Drilling 18-8 bolts

I have this job drilling 1/4" SHCS 18-8 x 3/4" length with a 9/64 hole. My present operation uses cobal 135 split point, 1200 rpm and 2 ipm feed, pecking at 0.075" mostly

G98 G83 X? Y? Z0.8041 R0.1124 I0.24 J0.075 K0.08 P0 F1.956 to be exact.

I am prepping the bottom of the hex with a .125 endmill to make it flat, otherwise the drill wanders too much. The main issues are #1 speed, and #2, rats nests. I have a jig that holds 120 pieces, so I almost have to keep an eye on the whole process. Also, I basically need to change the bit after 120 pieces.

I have done some experimenting with carbide drills, and my experience is that it rats nests a little, and after about 15 holes it snaps, pretty much at the different feeds and speeds I tried.

My machine is a VF2, without through hole coolant. Any ideas on a better process?

I drilled several hundred steel grade 8.8 bolts and found the thread rolling and head forging made for a huge variation in toughness along the depth. I would guess 18-8 will be similar. Your drill diameter puts the cut right in the work hardened region of the threads too.

I had better results using cobalt for longevity, carbide worked great for several holes then one catch on a hard spot and it snapped. Maybe try a carbide spade drill to start the hole down to 2-3x diameter depth then change to a cobalt twist drill.

spade here:
https://www.mscdirect.com/product/details/83245803

I also used some heavy tapping oil on top of the head. It was a lot of babysitting unfortunately.

18-8. Basically 304. But shittier (more shitty?) since its been cold worked.

I've found the biggest problem I have in work hardening materials when drilling, is the
retract. The very beginning of the retract.

I hand code my drill cycle and then run it as a sub. Feed in, then feed out a bit,
then either fast feed or rapid out.. Then back in, but above where you stopped cutting,
and then start going again. You can also come WAY out of the hole to give the coolant
a better shot of getting down into the bottom of the hole, and also give you a
greater chance at getting rid of your birds nest.

The reason I do this is because 304 work hardens. The chip is fricken hard, and its pretty
easy to rip the cutting edges off of the drill on a retract. Even if you have a cycle that
has a dwell before retract.. YOU ARE DWELLING ON 304!!!! in other words RUBBING. You really shouldn't
do that.

Also if you take the 5 or 10 minutes to hand code, you could add in some chip breaks in between
your pecks to attempt to eliminate your birds nest problem. Feed out .010 or so and then keep
going down.

Just my 2 cents.

Edit: One way to check if your problem is with the rapid retract without having to reprogram. Turn your
rapids way down and see what happens. When I only have a few quick holes to do, instead of wasting
time coding, I'll just run it with the rapids in the basement.

With 18-8 aka pretty much 304 I have the best luck using Titanium-Nitride (TiN) Coated Cobalt Steel drills. Carbide is great but they are pricey and any shock, like change in material condition or a little runout or misalignment and they break without warning.

Ditch the 1/8" endmill. Use a stout carbide 9/64" drill (meant for SS, not fiberglass), around 3Krpm and 7ipm for ~.1" Dp to establish hole location. Tune the feed to get where the chips fling off the flutes on retract, you can add depth if you find a stable area that gives adequate tool life. G81 or coded G1 to control retract.

Follow up with the cobalt drill at ~2200rpm and 5ipm, feed to just above hole bottom and start a G1 peck sub as Bobw suggests, but with a fairly short cut (start at .03"), and tune S/F to get chips that don't nest. This may require going in fairly hot, but always feeding above the last floor to avoid ramming in, pulling back to cleanly end the current chip (so not pulling the edges off the drill).

If nothing helps eliminate bird nests, you can set up a stripper plate (think like a slot or the "V" of a thread gage, as a diving board off a 1-2-3 block - bring the drill into the notch near the collet, feed up to strip off the nest. Reverse spindle if you must.

Work on your fixture plate array from the furthest points from coolant towards the coolant side (presumably left to right). This helps direct chips away from the "not yet drilled" heads and lessens chips falling into the screw heads before the drill gets there.

Smaller, heavier chips will be worse if they do fall into the heads before the drill gets there (or between the carbide and the cobalt), so you might decide the a nest that you can strip off winds up being better, but that's dependent on how aggressive your coolant spray is and the spacing of the bolt array on the fixture. I'd rather have a little more space for the bolts and give plenty of room for the chips to fall in between the heads.

Hope this is of some use...

friesen said:

I have this job drilling 1/4" SHCS 18-8 x 3/4" length with a 9/64 hole. My present operation uses cobal 135 split point, 1200 rpm and 2 ipm feed, pecking at 0.075" mostly

Click to expand...

You're running 45ish SFM and .0008" per cutting edge, per rev in 18-8!!! I'd be running .002" per side, per rev.

Birds nests occur when you're chip isn't heavy enough to break off. So you've got to make them break.

I have NEVER had good results using solid carbide Drills in 18-8 (304). Good ole black oxide HSS.

If you have a lot of holes to do something like a coolant inducer begins to make a lot of sense.
Quite a few companies make them, but they are all probably fairly expensive.
New Baby Collet Type | BIG KAISER

The only magic bullet is thru spindle coolant, which an inducer provides.
9/64th is a small drill, but with TSC you should have much more success.

