Advice on face mill use.

[Kalvin]

Busy Bee has a little sale going on so I could not resist.

I picked up a 2" End Mill with Carbide inserts.

http://busybeetools.ca/cgi-bin/picture10?NTITEM=B2136R8

Any tips you can share with a novice? How to calculate speeds and feeds for different material?

What kind of life can I expect from the inserts?

Will I be able to face stainless? (Being carbide and all.)

I did a little reading last night, should I have got a unit with more inserts? I read that three inserts can cause a lot more vibration when approaching from the side of work piece.

Cheers, Kalvin





Thanks guys.

[pzzamakr1980]

Facing stainless is easy enough to do. The amount of material removed in each pass will depend on the size(rigidity, dampening mass) and horsepower of machine. Feed rates will depend on your machine and to a certain degree rpm. If you have vibration try increasing feed rate and decreasing rpm's. This will work as long as you aren't trying to remove huge amounts of material with a small mill. Start with a low depth of cut and increase feed rate and depth of cut until you get poor surface finish and excessive vibration.

To calculate rpm use this formula.

For carbide tools only use the value (500) Other materials, have different values. Stainless with High speed steel cutters would be 50 or 60. Aluminum would be around 100. Keep in mind the given rpm is conservative and only a reference. But its a good starting point.

500*4/diameter of cutter.

[Kalvin]

Thanks pzzamakr1980,

I went ahead and tried some stainless on my own. Not too much luck.

I will try your recommendations and see how it turns out.

Is the formula you posted "500*4/diameter of cutter" for a four tipped cutter?
The cutter I have has three carbide tips.

I'm using and X3.

Cheers, Kalvin

[rwestbr]

Kalvin check this out, I bought one about 2 weeks ago and it works great.

http://www.wttool.com/product-exec/p...rts_WT_Import_

Hoss originally posted a link to it a little while back.....

Robert

[JoeyGH]

coming from working in tool and die. That 500 is way too high for stainless steel. 300 would be far more realistic. And a a chip load of .007'' or .008'' per rev in stainless. In normal steel .005 to .006'' chip load per rev. That is you'll have to devide that .007-.008" by 3 to get your chip load per tooth. Also that is assuming your using coolant. Stainless is relentless even on carbide and generates alot of heat. The old saying I also use to hear with stainless is half the speed double the feed. This works to an extent because if you don't get the chip out of their it tends to gum up and stick to the cutter it will go way down hill from there. Hope that hopes. Once you got that surface footage (300) and chip load per tooth you'll be able to get your rpm and feedrate.

[JoeyGH]

Thanks pzzamakr1980,

I went ahead and tried some stainless on my own. Not too much luck.

I will try your recommendations and see how it turns out.

Is the formula you posted "500*4/diameter of cutter" for a four tipped cutter?
The cutter I have has three carbide tips.

I'm using and X3.

Cheers, Kalvin

Also one more thing you have the formula correct and it's universal independant of how many flutes/inserts your cutter hows. Where that comes in is the feedrate. Which is rpm*chiploadpertooth*number of flutes. Ex. Which the numbers I gave you assuming you have a 2'' face mill. 300*4/2=600rpm. Feedrate EX 600*.0026666*3=4.8inches per minute. That should be a good starting point. If you were running a Full size cnc your would mostly likely buy inserts designed to cut stainless then in conjunction with a great coolant system your could push it alot fast. Hope all my ranting helps

[kingfisher]

Lots of variables to consider.....what type of carbide? Coated or uncoated? I can give a good speed and feed rec if you want to call me or shoot me a email so I ask some questions. With Stainless you need coolant, richer the content the better. What type of SS? Just changing from 303 to 304 makes a big difference. Having to low of a feed rate can wear tools out faster also. SS is abrasive and slow rubs the cutting edge, best to use positive sharp tools when possible because its gummy.

I am a factory rep that does this for a living I would be happy to help you if you want to contact me.

Bob