[Shop junkie]

I'm having a problem with a very simple dill and tap operation. I feel like a dork, but I haven't done and drilling and tapping in stainless since I got this machine so I'm kind of in the dark. So far I've broke a center drill and rounded off a drill. So if someone could take a look at my program and tell me what I'm doing wrong I would appreciate it.

Oh and my mill is a HAAS TM1

%
O7809 (shift plate for guys next door.)
T1 M06 D01 (#2 CEN DRILL)
G00 G54 G90 X-1.0 Y1.0
S1200 M03
G43 H01
X.375 Y-.250 Z.1
M08
G83 Z-.250 Q.020 R.1 F5.0
X1.0
X1.625
M09
G80 G00 Z1.0

T2 M06 (.242 DRILL)
S1000 M03
G00 G54 G90 X.375 Y-.250
G43 H2
Z.1
M08
G83 Z-1.100 Q.025 R0.1 F5.0
X1.0
X1.625
M09
G80 G00 Z1.0

T3 M06 (G DRILL FOR 5/16-18)
S1000 M03
G00 G54 G90 X.375 Y-.250
G43 H3
Z.1
M08
G81 Z-1.050 R.1 F8.0
X1.0
X1.625
M09
G80 G00 Z1.0

T4 M06 (5/16-18 TAP)
G00 G54 G90 X.375 Y-.250
S288
G43 H4 Z.1
G84 G98 Z-.500 R.100 F16.0
X1.0
X1.625
G80 G00 Z1.0
G00 X.375
G84 G98 Z-.850 R.100 F16.0
X1.0
X1.625
G80 G00 Z1.0


T5 M06 (.500 c-sink)
G00 G54 G90 X.375 Y-.250
S1400 M03
G43 H5
Z.1
M08
G81 Z-.210 R.1 F20.0
X1.0
X1.625
M09
G80 G00 Z1.0

T1 M06
M05
M30
%

( .500 thick 2.0 wide 304 stainless, XY0 left upper corner)

[AMCTony]

I would cut the RPM on all drilling down about 50% and take much larger pecks. If possible do not peck with 304. T1 = no peck, T2 = 0.250 peck. Pecking and dwelling in 304 is a sure fire way to ruin tools. Peck little or not at all if possible. Flood coolant!!!!

[behindpropeller]

How come you are not countersinking before tapping?

[Shop junkie]

I mostly work in plastics so with plastic I don't. Should I with stainless?

[billystein]

Hi,
I have had the best luck drilling 304 by holding the sfm at 48.

#2 c'drill rpm looks ok I would probably start at 1000 rpm feed 1 ipm
use g83. use good quality c'drill

.242 drill rpm = 757 feedrate start at 1 ipm maybe you can go 1.5 or 2
peck .03 - .04

.261 drill rpm = 702 feed start 1-2 ipm peck = .1
I know guys that can drill faster but I have found that the tools will actually last a while keeping close to these parameters
use the best cobalt drills you can find use proper coolant mix.
if you want to try to speed up job then increase feed instead of trying to increase rpm.
good luck

[Shop junkie]

Thanks for the help guys.

I'm not to worried about how long it takes, I just need to get the parts done with out killing my tools. I would have ordered some nice tools for the job but it's a last minute deal I took to help some guys out. So, nom I'm under the gun using a HSS c-drill and non coated drills. (nuts)

So, I need all the help I can get.

[billystein]

c'drill should be ok.
decrease rpm about 20 % to start. the feeds should be ok
just keep the chips coming and dont let the drills turn red and you should be fine. Also please show anyone how we do this or we will have to kill them.

billy

[Shop junkie]

Well with the hepl from you guys I got 1 good part so far. Here's what the porgram looks like now. What'cha think.

%
O7809 (shift plate for guys next door.)
T1 M06 D01 (#2 CEN DRILL)
G00 G54 G90 X-1.0 Y1.0
S400 M03
G43 H01
X.375 Y-.250 Z.1
M08
G81 Z-.250 R.1 F2.0
X1.0
X1.625
M09
G80 G00 Z1.0

T2 M06 (.242 DRILL)
S400M03
G00 G54 G90 X.375 Y-.250
G43 H2
Z.250
M08
G83 Z-1.100 Q.250 R0.250 F2.0
X1.0
X1.625
M09
G80 G00 Z1.0

T3 M06 (G DRILL FOR 5/16-18)
S400 M03
G00 G54 G90 X.375 Y-.250
G43 H3
Z.225
M08
G81 Z-1.050 R.225 F2.5
X1.0
X1.625
M09
G80 G00 Z1.0

T4 M06 (5/16-18 TAP)
G00 G54 G90 X.375 Y-.250
S288
G43 H4 Z.1
G84 G98 Z-.500 R.100 F16.0
M00
X1.0
M00
X1.625
M00
G80 G00 Z.1
G00 X.375
G84 G98 Z-.700 R.100 F16.0
M00
X1.0
M00
X1.625
M00
G80 G00 Z.1
G00 X.375
G84 G98 Z-.850 R.100 F16.0
M00
X1.0
M00
X1.625
M00
G80 G00 Z1.0

T5 M06 (.500 c-sink)
G00 G54 G90 X.375 Y-.250
S1400 M03
G43 H5
Z.1
M08
G81 Z-.180 R.1 F20.0
X1.0
X1.625
M09
G80 G00 Z1.0

T1 M06
M05
M30
%

( .500 thick 2.0 wide 304 stainless, XY0 left upper corner)

[davereagan]

Why center drill, drill .242 and then drill .261? Drill right to .261 Real oil on the tap and the new speeds are much better.

