Deep holes in 304 SS

[Clarence]

I am trying to drill a 1/2" hole approximately 6" deep in 304 SS. The holes are for heating cartridges for a heat staking machine.

 

We had a 1/2" dia. by 12" long 135 degree cobalt aircraft drill. It got to about 3 inches and stopped the spindle. 534 rpm @ 4.28 ipm. When I tried to remove the drill, it broke in the hole.

 

Any help is appreciated.

[Colin Gilchrist]

I would start with dropping the feed about 20%, you are doing .008 per rev in stainless. Are you pecking? You really need to peck or at least run a chip break cycle. I would use full peck and return to .1 above the hole to help get coolant down in the hole.

 

To remove broken drill bits, I chuck up an old worn out, center cutting endmill, crank up the RPMs to about 7500, and feed the endmill down onto the broken drill really slow. It basically burns the drill out. Just be really careful and go slow. I've rescued quite a few parts this way. Sometimes I'll do it with a slightly larger endmill, then drill the hole oversize and install a helicoil if necessary.

 

HTH,

[Clarence]

Yes I am pecking with a full return to help evacuate the chips and allow the coolant to pool in the hole.

 

I am going to try and use an old endmill to remove the drill pieces.

 

Thanks.

[MACHINEMASTERG]

i would also start out with a stub drill go as deep as posible then step up to the next longest drill a taper lenth drill has an overall lenth of 7.75 that should do it the drill your using is kinda long

[Goldorak]

do you have thru coolant on your machine

 

if yes,osg makes an 18x drill

 

linky to osg

[Clarence]

That is a good idea with the stub drill. I will give it a try.

 

We do not have coolant thru.

 

We use Blazer 2000 coolant. I will also check the concentration.

 

Thanks.

[Goldorak]

ok

so boost your concentration to provide a little more lubricant

 

i will try a .025 peck and full retract every .1 to .125 and set rapid override to 50% to let coolant go to the bottom of the hole between each retract

 

and leave hour hand on the red mushroom

[horsepowered]

I would use a parabolic tin coated non cobalt Guhring drill. Run 400 rpm @ 4.0 feed .350 peck. Cobalt is great for wear resistance but tends to grab in malable material such as 304ss and break. I would net be afraid to up the feed a little above the 4.0.

[Clarence]

I am checking now with my tooling supplier now. With what he has available, I may go with a smaller drill and then ream the hole. I have to check the length of reamers I have in the shop.

 

Thank you for all the information.

[?Mark]

Waaay too fast.

Good starting point for .500 hs-co drill in this material is S306, F1.2 and Q.1 at the most for this depth.

If there is a lot of holes you might want to consider investing in a coolant thru setup.

edit:

why would you want to use smaller drill?

hth

[Clarence]

I will slow everything down. I haven't machined much stainless, but I have heard that if I go to slow on my feed, I will work harden the material.

 

At 534 rpm, with a 1/2" drill, I am at 70 sfm. From everything this thread is telling me, I am still way to fast. I will slow it down.

 

I appear to be taking way to much per tooth. I will slow that down also.

 

The smaller drill and ream is only what I can get fast. I only have 7 holes and only one of those is 6" the others are 4". The drill broke on one of the shorter hole, so I thought I better look for some advise.

 

Thanks.

[?Mark]

For .500 hs-co drill try S306, F1.2 and Q.075.

Should work well especially if pre-drilled with shorter drill (use the same parameters but increase Q to .125)

 

hth

[mold100]

It will only work harden if 1 to much heat is generated and 2 if your pushing instead of cutting, if your tolerance doesnt require a reamer dont do it, there is a happy medium between babying it (most likely to work harden) and being to agressive (thus eating your tooling and profit margin) I agree completely from exp with Mark I would step it down a knothch as you go deeper with less peck depth. 6 inches is deep but not out of the ordinary for a 1/2 in drill, you just havent done it much. +1 to starting with a stub, or even standard drill, peck this at .1 to .125 at 350 to 400 rpms and 2. in per min, then I would take your airraft drill and whack some of that shank off if you cant get a taper length drill with 6 in flute. same rpms and feed mabe cut it back to 1.5 ipms, but i would reduce peck to maybe .075. If you buy a new drill try a 135 degree tip vs. the standard 118 also IMO.

