stainless mayhem

[elraiis]

hi guys.. anyone familiar with S.S? i got few question here this drove me up the wall...

 

first, for S.S 304, 316

AlTiN coating or TiCN?

 

I have AlTiN coated tools.. someone suggested i go high feed and small cuts.. and it runs nice.. but the tool life is horrible. am talking 8500RPM for a 1/2EM and cutting feed of 110in/m. DRY. tool does not live long at all its costing us a fortune.. what should be the proper alternative? or is it normal for the tool to die fast when cutting stainless steel? am not familiar... any suggestions is welcome please...

 

thx.

[88Matt]

How small of a cut? You need to take a bite and take the heat out with the chip. small bites puts the heat in the tool and kills the tool. what coolant are you using?

[Jaz]

AlTiN should be fine. Spindle speed seems excessive, I would start at about 1/2 that for annealed 303/304/316 SS, maybe S4000, F50. Chip load of .0038 might could be increased depending on what you call "small cuts". Dry shouldn't be a problem if you have some good air to move chips out of the way.

[elraiis]

small cuts as in .04 x .5 deep... profiling all around.. no coolant.. for the 1/2. the chips comes out yellow...

[X-L Engineering Corp]

niagaracutter

 

Check this link out I use this all the time to start from with my speeds & feeds

[elraiis]

I used that before ted thanks... i deviated from it because it was too slow... this is the formula then i guess? either slow and longer tool life, or faster and much shorter life?

[Jaz]

At .04 radial cut you should be able to use the entire flute length if you need it and increase your fpt. Try leaving your feed rate alone just decreasing you spindle speed to 4500RPM which give a surface speed of about 600, and a fpt of .0061.

[elraiis]

thanks jaz, i'll surely try that out. dry?

but wouldn't this kill my tool faster hence the load per tooth increased almost to double? or is the main tool death reason with S.S. is the heat so reducing the rpm helps? just trying to grasp the concept!?

[elraiis]

my tool is 4 flutes by the way...

[Jaz]

I was assuming 4 flutes. Yes, dry if you have enough air to get the chips out of the way so you don't re-cut them. By 'air' I mean an air stream directly onto the cutter like through the coolant nozzle instead of coolant, not an air gun stuck through the door, otherwise use flood coolant.

[elraiis]

AIR GUN.. yes the machine is equipped with one... thanks.

[Jaz]

The heat is what is killing your cutter. At only .04" radial engagement your actual chip thickness is much lower than your feed-per-tooth and you do need to keep that up so the cutter has something to 'bite' into and give a big enough chip to carry the heat away. The higher feed rate may make a problem if you have to dive into an internal corner somewhere resulting in signifigantly larger actual cutter angagement.

[elraiis]

thanks alot... do not worry about gouging at corners i relief those to be sure of a consistant cut... what about ramping and helix cut depth and feed? i noticed my tool die the most when there is some sort of material removing while going on z axis such as ramping... i feel really annoying asking for all this help.. anything would be appreciated guys.. thanks alot already for all

[X-L Engineering Corp]

I've had 3fl radius tools work really good with this material but I never ran dry always with coolant.

[Jaz]

quote:

---

what about ramping and helix cut depth and feed? i noticed my tool die the most when there is some sort of material removing while going on z axis such as ramping

---

Most end mills are not really made for end cutting although they can do it. Set your plunge feed rate to what would work good for slotting or a little lighter then set your parameters to use the plunge feed rate when ramping down. In this case I would be looking at about F50 with 5 degree ramp angle. The shallower the ramp angle, the faster your feed rate can be.

[elraiis]

thanks alot guys.. i don't care if all this is actually going to work or not.. i'll try and i hope it does.. but even if it doesn't.. still thanks alotttttt for all the help.. am going to test whatever you gave me today hopefully..

 

thanks again..

peace

[Jaz]

Keep us posted.

[Justin Beebe at Folsom Tool]

elraiis,

 

What endmills are you using? Have your tried Hanita Varimill or Niagra Stabilizer?

[Watcher]

+100 for Hanita Varimill

+1000 for Hanita Varimill II

[MACHINEMASTERG]

we cut alot of 316 ss and its the rpm's that are killing your cutter like they said before around 4000 should be the rite rpm

[[email protected]]

I'm cutting 303 right now 4510 RPM @ 64 IPM 1.09 ADOC and .05 RDOC, air blast,tiAln(s?) fraisa P5926.530 (.500 w/.09 Rad Bullnose)

 

www.fraisausa.com

 

HTH

[tooljockey]

Download the TOOLEXPERT from Fraisa here:

 

http://www.fraisa.ch/CH/EN/NAV/PRODUCT/ToolExpert.aspx

 

The Fraisa NX-NV's (Variable Helix tools)& SX series cut 303/304 stainless like butter!

The Fraisa tools kick Hanitas A**!!!!

[[email protected]]

quote:

---

The Fraisa tools kick Hanitas A**!!!!

---

I agree 100%

 

[hijack] Is Steve your reseller? [/hijack]

[Carl Hessig]

tooljockey works for Fraisa. He also has about 10

 

yrs of using mastercam building molds and more than

 

20 years of machineing. Steve use to work this area

 

but Brian took over a few years ago.

[elraiis]

hi again guys... unfortunately i can't get my hands on hanita varimills or fraisa... i know for sure that those are higher end tools but as they cost more, they won't buy them here. So am stuck using lower end coated mills... unfortunately. i did my first test on mild steel as in keeping the feed up and only cutting my rpm.. i liked the result.. even the sound of the cut was nice and smooth so far.. so tomorrow... i'm biting some stainless..

by the way, if i'm going 4500rpm while cutting with a 1/2 AlTiN coated Em... does that mean i should run at about 8500rpm when cutting with a 1/4EM coated? won't that be much? and is there another type of tool coating that would give better result than AlTiN for Stainless cutting?