facing and tapping 304 stainless

[1cnchogger]

Having trouble with a 304 stainless 3in by 3in extrusion 60 in length. I have to face it and tap 3/8-16x40 times, they go in .7 in depth . The hole size is up to 9mm just to get that many. I'm running 300rpm with feed of 18.75ipm. I have rigid tapping on my VF3 Haas mill. I have been using a greenfield roll tap with no luck(might get 30 holes). I have iscar 3 in facemill that eats through the 928 inserts, lucky they are four sided. I only have to take 1/16 off face. Question-Has anyone had any luck with tapping s/s in this way, or should I forget about the roll form all together. Also, anyone using anything different to face?

[mark c]

What is your speed and feed for the face mill? What type of oil/coolant for the tap? Spot drill or center drill?

[cdlenterprises]

OSG Hypro High spiral taps. Those have always worked well for me in 304. I haven't had much luck form tapping. Try IC328 for your facemill @ 300 sfm.

[1cnchogger]

speed and feed for facemill is 650 rpm feed of 10.00ipm. I tried speeding up but burned out quicker. I've tried the iscar 328 not much of a change. I think the problem is I'm conventional milling with a 3.00" cutter. I'm trying to get in a 6.00" button cutter to see if climb milling will make a difference.

[1cnchogger]

syntillo 9954 is what I'm running for coolant. Tap seems to be shattering. It's funny the previous holes are fine. No sign of fatigue until it breaks. I am centerdrilling.

[VMC_Jeff]

We machine alot of 304 SS and have found it is one of the least predictable material to machine. One week we get material in that machines great, the next week it machines like granite. I'm sure it has to do with the nickel or chrome content varies from batch to batch. Just my opinion.
We found the Iscar 28 or 328 grades to hold up a little better than the 928. Thread forming usually only works in shallow holes. In the deeper blind holes we use a reverse spiral emugee ticn coated tap. Drill as large as you can and still pass inspection. Even then we found there is usually no warning before they shatter.
Good luck
Jeff

[cdlenterprises]

Sounds a little high on the rpm. I generally try to run 300 surface footage which would calculate to about 400 rpm for a 3" cutter. You have to "push" cutters in 304 or else you'll work harden the material. Try to reduce the rpm to 400 rpm or so and leave the feedrate. As far as the tapping, have you tried a tension and compression holder or a tapmatic tapping head? They tend to be a little more forgiving should you hit a hard spot in the material or bind up the chips. Keep us posted...

[Hogger]

We tap a lot of 304 in the lathe and mill, we use spiral flute USA made taps and run them at 25 FPM but haven't had much luck using coolant, we have to use Castrol Moly-Dee cutting oil to get the taps to live, but can get 1000 or more 3/4-16 by 1.5 in. deep threads done on a single tap, we use forming taps on 3/8 and smaller taps but still have to use Moly-Dee to get any life out of them.

[1cnchogger]

Found solution to facing problem. Iscar rep brought me in an octagonal insert. I have been using it without indexing once. I would have gone through a pack of 928's. Cutter is a ISCAR 3in HOF D3.00-5-1.00-R07 inserts are OFCR 07T3-AEN. Unbelievable difference. I think it may be the clearance allows the chip to be expellend rather than drug along the face. I'm still looking into the tap and drill. Thanks for advice on holders, speeds and fluids.

[jackson]

also dont use coolnt when facing

[protopath]

Try a spade drill, we have pretty good luck with those in 304. 304 is like fossilized bubble gum, hate that stuff. We also do not rigid tap it, we use a tap head and never use a form tap.

[1cnchogger]

What kind of spade drill are you running? Make, size, speed, feed etc. I need to drill 8.75mm for the form tap. Might try compression tapping head now. Much appreciated