Metric rigid tapping, TM 1

[Shop junkie]

Sorry for the noobie question but I'll throw it out anyway. I've got a TM 1, and I'm going to rigid tap for the first time. I would like to to make sure I did the code right so i don't stuff it and make alot more work for my self.

I'm using an OSG roll tap m3x.5 6h. The material is 18-8 .250 thick. To get my feed rate i Divided .5 by 25.4=.019685 x 1000 rpms (random rpm I chose) to get 19.68F

N2G00 G54 G90 T3 M6 (#35 DRILL)
X.620 Y-.1251 S2000 M03
G43 H03 Z.250 M08
G83 G98 Z-.350 R.050 F20.0 Q.050
M09
G80 G00 Z1.0


N3 G00 G54 G90 T4 M06 (M3X.5 ROLL TAP)
X.620 Y-.1251 S1000 M03
G43 H04 Z.250
G84 G98 Z-.275 R.250 F19.68
G80 G00 Z1.0

[extanker59]

Looks OK to me but I've never tapped 18-8, just 300-400 series. Seems like a really high feed for the drill. You don't need to put the M3 S1000 where you usually put it. It should go on the same line as the G84. The controller will just stop it and restart it when it gets to the G84. Saves a tiny bit of time. Doesn't hurt to have it up there though.
Don't forget the long lead of the tap so you'll have to go a lot deeper. And make that GOO a G00 (OK, I knew you knew that).
If the threads aren't formed enough, you may have to increase your RPM (and matching feed rate) to get it to flow properly.
Are you manually putting tapping fluid on or are you missing the M8?

I don't see anything else but I miss things all the time.
Good luck and tell us how it worked.

[Shop junkie]

Yea, I've already caught and fixed the GOO, I hadn't had my coffee yet when I did the program.

I put the speed there just caause that's how I've done it in the past, (with other tools) But I've never used a G84, thanks for the tip. I didn't know if I needed to have the spindle moving before it got to the part or not.

18-8 is just any 300 series stainless, atleast from what I know.

I didn't put an M8 in because I'm going to use some moly-d by hand. If it looks like it's going to work well I might add the M8 later and let it run.

[Geof]

On Haas you do not need to start the spindle, just set the rpm, but I always start it at 1000 rpm in the same manner as for any other tool. Although for such a fine pitch doubling the speed is probably okay.

18-8 stainless is 304.

[Shop junkie]

On Haas you do not need to start the spindle, just set the rpm, but I always start it at 1000 rpm in the same manner as for any other tool. Although for such a fine pitch doubling the speed is probably okay.

18-8 stainless is 304.

Doubling the speed?

Is the way I came up with the feed rate correct? Is it to fast or slow? I just pulled the rpm out of my booty crack.

If 18-8 is 304 why wouldn't (the dowel pins I'm modifying for example) the say 304 on the box? I can get the same pins in 304. Just curious.

[extanker59]

Thanks. I didn't know that 18-8 was 304. I wonder why the different nomenclature? I'd forgotten about the M3. I always put it in (obviously for no reason).

[Geof]

I stole this from someplace;

18-8: 300 series stainless steel having approximately (not exactly) 18% chromium and 8% nickel. The term "18-8" is used interchangeably to characterize fittings made of 302, 302HQ, 303, 304, 305, 384, XM7, and other variables of these grades with close chemical compositions. There is little overall difference in corrosion resistance among the "18-8" types, but slight differences in chemical composition do make certain grades more resistant than others do against particular chemicals or atmospheres. "18-8" has superior corrosion resistance to 400 series stainless, is generally nonmagnetic, and is hardenable only by cold working.

304: The basic alloy. Type 304 (18-8) is an austenitic steel possessing a minimum of 18% chromium and 8% nickel, combined with a maximum of 0.08% carbon. It is a nonmagnetic steel which cannot be hardened by heat treatment, but instead. must be cold worked to obtain higher tensile strengths.



Doubling the speed? Sorry I should have been more explicit; double the rpm to 2000 and double your feed to F39.36

Your calculation for the feed is correct; I always use 1000 rpm for my tapping because it is easy to calculate the feed from the pitch exactly as you did.

[Shop junkie]

Thanks for the info on the 18-8.