[heavychevy2155]

On deep holes like that, I have posted it out longhand and manually add dwells every .5 inch or so. The deeper in the hole the longer the dwell to allow coolant into the hole to help cool the part and flush chips out.

[MACHINEMASTERG]

a dwell in the hole while in contact with the material will cause work harding

[?Mark]

ss material + dwell + drill = bad idea

[Kevangel]

Some aircraft drills have a short flute length and anytime a drill enters a hole and goes deeper than the lenght of flute I use extra care it does not catch a chip between hole and "solid" dia. I am doing some 420SS pre-hard right now and agree with 300RPM for .5 hole to stop work hardening..

[chris m]

I think he's talking about dwelling at the retract height, which would be fine

[Clarence]

I hadn't gotten to the end of the flute, so I know that wasn't the problem. I have caught a chip between the material and the solid part of the shank before and it go exciting real quick. I will attempt to never let it happen again.

 

Using the information that everyone kindly provided, I ran an experiment on the other hole location and it worked great.

 

Thanks to everyone that has help. I have been lurking on the forum for several years now, and it has helped in many ways.

 

Thanks again.

 

PS I know not to ask for post processors.

[GoetzInd]

We've had good luck with Indexable spade drills even that small. Good finish and really tough. Not too expensive either. Like others have said, the 135 split isn't optimal for 304 because it grabs and that split point is really fragile. I thing point geometry is going to make a big difference in this one.

 

Mike

[bhyde]

Has anyone actually tried dubbing the drill? By dubbing I mean putting a small flat on the cutting edges. I did this years ago, when I ran a fair amount of 304ss and it seemed to work pretty good. The drills seemed to last longer. I don't think I would do this at 6in deep though.

[heavychevy2155]

Yes, I was talking about a dwell at the retract. Dwelling in the hole would be bad for sure.

[Lvs2Dv]

Try starting out at 48-50 SFM, feeding at about .0037 IPR, for the first 3 diameters deep.and pecking 1/3 of the drill diameter.

Reduce the speed and peck amount 10% and the feedrate 5% for the next 2 to 3 diameters. (IPR feedrate, IPM calculated from reduced RPM and IPR.)

Do this every 2 to 3 diameters of depth, using the values attained from each reduction calculation, until feedrate has been reduced 30%, (to about .0026 IPR, in this instance), and peck amount has reduced to between 15% 20% of the tool diameter

Continue reducing the speed until you have reached 1/2 the SFM you began with, and continue to the bottom at 50% of original tool velocity, 70% of original advance per revolution, pecking about 1/5 tool diameter.

I am assuming 135 degree splitpoint geometry and a good quality cobalt drill, with polished flutes or a TiN coating, to reduce friction and aid in evacuation of hot chips and swarf from the cutting zone.

This sounds like a lot of trouble, but using this approach has worked reliably for me in 300 series SST, since way back when it was me, my TI59 calculator, when that model was "latest and greatest".

Cutting the code consisted of transfering pages of hand written G code to machine ready media by hammering away on a Flexowriter, as it clattered back punching a row of holes the tape each keystroke.

Ah, the stories I could tell. Of paper tape power winders, and paper cuts of epic proportion.

Alas, that is for another time ........

 

Hope you try this. Me thinks you will be pleased.

 

PS: Why not start slow, and do the hole with one cycle call? Calc the time difference for, say, 300 holes, 15 diameters deep, on a job that runs 4 times a year. Now, THAT'S a good number of beer runs paid for!

 

With TiAlN coating, starting data could be up to 65 SFM, with maybe a 10-15% increase in IPR, with data reduction every 3 to 3.5 diameters.

This sounds like a lot of trouble, but has worked for me, back when it was me with hair, my Flexowriter, and a TI59 calculator, when that model was "latest and greatest". (Still have it, still works after 30 years, even the thermal printer)

 

Past my bedtime, the twelve pack is gone, and I had to type twelve 3 times to get it right. Good night.

[chris m]

NICE handle...

[mtnflyr]

+1 to bhyde on dubbing.

I do this on all stainless drilling using cobalt drills with 135 degree split point. Also helpful is spotting the hole with a Body drill. Precision Twist Drill makes these. They are a 135 degree split point drill with only 1/2" LOC. Since the point of the starter drill matches the point of the drill it locates better and keeps the corners from prematurely wearing or breaking off the drill.