CNC milling/lathe cutting speed

[rEtarD]

Guys, sorrie i posted in the wrong forum, theres just so many of them and i think this is the best match.
Ok, anyway im currently studying Mechanical Engineering technician cert and i chose CAD/CAM as my specialisation. Currently my teacher is covering on the topic CNC milling. I did CNC turning on my free-time, ( i took up an extra module on that ) with FANUC 21iT and HeidenHein simulation program, i think its named AutoPilot or something.
I want to ask a simple question about the preferred RPM, feed rate and spindle speed to use for different materials and also considering the material of my cutter. I think my teacher said it was steel or even carbide, i forgot.
I wish to look for a chart or something so that i could cut properly without damaging the finishing or wear out the cutters. ( is it true that if i cut with low spindle speed and low feed rate, Carbide cutters will wear out faster ? )
Do anyone has any to offer so that i could use on FANUC 21iT or LEBLOND MAKINO 2 Axis antique milling machine ?

[Karl_T]

Everything "depends". Your best bet is to go to a vendor web site and look at a given insert and material. They will give you a table of DOC and SFPM for a given material. It will be a large range. Where to operate in this range depends on your machine; rigid high horsepower machines at the top end.

There is a HUGE difference in capability of inserts. Find tables on generic TPG inserts and compare to one of the best: Sandvik R390. Of course a Sandvik insert costs more than five TPGs. http://www.coromant.sandvik.com/

In the real world most machinists just get a feel for what their particular machine will do with a given insert. A rule of thumb my machine shop instructor taught me about carbide,"If your chips aren't blue, you're going too slow"

If you ever run a production job, the insert and toolholder vendors will help optimize inserts, speeds and feeds. And give you trial inserts and holders to try.

Karl

[BillPSu]

Probably the most widely used reference book for an engineer, toolmaker, and machinist is the Machinery's Handbook. It will cost $50-$100 depending on new/used and edition but it is by far one of the best reference books you will ever purchase and it has machining speeds and feeds recommendations.

You will eventually learn these are starting recommendations and depending on your fixturing, rigidity, length of tools and a myriad of other factor will have to be modified to each machining operation for optimal tool performance.

[rchprks]

as a rule of thumb, hss(high speed steel) uses lower rpm and feed rates than carbide. if you run carbide at the same rpm and feed as hss you will dull the cutter quickly

[rchprks]

guys! my boss (die maker) thinks carbide is majic, he is constantly handing me hardened d-2 and telling me to "just buzz off a half thou or so" where can i find info on maching hardened tool steel ( milling machine0

[HuFlungDung]

I cannot say that I've ever run carbide at low surface speeds as I would high speed steel, to know if "running slow dulls the edges or not". I mean, what is the point of running a high productivity tool at the production rate of yesteryear?

Perhaps recutting of chips damages the tools more than anything, and a slow turning milling cutter has less tendency to throw the chips out of the vicinity.

What often happens, is it seems the novice will hear about running carbides fast, so he'll run the hell out of tool, and yet feed it as if it were HSS running many times slower. So sure, run your carbides fast, but feed them heavily, to match.

I don't say the speed is "good" for the tool, although this was more of a case in the early days before carbides were coated. When cutting below a certain critical speed ( around 400SF/M), steels were bad for welding to the surface of the carbide, then breaking away, pulling chunks out of the carbide surface. This causes a crater to form at or behind the cutting edge, and soon spoils the smooth flow of the chip over the rake face of the tool. Then the tool will fail.

This still happens a lot if using the wrong coating for machining the austenitic stainless steels: the chips will eat a notch out of the tool at the depth of cut mark.

When cutting fully hardened steels, you should likely slow down a bit, to prevent overheating the substrate, and let one of the fancy coatings do its work with preventing premature tool failure.

[gripper]

On the machines i run which are Bridgeport CNC lathes, on alimimum using carbide tooling with ali geometry I would run on a 2" bar of ali at 2800-3000 rpm at a feed rate of .3mm(.012") a rev and a depth of cut of 3mm(.125") .
On stainless steel 303,using carbide tooling with steel geometry. Run a 2" bar at 1400-1600 rpm at a feed rate of .2(.080") too .25(.082) per rev and a depth of cut of 2mm(.080"-.085")
On stainless steel 316 reduce everything by about 15% - 20%. On larger size bars you should use constant surface speeds, for ali about 300-400 metres a minute, on 303 stainless about 180-200 metres a minute and for 316 stainless about 100-130 metres a minute.
As for turning Hardened steel, we us diamond tip tooling and it a piece of cake! Speed is 100 metres per minute and a feed rate of .1(004") per rev and a depth of cut of .1(.004) and you must not put any coolant on the job or the tip as it will break. The swarf comes off red hot and in one piece. do not touch the tip when assembleling in the tool holder as this will get grease on the tool and it will affect the tool, must be kept grease free and that inculdes what you are turning.

[rchprks]

gripper!
thanks for the info, i definitely want to look into dimond tools,(if i can get the cheap SOB i work for to pay for them) once again thanks

rchprks

[Geof]

Originally Posted by gripper On the machines i run which are Bridgeport CNC lathes, on alimimum using carbide tooling with ali geometry I would run on a 2" bar of ali at 2800-3000 rpm at a feed rate of .3mm(.120") a rev and a depth of cut of 3mm(.125") .

Gripper; you did not pick up your typo. .3mm(.120") (sic) a rev??? Mind you a typo like that here does not create a flashing red light. I have done similar ones editing on a machine much to the amusement of my guys.

[gripper]

Your right Geof, it should have been .3(012") thats what you get when you try to think and type! When I do it at work ie forget to put in the right amount the turret usually ends up behind the chuck!!!
The cost of the Diamond tips are about £65-£80($110-$144) and only have one side.

[Geof]

Originally Posted by gripper Your right Geof, it should have been .3(012") thats what you get when you try to think and type! When I do it at work ie forget to put in the right amount the turret usually ends up behind the chuck!!! The cost of the Diamond tips are about £65-£80($110-$144) and only have one side.

As the guy who pays the bills I am not sure which is the worst thing about trying to exchange the relative positions of chuck and turret: paying for everything to be sorted out; or enduring the smirking from the guys. I sorted things halfway a few years ago when my guys asked for a four day week; now I have Mondays without witnesses. And you know the funny thing is now I rarely do anything that could be embarassing on Mondays so I came out ahead both ways.

[gripper]

The only good thing about me putting the turret behind the chuck, is that I can rebuild the machine without the boss having to call the service guy. If I have a real bad crash i.e. spindle moved and turret off centre and twisted, I can usaly get it back up and running within 4-6hrs and with in the machine manufactures spec's which is about .002mm in any direction. I have had to do this about 3 times in the last 2 years. When you think that I do not use a cad/cam program to write my programs, I just have a drawing and stand in front of the machine and punch in the numbers and work most things out in my head or with a calculator and then prove the program with my finger on the stop button and feed rate! I hope this doesn't sound big headed, it's that I've been around machines for a long time and had a lot of good teachers and a lot of frendly service engineers who are willing to pass on thier knowledge, just like the people here on this site.