Constant Surface Speed

[raymond1]

Need Help On Calculating The Constant Surface Speed On The Lathe How Do You Know What To Put In For A Part That Has A Big Diameter Of Say 20inches And A Small Diameter Of 12inches. Its Sst.

[Willbird]

I'm not sure what your asking exactly ??

Typically with constant sfm you clamp the max spindle rpm so it does not run to the max the spindle can run when it faces to center, it is important to consider the centrifugal force on your chuck jaws when using constant sfm. If you wing the spindle too high of an rpm the chuck may explode, the part can come out, small animals may die, you may die. Often a clamp on maximum spindle rpm (by G or M code) is a very important part of a cnc lathe program often overlooked.

The cheap and dirty formula I use is
(SFM * 4)/dia of part = rpm

it is not exact, but it IS easy to remember...and it errors to the conservative side on the rpm.

[raymond1]

HOW DO YOU FIND THE (SFM) IS THERE SOME KIND OF CHART AND ALSO CAN YOU DISCRIBE ON EXAMPLE. LIKE SAY I AM MACHINING A ALUMINIUM PART THAT IS 14 INCHES IN DIAMETER HOW WOULD i FIND THE RPM FOR THIS PART

[ricotututi]

SFM is a myth you get this from the tool manufacturer, or there is something standard with high speed tools or cardide, and then it depends what type of material your cutting, and if you are using coated tools then the SFM might double or triple.
From what I remember usualy for
High Speed tools is about 50-100 for steel
Carbide about 200-350 for steel
for alum it probably can be twice than for steel
for Stainless Steel its probably 25-50% lees

and example would be
lets say you are machining
a 1.0 diameter aluminum bar stock
your smaller machining diameter is .500

Then you calculate 350(SFM) x 4=1400 / .500(smaller diameter)=2800(RPM)
This means that when your machining your .500 diameter the lathe will running at 2800RPM .

then you have to input this information in the program

What I use is something like this

G50 S2800 (this is the maximum RPM the machine will run)
M3 S1000 (this is the RPM at which I will start the spindle before start cutting)
G96 S350 (This tells the machine what is the SFM, so the machine will calculate and change RPM accoding to the Diameter)
hopefully this makes sense.

[raymond1]

Thanks For The Quick Reply .by Any Chance Do You Know Where There Some Kind Of Chart Where I Can See On All The Material And What To Punch In For The (sfm). Also Do You Know If They Sell Some Kind Of Calculator Not A Software. That Will Figure All That Stuff Out For You.

[philbur]

Try:

http://www.niagaracutter.com/techinf...eed/chart1.gif

Or google "speeds and feeds"+chart.

Regards
Phil

Originally Posted by raymond1 Thanks For The Quick Reply .by Any Chance Do You Know Where There Some Kind Of Chart Where I Can See On All The Material And What To Punch In For The (sfm). Also Do You Know If They Sell Some Kind Of Calculator Not A Software. That Will Figure All That Stuff Out For You.

[Geof]

Machinerys Handbook has all that type of information; no calculations are needed. For example if the cutting speed for is 450 fpm your program needs the command G96 S450 to start the CSS. Depending on the size of the material you will have a G50 Sssss spindle clamp command; if your work is large you might want to clamp the spindle to a low or medium rpm and if your work is small you might use a faster rpm. The spindle clamp has nothing to do with the required sfm it is for safety as you do not want the chuck to loose grip at very high rpm on a large part.

Incidentally the chart philbur linked is for milling cutters. It is not always valid to use the same sfm for a lathe tool because the cutting conditions are very different. Lathe tools are always buried deep in the cut and may overheat if run at the same sfm as a mill which often spends 50% of its time away from the material and freely exposed to cooling air or coolant.

[Willbird]

easiest to remember is SFM x 4 / DIA = RPM so for a 1" cutter running 150sfm

100 x 4 / 1 = 400 rpm

To never melt a cutter in any unknown steel that is not harder than 4140ht I simply use 50sfm for HSS and 150 for carbide, this is for milling machines that are not super rigid, this is quite conservative. but often the cut takes less time than looking up the EXACT speed/feed for A2 steel, or D2, or 4140ht


Bill

[Newby2]

For those interested, I run stainless at 200fpm roughing, 350fpm finishing. Depending on the steel being turned, I run 12L14 at 750fpm@.09DOC for roughing, and 1100fpm finishing@.015 DOC. 8620 will run a little less, but not much, with the DOC remaining the same. These are using flood coolant.
The Seco/Carboloy recommended feeds and speeds are higher than that but the tool life is greatly less. I use TIcn coated inserts but find the TINal inserts last longer. I can run 4 hours (half a day) on one corner, index the insert after lunch, and run the rest of the day.
Another thing interesting is that the insert manufacturers are placing the various materials in catagories based on the materials machinability and placing this information on the label of the insert container.
The formula I use for SFPM is simple, Pi * DIA/12 * RPM. (Pi =3.1416)
Steve

[DocHod]

To let you know not all machines controll the max. R.P.M. by using G50 one of our controllers uses a G92 for max. R.P.M.