Feed & Speed for Inconel

[Rookie Cam]

Help!Never work with Inconel, I need help with feed and speed, try to machine 2 X .400 X 1.125 Deep Slot and .372 Dia X 2. through hole on the side of 4.720 Cylynder. I try those parabolic cobalt drill => it's not woring, now using cobalt drill (Cleveland brand!!)to drill .281 pilot hole for .372 Dia with F.15 X S250 X .01 peck. for the slot i use 3/8 rough carbide EM(accupro brand!!) F.4 X S300 X .1 Step. Am I too slow? Using the right tool? Thank You for Your time

[Guest]

"assuming" Inco 718

 

Set your drill SFM to about 60-70 and your milling to about 90 SFM.

I would use between a .001/.002 CPT feedrate

 

Start there an bump up as you can.

 

And make sure you maintain a chip, you don't want to "rub" the stuff

[Guyinthedesert]

Help!Never work with Inconel, I need help with feed and speed, try to machine 2 X .400 X 1.125 Deep Slot and .372 Dia X 2. through hole on the side of 4.720 Cylynder. I try those parabolic cobalt drill => it's not woring, now using cobalt drill (Cleveland brand!!)to drill .281 pilot hole for .372 Dia with F.15 X S250 X .01 peck. for the slot i use 3/8 rough carbide EM(accupro brand!!) F.4 X S300 X .1 Step. Am I too slow? Using the right tool? Thank You for Your time

 

I would recommend Guhring carbide drills. If you use cobalt drlls, 15 sfm, don't peck, don't spot drill, and dont ever pilot drill.

With your carbide em, try 50 sfm, .003 cpt. go as deep as you can, with a .1 step your just going to wear off the end on the tool

[Rookie Cam]

Thank You much

[JAMMAN]

We do some inconel 713C I believe, I stopped drilling pilot holes because the pilot drills would last but the next drill would only last a couple holes. I put a small spot with a carbide center drill (just tip depth) and let the drill take the full cut the first time. Heavy concentration on coolant, I ended up using carbide tipped Cleveland drills. I tried about 20 things before this, solid carbide, cobalt, HSS, and I get the best holes from a carbide tipped drill/no pilot/no center drill hole (just spot for location).

[brandon b]

Wow! My first attempt at inco today. .. what's the trick to drill a .5 dia hole 4 inches deep? All I can use are cobalt drills. I'm running 200 rpm 2 imp .05 peck flood coolant. I can get about 2 inches deep,just can't get the heat out,and it work hardens. .

[Guyinthedesert]

Wow! My first attempt at inco today. .. what's the trick to drill a .5 dia hole 4 inches deep? All I can use are cobalt drills. I'm running 200 rpm 2 imp .05 peck flood coolant. I can get about 2 inches deep,just can't get the heat out,and it work hardens. .

For a cobalt drill, you speed is way too high, your feed is WAY too high, and each peck you take is like rapping the end on the drill with a ball peen hammer.

 

I've been having good luch with OSG VPH drills.  They are powdered metal, so they're  nowhere near the price of carbide and they work great ininconel.

[Greg_J]

IMHO,

 

5 SFPM for hss dills small peck .03, .001-.003 FPR for Inconel 925.

 

100-110 SFPM for indexable tooling for roughing, roll in and out of your cuts for better tool life.

 

You can run faster SFPM for profiling just use the chip thinning formulas to increase your feeds.

 

On average it takes 6 times longer then the machining time of 4140.

 

If  your doing a lot of machining bring up the concentration of your coolant, rich coolant helps with machining.

[brandon b]

Ok I'll try that. As for roughing I'm using pct curve cut.75 cobalt rougher. Running 325 rpm at 5 imp. It seems to be running pretty nice now. .375 step down. .25 step over using dynamic core.

 

Then using area for the pocket.but the helix entry is killing these cutters. What angle is easy on the em?

[Guyinthedesert]

Ok I'll try that. As for roughing I'm using pct curve cut.75 cobalt rougher. Running 325 rpm at 5 imp. It seems to be running pretty nice now. .375 step down. .25 step over using dynamic core.

 

Then using area for the pocket.but the helix entry is killing these cutters. What angle is easy on the em?

I would use a start hole

[Greg_J]

I found that depth of cut doesn't matter so much in Incoloy / Inconel, your running pretty slow anyways so heavy cut is doable if you setup is rigid enough and you have a way to keep the part cool.

[brandon b]

Ok my helix bore pitch was set way too high. Brought it down to. 01 and it was golden. Drilled three .5 hole with one drill at 130 rpm 1 imp .03 peck. 2 inches deep

[Greg_J]

When I mentioned depth of cut didn't matter so much I should have stated that plunging into air and milling into the part is what I was meaning.

 

My last incoloy job I had to drill a 2.0 hole 8.125" deep from both sides of the part 16.25" in total using a Ingersoll quad drill 5xd 240 rpm @1.0 ipm (125sfpm, .0021fpt), then using a 2.5" high feed tool helix bore to 3.5 dia. through 191 rpm @ 15.28 ipm (125sfpm, .020pft,.03 pitch).

[brandon b]

Don't think our fadal. Can handle that lol.