need ideas for 304 SS pockets

[mchin-pilot]

I mentioned feed mill before.

There are other makes/brands if you really want feedmill that size.

[Reko]

Who makes 3/8" Feed Mills? Are they any good?

[Guest SAIPEM]

Your cutting speed is way too slow.

 

What I would also recommend is that you create several different Ops in MC.

Have each with 20 slots.

Force a toolchange and a program stop with a prompt to the operator to change the tool.

 

If nothing else you'll prevent the gouging when the tool breaks.

[Goldorak]

rougher 7/16 to rough the slot with a ramp entry

 

3/16 end mill to finish and avoid the tool to stop in the corner using morph pocket with an additional finish contour operation

 

 

we use niagara elite SR 420 for roughing ans S545 for finishing

 

rougher at 350 SFM and .003 to .005 IPT

 

finish a 550 SFM .002 IPT (5 flutes )

 

this should make easily 80 to 100 slots

[Dave Ball]

quote:

---

Who makes 3/8" Feed Mills? Are they any good?

---

SECO has a line of solid carbide HFM cutters that range from 1mm to 12mm, they are pretty impressive in my experience.

[cunder]

I recently used a variable helix endmill from Contour 360°. Milled 56 slots about .375" wide 77" deep 15" long with one tool. Did have coolant thru. On our some tool holders We wire EDM small half holes for coolant along the shank of the tool.

[cunder]

that should be .77" deep

[jeff]

I would definitely get the Hanita Varimill to rough them out. (280 SFPM and .0014 per tooth chipload)

They are excellent for stainless,and I use them for just about any other type of steel/alloy also.

[tooljockey]

http://www.fraisa.com/CH/EN/NAV/PRODUCT/e-Katalog.aspx

 

Fraisa has a new line of high performance tools with high feed endmills from 3mm-16mm. They are in the "tool and mould" catalog.

[tooljockey]

http://www.fraisa.com/CH/EN/NAV/PRODUCT/e-Katalog.aspx

 

Fraisa SX series tools last forever in 300 series stainless.

 

Also, try the U15990 Variable helix tools from the INCH catalog. I have seen these outperform Z-Carbs, Varimills, Stabilizers, & Data Flutes in many applications.

[[email protected]]

+ 10 billion on Fraisa

[BBprecise]

I've used Iscar's multi-master cutters in similar situations as your's with good results. We ran 2545 rpms' with a feed of 163 IPM with air and not coolant. Kept fracturing inserts with flood coolant, to bad they aren't coolant thru.

[Nick Eaton]

I think the important thing here is the surface footage rather than the actual type/brand of cutter.

Bear in mind that carbide has to reach a certain temperature to cut efficiently. Too low a surface footage is ALMOST as bad as too high a surface footage as far as tool wear is concerned.

This is why simply "slowing it down" often leads to nothing but lost profit,

 

Nick Eaton

[left coast lefty]

Thanks to all for the help!

 

Hardmill, I took your advice on the ramping and the endmill looks great after the first two slots.

 

Thanks again!

[Hardmill]

Good to hear

 

 

PEACE

[NOTW Programmer]

I would use Dynamic Mill, RPM 5100 IPM 98; for the entry Helix .025, Angle 2.0, Ramp IPM 20, Ramp RPM 3500, 3s Dwell. MasterCAM calls for a 9 minute cycle time. You still have to use a finisher for the corner radius.

[Goldorak]

you are just 16 months lathe , i think he get the job done .......i hope