Another trick with peck drilling is to retract and reverse the spindle which can help to fling off the chips, then advance again.
Stringy Chips Wrapped Around Your Tools? Mark Has a Solution! – Haas Automation Tip of the Day - YouTube This video explains the topic well.

Rob is right, you need to feed hard enough to force the chips to break.

I think I'm going to try some of the suggestions here, especially hand coding exit and entry. I do wonder what value coatings could be, something like this ? 9/64 - .1406" Cobalt 130deg Screw Machine Length Drill TiAlN Coated MariTool

I think that a TiAln coating is more appropriate when cutting dry, and for 18-8 I'd rather have coolant. I'd stick with quality uncoated cobalt, perhaps a more exotic version from a Titex/Guhring/Nachi with a more free cutting tip than a simple split-point.

This cobalt drill welded the tip at about 0.300 depth on the first bolt - 9/64 - .1406" Cobalt 130deg Jobber Length Drill Bright Finish MariTool

3.9 IPM at 1950RPM

friesen said:

I have this job drilling 1/4" SHCS 18-8 x 3/4" length with a 9/64 hole. My present operation uses cobal 135 split point, 1200 rpm and 2 ipm feed, pecking at 0.075" mostly

G98 G83 X? Y? Z0.8041 R0.1124 I0.24 J0.075 K0.08 P0 F1.956 to be exact.

I am prepping the bottom of the hex with a .125 endmill to make it flat, otherwise the drill wanders too much. The main issues are #1 speed, and #2, rats nests. I have a jig that holds 120 pieces, so I almost have to keep an eye on the whole process. Also, I basically need to change the bit after 120 pieces.

I have done some experimenting with carbide drills, and my experience is that it rats nests a little, and after about 15 holes it snaps, pretty much at the different feeds and speeds I tried.

My machine is a VF2, without through hole coolant. Any ideas on a better process?

Click to expand...

It might help to start with a drilled screw... McMaster-Carr

friesen said:

This cobalt drill welded the tip at about 0.300 depth on the first bolt - 9/64 - .1406" Cobalt 130deg Jobber Length Drill Bright Finish MariTool

3.9 IPM at 1950RPM

Click to expand...

Okay, I think your feeds and speeds are right on. So that's a good start. I don't know what value #10 is or what it's conditions are. But some of your macro looks weird to me. Not saying it's wrong, just looks funny. #10_#3 and #6+#3 not sure why that's sequenced like that.

You should drill into the material, feed away from the cut, come out of hole however you want, go back in just shy of where the last cut was, then feed in more. BUT you're feeding too deep for a .14" Drill. Id back #4 off to .075". jmo.

R

#6 is z depth, #10 tracks this peck total depth.

I said you're feeding too deep in post 12. I meant your peck amout is too high. 2000 for a 1400 Drill is asking a lot in any steel. Anything over the diameter of the Drill is tricky. 304 needs nice easy chips, especially when making holes.

R

I tried .050 of .100 peck, with about the same results. One mistake I think it needs to pull back at a higher rate.

Ultimately I think the material is too hard or something for 70sfm.

friesen said:

I tried .050 of .100 peck, with about the same results. One mistake I think it needs to pull back at a higher rate.

Ultimately I think the material is too hard or something for 70sfm.

Click to expand...

It's possible. Without a hardness tester you'll just guessing. But I would not change the chipload, regardless of spindle speed.

Is it screeching at you when you get into the hole? Or does it sound like it's breaking chips off like a chisel? Or is it just great except the melty part?

R

If there's nothing wrong with the program, I would suggest looking into a more specialized drill point hike a helical/"S" type, as shown near the bottom of this page: Which Drill Point Angle Should I be Using? | Regal Cutting Tools

I'd stay with cobalt for the material. I like/use split points for most materials, but in some (like gummy stainless) I'd prefer something a little more free flowing. The split acts as a plow, and soft stainless can "pack up" rather that smoothly flowing up the drill. The S point is less likely to have that happen.

id cut the spindle speed down to 800 rpms same feed rate maybe slower then work it up. start at .05-.070 pecks.
the break out on the back side has a tendency to ruin drills so slower rpms is better.
we used to do tons(thousands) of button heads with a .125 hole through. the break out was usually the issue, I center drilled them 1st using a #2 center drill but only just about .025 deep and used stub cobalt screw machine 135º split points. if your center drill is too deep you will burr the edges of the drill hence why I only touched it.

also check the break through and see what color it is, if its blueish your rpm is way to fast, once you get it silver your good.
We used to do them on the mill, but since I had a wife with nothing to do and the lathe was in the next bay it was a win win

I'd be drilling these from the other side. Rework your jig so that it mounts upside down. Drilling in the hex without through coolant and with lots of pecks means that the hex pocket is going to retain a lot of chips that will get dragged back into the hole. This is probably happening on a scale that is difficult to see, and taking out the corners on the drill.

Use a spot drill instead of the endmill.

The problem with backside drilling is that natural progression is out of the jig rather than in.

Attached is a photo of a 1200rpm x 2.5 ipr hss 135 split point cheapy michigan drill.