Silly Question BUT What Unit is Feed in on a Haas Mill

[JWB_Machining]

Yes, This is probably common place to you all but is the Feed rate that you enter on a Haas Mill (TM-1) in surface ft/min or in .001 in/tooth?

Also I was just using a 0.3125 4 flut Carbide Endmill to mill a ccw circle in a 0.25 thick piece of aluminum. I had my spindle speed set at 4000 and my feed set at 64. However there was a horrible screeching sound being produced, what gives?

Remember good machinist don't mock novice machinists when they ask questions, they simply instill their knowledge. Thanks.

[ckirchen]

inches per minute

[JWB_Machining]

Ok so let me make sure I understand this correctly. When I go to the Machinery's Handbook and look up a speed (ie. Aluminum 6061 HSS End Milling Avg. s=850) I would take this value multiply it by 12 giving me a feed of 10200. Would I enter that as F10200 which would be F10.200 or would I enter it as F10200.0 Which would be insane? Sorry, I'm let loose on a TL-1 and TM-1 all day and there's no one there to help me other than the Machinery's handbook and this website. I'll be honest I can't believe I'm getting paid to do nothing but try n learn these machines all day.

And then with this speed of 850 to determine my RPM I would use the ol equation

RPM=3.82 x SFM / Dia?

So for a 1" cutter this equation would be

RPM = 3.82 x 850 / 1 = 3247

So I would have Spindle Speed of 3247 RPM with a Feed of F10.200 for a 1 inch cutter? Is this all right or what am I missing?

-JWB

[Geof]

Where did you get the 64 from?

To give a complete answer the feed is entered into the program in inches per minute, as in F10.0 for ten inches per minute, but it is obtained from the inch per tooth figure taking into account the number of teeth, the cutter diameter and the surface feet per minute (sfm) for the material being cut.

Carbide on 6061 can be run at 2000sfm which is 24,000rpm for a 5/16" cutter, obviously you don't go this fast with a TM-1 so using your maximum speed of 4000rpm is correct.

The feed per tooth for a four flute cutter in aluminum should not be much more than 0.001" so each revolution of the cutter can take 0.004".

Four thousand revs per minute multiplied by 0.004" per rev gives 16 inches per minute for a feed of F16.0 (which is why I wondered where the 64 came from).

Possibly you used F64 without any trailing decimal? The machine interprets this as 0.0064ipm which is a bit slow; your squealing may have come from the cutter rubbing rather than cutting.

Incidentally I suggest avoiding four flute cutters on aluminum unless you are wanting to get a fine finish while removing only a very small amount. Two flute high helix cutters will remove material faster without jamming chips in the flutes. Also always use coolant, flood preferably but on a TM-1 you may get a shower so you have to compromise.

[ckirchen]

You're right on the rpm, but I would ask the cutter manufacture for SFM. I use Garr and they have charts in the back of their catalogs.

To figure out feed, use rpm * no_of_teeth * feed_per_tooth. You can usually find FPT in the same chart that gives you SFM.

For example, my Garr catalog list SFM as 500 minimum and FPT at about .003" minimum for a Ø1" carbide cutter. With a 4 flute cutter, the numbers are RPM = 3.82*500/1 = 1910 rpm and Feed = 1910*4*.003 = 22.9 ipm.

I just noticed that Geof beat me to the punch...hopefully this is helpful anyways.

[Geof]

Originally Posted by JWB_Machining ....there's no one there to help me other than the Machinery's handbook and this website....-JWB

For the moment it may be less confusing to ignore Machinery's Handbook and just post your questions here. You may sometimes get conflicting answers depending on the differing opinions of different posters and if that happens ask for explanations.

[JWB_Machining]

Where did you get the 64 from?

I got 64 from the program that was put together by the Haas training technician who came in and taught me for a few days. I'm sure however he was smart enough to turn down the feed because I recall when he ran the program with those settings it went perfectly.

Thank you for all the information I'll try and remeber all this when i'm trying things out on the machine today.

And because you invited me to it you'll be seeing a whole slew of questions from me. I did a bit of machining when I was in college this past year building an SAE Baja car, that got 7th out of 94 BOOYAH but everything at my school was manual so when it came to speeds on the ol Bridgeport Fastest Was Aluminium and Slowest Was steel, feed was determined purely by feel and how the chips loked coming off so knowing what feeds n speeds to use is my biggest learning curve while processes and clamping and stuff I already know. Now that I actually feel the need to know the specific material i'm working with beyond the two categories of steel and aluminium I feel a bit over whlemed but thanks for all the help.

You can expect more Newbie questions in the general metalworking section to come.

-JWB

[JWB_Machining]

I'm putting a post up regarding Coolant in the General Metalworking Forum, if you guys could check that out and educate me when you get a chance that would be great.