be aware of the possibilities.

Does anyone else tend to slow things down a bit when running a manual machine, especially an engine lathe ??? I've found that the few times I did try to figure out surface feed, they recommended speeds and feeds that would be far too dangerous to stand in front of without some kind of guarding, and I found that at these speeds and feeds, I had trouble stopping the machine at the end of each pass. At the shop I work at, I'm given a maximum of 1/8" to hold onto a part, regardless of size, so extreme speeds, feeds and depths of cut can get a little scary. As it is, I often have people stop and
tell me I'm living life on the edge holding onto so little, but it's what I've got to do most of the time to get the job done right.

Absolutly slow it down to a SAFE speed and feed....

Unless your Dale Jr or whatz his name Tony Stewart...your not paid to take the chances they do.

I remember as an apprentice doing a job on a W&S BIG SADDLE type Turret Lathe... Operation was chucking what amounts to a Cast Iron Pipe 8 or 9 inches OD and 4 or so ID and maybe 20 inches long. This is a regular job and Time Study had standards on it and the operation sheet said Turn the OD and Bore the ID at the same time at whatever RPM. Now that's ok, but the speeds and feeds skeeered the hell out of someone not used to this. As far as I remmeber that machine had 40 or 50 HP and all of it was used in that cut.

Botton line... BE CAREFULL

That's the job of the machinist to make the best and most productive use of the time and equipment available. Anything less and you play into the hands of job flight off-shore not to mention a shorter career.

Every place I worked there was plenty of plywood, plastic, and stuff to make quick and dirty chip shields. These days all engine lathes are supposed to have chuck guards. If you want to make the boss enjoy his day work his equipment to capacity not what you think is safe and conservative. If the boss is happy with you your job is more secure and you can bet on a good share of end of year bonuses and first pick of vacation days.

I always run too 'carefully' so I made a display that mounts on my mill to give me suface speed for a given tool diameter.


OK - I was looking for a project to teach myself about microcontrollers and it's proven moderately useful as a starting point to set spindle speeds. Obviously if I had the skills and experience of some of the old hands here I wouldn't need this!

(Last year for example, I was turning 4140 pre heat treated steel way too slow.)

This is another common misconception that I see among machinists. People think that because something has the word "hardened" in it that it must be difficult to machine when USUALLY the opposite is true. That is partially the reason for prehardened steel...makes it easier to machine.
Unhardened would not want to break chips and transfer heat to the tool.
People also think you have to run stainless at a slower SFM because it is "harder" just the opposite is true it is actually quite soft not to mention all the nasty nickel and chrome in it that requires lower SFM.

I think it makes far more sense to calculate the SFM and use your training, experience, and judgement to fudge the numbers you shoot for. After all we generally do not just "take some off" until we get to size, we measure the rough size and take off pre determined bites, and check to make sure we didnt get lost along the way.

Seat of the pants is not gonna get you anywhere very fast if you have to cut a new material that you have never touched a tool to before, the numbers in machineries will let you make a part without ruining it or the tool, that is their purpose.

Bill

I had s.f.p.m. hammered into me when I broke in 30 years. I also have spent alot of time cutting on lathes that were up to 14 feet in diameter.
Calculate the speed for a steel part that is that big. Most people have no concept how slow that is. If you watch the od of the part there is alot of material whizzing by though. Another thing that I would do if there was a lot of cutting to do was find out what speed the insert failed at. Then back off to a safe level. There is no other way to know what your max speed is?

Rockfish;
If you don't know the formulas, most Machine shop
text books, will cover them. There is also a small
freeware program called "Cimco Speed & Feed".
You only have to know the SFPM of the material
you are cutting and the material of the cutter.
It does the calculations for you. But it is in
my opinon that you learn how to use the formulas,
cause you don't always have access to a PC.
Jamie