Well so far everything is looking good. I've ran the program dry a couple of times. Looks like it should work. Now I'm just waiting for my taps to arive. They should be here tomorrow am. So I'll let ya know.

OSG recomends 15-40 ipm for that tap, so that fits in their scope but can I really run it at double with the TM1. Or am I asking for trouble?




Thanks for the help

[extanker59]

I always look at the manufacturer's recommendations too. I usually start in the middle of their range and go from there. I suggested a higher rpm because of past experience (but with different SS and probably a different tap). I like your approach. Just, after running it, if the threads aren't fully formed, try increasing the rpm. Slowing it down might help some tapping situations but not usually with a form tap.
Geof- Thanks, I'll look into that G31. I always start high, like I said, to be safe, but I like the protected move method much better.

[extanker59]

Sorry Geof. That last comment probably had you scratching your head since you said nothing about G31. That G31 comment was for Al the Man on a different thread. I get confused easily, apparently.

[Shop junkie]

Thanks for the help guys. So far so good. I got my taps in this morning, set my z and gave it a shot. So far the parts are beautiful. But I've only run 3 (had to do a first artical through Q.A. before I start the run)

So really qurious to see how many parts I'll get on this tap. I'll let ya know.

Here's the program do you see any really stupid mistakes I should correct?
I've done alot of conversational CNC mill work over the last 10 yrs, not much G-code at all since college. So any advice, help or criticism is appreciated.


%
o0019(7716-01)
N1
T2 M06 (CEN-DRILL)
G00 G54 G90 X0.0 Y0.0
S2000 M03
G43 H02
G00 X-.620 Y-.1251
G00 Z.050
M08
G82 G98 Z-.050 R.05 F10.0
M09
N2
G00 G54 G90 T3 M6 (#35 DRILL)
G00 X-.620 Y-.1251 S1500 M03
G43 H03 Z.250 M08
G83 G98 Z-.550 R.050 F3.0 Q.035
M09
N3
G00 G54 G90 T4 M06 (M3X.5 ROLL TAP)
G00 X-.620 Y-.1251 S1000
G43 H04 Z.250
G84 G98 Z-.350 R.250 F19.68
N4
G00 G54 G90 T5 M06 (90* C-SINK)
G00 X-.620 Y-.1251 S1500 M03
G43 H05 Z.250 M08
G82 Z-.070 P.6 R0.1 F10.0
M09
M05
N5
T2 M6
M30
%

[extanker59]

If it works then there are no stupid mistakes. Nice work. EVERYBODY does it a little different from each other. My take on it is: stay consistant. You don't have to copy somebody else. Just make it work (like you did). Then shoot for better parts and shorter cycle times. That includes programming time. That's where consistancy helps. Standardized programs are easier to remember and so quicker to write (you can cut and paste easier too, if it's always done the same way). Here's my slightly different way:


%
o0019(7716-01)
G00 G17 G20 G40 G49 G90 G94 G98 (safety block-mostly unneeded but...)

N2 (N# matches tool # to make tools easier to find in long programs)
T2 M06 (***90 DEG SPOT DRILL***)(one tool to spot and chamfer)
G00 G54 G90 X-.62 Y-.1251 S2000 M03
G43 H02 Z1. M8 (easier to stop if it's going to the wrong z level if at Z1.)
G82 G98 Z-.07 R.05 P.1 F3.
G80 M09 (I always cancel drill cycles)

(spaces to easier see tool changes)
N3
T3 M6 (***#35 DRILL***)
G00 G54 G90 X-.620 Y-.1251 S1500 M03
G43 H03 Z1. M08
G83 G98 Z-.550 R.050 F3.0 Q.035
G80 M09


N4
T4 M06 (***M3X.5 ROLL TAP***)
G00 G54 G90 X-.620 Y-.1251
M0 (program stop to apply tapping fluid-I forgot that you're doing that)
G43 H04 Z1.
G84 G98 Z-.350 R.250 F19.68 S1000
G80 M09
M05

T2 M6
M30
%

I do a few other things too, like:
G53 Y0 Z0
M1
after every tool to make it easier to set up.
etc...
Everybody is different. Again, nice work.
Chris