[Shop junkie]

I center dill out of habbit mostly and not wanting the holes to be off. As far as the other I don't think I have the HP to pull a .262 in SS, 1" dp, it's only a TM1.

[beege]

Sure you do! If you can't cut 1/2" I'd be very surprised/disappointed.

[Shop junkie]

Really..?:devious:I guess I've just been a puss...

[davereagan]

That makes no sense. You are pushing a .242" drill just fine right? The difference between .242 and .261 is 8%. Do you have a split point .242 and only a chisel point old style .261"?

[little bubba]

I see a lot of things wrong, and these are from my mistakes.

First, you're driving a #2 center drill .250 deep at .004" per rev, no pecks. Thats a .078 drill point going over 3X deep, no pecks at a HUGE feed for such a small drill. Then on the revision you are up to .005 per rev. Far too much, your original RMP and a 2ipm feed should work ok.

Second, you are using a center drill, and a little one at that, and driving it half way through the part. Center drills are for putting in centers to use on a lathe. What you are doing is spotting, use a spot drill, or the very tip of a bigger center drill. Since its a quicky job and you may not have the tools, take that little #2 and just stick her in about .030 or .040, not .250, you need a spot, not the grand canyon.

Third, as has already been said and corrected, pecking a lot DOES NOT make things better. The part is only .5 thick, one shot and done. On the same note, going from a .242 to a .261 drill isn't helping you at all. Drills get really pissy going down a hole that is close to their own size. They jump, chatter, chip, run oversize and do all kinds of nasty stuff. General rule, don't stuff a drill down a hole that is more than 1/3rd the size of the drill. I also think you are banging the feed a little hard, though I'm not an aggressive driller. .0025 to .003 for something in the .250 drill size, I would consider that the transition from ***** footing to aggressive. You have enough chip, but not too much.

A few more thoughts, if the part is only .5" thick, why are you drilling over an inch deep? Also, already been said, why do you think you can't drive a G drill? But can drive a C drill?

304 is a big jump from plastic(It's not harder to work with, just different), ease the feed(per rev) back a bit, skip the C drill, smaller spot or a better tool and you should be fine.

[Shop junkie]

Sweet thanks for the advice.

I made a mistake it's a #3 c-drill. But I'm pickin' up what your putting down. Next time I'll try a spot drill. I agree .250 might have been a bit much and I think it caused the early retirement of the .242 drill. So next time I'll use a spot drill and just pound the .261 in after, correct?

The part is .500 thick X 2.0'' wide X 2.750 long and I'm drilling and tapping with the part standing on end going into the 2.750, 1.100dp.

Sorry guys still fairly new with this machine not sure what the capabilities are, Ill take any help I can get. Everything you said so far has made sense and worked really well. I appreciate it.

[davereagan]

No spot drill. .261" Screw machine length drill can drill 1.1" and does not walk like a jobber drill. I'd go 400 rpm with cobalt split point drill, flood coolant with preferably soluble oil not synthetic, .004" fpt or 1.6 inches per minute and you'll be done without worn out tools. Need high vanadium tin or ticn coated spiral flute tap and tapmagic or other straight oil for long tap life. I would consider .266" drill to make tapping easier. Tap depths: .300", .500", .700" McMaster.com has nice selection of drills and taps.

[Shop junkie]

Awesome, I'll give it a try.

So peck or no peck on the drill?

[tnik]

for .5 deep, unless you have problems with the chips not breaking or not releasing from the drill, I wouldn't peck.

I tend to use a 35/40 SFM on stainless, and on small drills I go about 1 - 2% of the diameter for the chipload per tooth.

Worst thing with working in stainless is work hardening the material or the tool. Make sure to use plenty of coolant.

Also, why are you pecking the tap? I would just use some oil and drive it through. I usually run all taps at 100 rpm and oil by hand. unless its a huge production job then I purchase the more expensive coated taps and use coolant.

And I saw a couple other people say it, but you want to countersink the hole BEFORE tapping. Taps love a nice clean hole to enter, and having the countersink there before tapping will help the tap keep its life, not chip up, and give you a nice lead in thread.

[BigC]

I realize I'm commenting on an old post, but here is my 2 cents. You've had some good recommendations. Lots of coolant for sure. If you do get the 304 too hot from excessive speed you will work harden the material and NO slowing down will fix that part. You will not be able to go bigger or deeper or cut threads with HSS tooling.