[Vern Smith]

Made my first attempt today to use rigid tapping on my new Haas TM-1P. Didn’t have much success. I drilled the holes .7 deep with a #24 drill in 6061 T6 which I thought would make life easy for the tap. I left .3 under the tap for chip accumulation. Used a spiral flute tap, brand new. The tap seemed to go down fine but snapped off as soon as the spindle reversed. All .4 of the tap is still in the first hole. The spindle came up at twice the RPM that it went down at. I’m sure there is a setting somewhere to change this. I used the default setting. I used my CAM program to write the code. I chose the G84 machine cycle and G98. These were the only options offered. Hopefully someone can tell me what I screwed up.

O0011(PART - TAP TEST)
N1 (NOTES - NONE)
N2 T6 M06 (#10-24 NC TAP)
N3 G90 G80 G40 G54
N4 S448 M03
N5 G43 H6
N6 / M08
N7 G00 X0.5 Y1. Z0.2
N8 G98 G84 Z-0.4 R0.2 F18.6668
N9 X1.
N10 X1.5
N11 G80
N12 G00 Z0.2
N13 M01
N14 M30

Vern

[Gandalf]

Hi Vern

You did nothing wrong in the programming of your part. The Haas tapping cycle always comes out faster then then it goes in, unless you change that parameter. I suspect that you are using coolant for tapping. I found in past situations that a rich mix or tapping fluid works better.

[Geof]

Did you check that both the correct SETTING and the correct PARAMETER are turned on?

There is a SETTING or PARAMETER to change the retract speed, I forget which it is. However, whatever it is set at you can override it with a J command in the G84 line. I think it is J, read the manual and you will see it mentioned. Use J1 to come out as fast as you went in.

[WITOMCIO]

In settings ,parameter 130 shold be set to 1.
Also see if you have parameter 131 repeat tapping on.
My gut felling tells me thou that your rigid tapping option my not be on.
Check your parameters ,if they are OK , call Haas to make sure you have rigid taping enabled.
Nothing wrong with program, looks good.

[Vern Smith]

Thanks Fellows, I'll check the settings and parameters in the morning. I paid for rigid tapping and the installer called Haas for a code when he set up the machine. I'll check with Haas to be sure the code is correct before I sacrifice any more taps.

I hate to think that coolant (Hangerstfers S500) verses tapping fluid would be the difference between smooth sailing and diaster with a brand new tap going two times it's diameter deep into an oversized hole.

Vern

[Geof]

I actually read your post a bit closer, you are going 0.4" deep that had not clicked in my mind.

In my experience in 6061 0.40" is too deep in one go. You need to ensure your Rigid Tapping is correctly turned on with REPEAT RIGID TAPPING and then go in 0.25 first pass and 0.4 final.

Your coolant should be fine, we use a water mix coolant (Shell Dromus B) at around 1 in 10 to 1 in 15 dilution and do a lot of tapping in 6061.

Also I have found going faster seems to work better many times. I nearly always use 1000rpm which makes the feed calculation easier anyway.

[100]

I would use a form/roll tap in aluminum. You have to drill the hole quite a bit larger with a form tap but you get a stronger thread and the tap has no flutes or chips so it will be hard to break in aluminum. I have not had great luck with deep holes and small spiral taps.

[big_mak]

I have my CAM post set up to post

G95(Feed Per Rev)
G98G84 X####Y$$$$$ F(TAP PITCH) R****
G94(Feed Units PEr MInute)

This way when you change the RPM at the COntrol, you don't have to recalculate Feed.

Vern, u have OneCNC?

[miljnor]

when your talking anything below 1/4-20 taps the tap itself is one of the biggest factors.

what tap are you using?

probably the biggest factor is drill size (and you should be fine with a #24) Since most taps deform the aluminum you can actually go to a #23 or 5/32 then check with a go no/go gauge they will probably still give you good numbers.

You just have to be sure you QC the thread properly if you use oversize drills to make sure it gets deformed into spec.

I typically use ex-o taps (I think OSG makes them), they aren't cheap but the are the real deal. Emuge makes really nice stuff, but, I haven't used it much since Ive been doing 90% aluminum these days.

you can peck drill if you want, but, I tap 10-32 to .75" in one shot all day long.

[Vern Smith]

I used a Union Butterfield tap, H3 tolerance. The post comes from OneCNC. How does one go about using the repeat rigid tapping feature? Do you run subsequent G84 operations into the same hole with increasing lengths of depth? Will the spindle orient itself to the same position for repeat plunges? I can't find any options for re-tapping or peck tapping in the OneCNC G84 tapping operation.

Please keep the conversation coming, I'm leaving town at 10 AM EDT and will be back Sunday afternoon.

Vern

[Vern Smith]

Quick thought, my spindle clearly went to the bottom of the hole and reversed rotation. Would this happen if rigid tapping was not turned on? I checked the settings, 130 tapping retract was set to 2 which explains the 400 RPM plus in and 800 RPM plus out. 133 re-rapid tap was set to on, 57 exact stop canned is off. I guess I have to learn how to program multiple tap operations in the same hole.

Vern

[KEP]

Settings from The Manual:

130 Tap Retract Speed ( Set to 1, usually 4 from factory)
This setting affects the retract speed during a tapping cycle. Entering a value, such as 2, will command the mill to
retract the tap twice as fast as it went in. If the value is 3, it will retract three times as fast. A value of 0 or 1 will have
no affect on the retract speed. (Range 0-4)
Entering a value of 2, is the equivalent of using a J code of 2 for G84 (Tapping canned cycle). However, specifying a J
code for a rigid tap will override setting 130.
Note: If the machine does not have the Rigid Tap option, this setting has no effect.

133 Repeat Rigid Tap
This setting ensures that the spindle is oriented during tapping so that the threads will line up when a second
tapping pass, in the same hole, is programmed.

Also in parameter 57 there is a bit for Rigid Tapping - it should be a 1 if it's turned on.

[HuFlungDung]

I used a Union Butterfield tap, H3 tolerance. The post comes from OneCNC. How does one go about using the repeat rigid tapping feature? Do you run subsequent G84 operations into the same hole with increasing lengths of depth? Will the spindle orient itself to the same position for repeat plunges? I can't find any options for re-tapping or peck tapping in the OneCNC G84 tapping operation.

Please keep the conversation coming, I'm leaving town at 10 AM EDT and will be back Sunday afternoon.

Vern

Yes, a special canned cycle is required in OneCNC. Basically all it does is what you suspected: repeats the tapping operation at other depths. You can find some Haas posts on the OneCNC forum that have such cycles ready made. You can also contact me for a copy of my Haas post if you like.

[Geof]

.... Will the spindle orient itself to the same position for repeat plunges?...

I think you can cancel the G84, go off and do something else and come back with another G84 with the same start Z and everything orients correctly.

[miljnor]

I think you can cancel the G84, go off and do something else and come back with another G84 with the same start Z and everything orients correctly.

This is what happens on my machines and all of my machines are older haas.

I don't even think they offered repeat tapping on a 1993 machine and it will repeat every time I want it to.

[Geof]

This is what happens on my machines and all of my machines are older haas.

I don't even think they offered repeat tapping on a 1993 machine and it will repeat every time I want it to.

The difference is now they charge you $1000+ for telling you it will do that?

Oh well, I guess they are in business to make a profit, aren't we all (theoretically)?

[miljnor]

I did some tests for you since I was doing a 10-32 tap On another project.

1. 2 flut spirle point alum tap No reduction in shank (ie old school tap) uncoated

I ran it in:

1. blaser 2000 coolant
2. blaser thread lube
3 Moly -d (molybendumdisulfied ) excuse any misspelling please.
4. Dry

All were drilling a .95" deep hole

Alll of the first 3 worked with no hitches into 20 holes each.

number 4 would only go about .4" in before breaking Regardless of peck tapping or not (my guess is galling do to friction and dissimilar metals ect...)

So I wouldn't do it dry!!!

and as far as your machine I would think its maybe an application problem (ie wrong tap or wrong coolant) or you Don't have rigid tapping on this machine or your machine maybe has some parameters set incorectely.

In that order.

Oh.
I didn't try a different drill (maybe because I am lazy!

You could go up in drill size, if your a masochistic SOB and like doing it with no lube!

edit: Oh and Geof My sales person almost said as much to me about the charging 1000.00 for the repeatability issue!

[Geof]

I did some tests for you since I was doing a 10-32 tap On another project.....

He is using 10-24 which I have found to be much less forgiving than 10-32; this is why I suggested pecking even on 0.4" deep. With 10-32 I find it is possible to tap much deeper in one go.

[miljnor]

I don't do any 10-24 stuf so I used what I had.

but I think the test is still valid.

I do some 6-32 stuff and 4-40 as well and I don't have any problems with these going past .4" (of course thats just about as deep as a 4-40 can go )

[miljnor]

I just had another thought as well

One of my old bosses always bought the cheapest material he could lay his hands on (nothing wrong with that ), and sometimes we got this aluminum that was so gummy that you could put your fingernail into the surface. It was still "6061-t651" spec. (or so they said) but We couldn't tap this $h1t for nothing.

So maybe its the material?