Rigid tapping on a Haas

[So not a Guru]

We're trying to get rigid tapping working on our Haas machines. My code format matches the format of their instructional video, but the tap is drilling a tap sized hole. The spindle reveres out. Does anyone see where I've goofed on the code?

N8190 (OPERATION NO - 6)
N8200 T21 M06 (6-32 UNC TAP)
N8210 G54 G17 G90
N8220 S320 M03
N8230 G00 B90. C90.
N8240 G254
N8250 M10
N8260 M12
N8270 T13
N8280 X.2532 Y-.6
N8290 G43 H21 Z4.
N8300 M8
N8310 G94
N8320 G98 G84 Z.5563 R.6263 F10.
N8330 X.2532 Z.5263
N8340 X.2532 Z.4963
N8350 X.2532 Z.4663
N8360 X.2532 Z.4363
N8370 X.2532 Z.4063
N8380 X.2532 Z.3763
N8390 X.2532 Z.3463
N8400 X.2532 Z.3163
N8410 X.2532 Z.2863
N8420 X.2532 Z.2563
N8430 X.2532 Z.2263
N8440 X.2532 Z.1963
N8450 X.2532 Z.1663
N8460 X.2532 Z.1363
N8470 X.2532 Z.1063
N8480 X.2532 Z.0763
N8490 X.2532 Z.0465
N8500 Y.6 Z.5563
N8510 X.2532 Z.5263
N8520 X.2532 Z.4963
N8530 X.2532 Z.4663
N8540 X.2532 Z.4363
N8550 X.2532 Z.4063
N8560 X.2532 Z.3763
N8570 X.2532 Z.3463
N8580 X.2532 Z.3163
N8590 X.2532 Z.2863
N8600 X.2532 Z.2563
N8610 X.2532 Z.2263
N8620 X.2532 Z.1963
N8630 X.2532 Z.1663
N8640 X.2532 Z.1363
N8650 X.2532 Z.1063
N8660 X.2532 Z.0763
N8670 X.2532 Z.0463
N8680 X.2532 Z.0465
N8690 G80
N8700 M9
N8710 M05
N8720 G255
N8730 G53 Z0.
N8740 G53 X-30. Y0.
N8750 M11
N8760 M13
N8770 G53 B0. C0.

[Roger]

This works on our Haas machines.......

%
O0258
(T)
(T1|NO. 6-32 TAPRH|H1|D1)
G20
G0G17G40G49G80G90
T1M6
G0G90G54X0.Y0.S320M3
G43H1Z.1
M8
G99G84Z-.5R.1F10.
G80M9
M5
G91G28Z0.
G28Y0.
M30
%

[So not a Guru]

3 minutes ago, Roger said:

This works on our Haas machines.......

%
O0258
(T)
(T1|NO. 6-32 TAPRH|H1|D1)
G20
G0G17G40G49G80G90
T1M6
G0G90G54X0.Y0.S320M3
G43H1Z.1
M8
G99G84Z-.5R.1F10.
G80M9
M5
G91G28Z0.
G28Y0.
M30
%

I'm sorry, what we're trying to get working is the peck tap (synchronous tapping). I did not do a very good job of describing our trouble.

[Roger]

Would this video help?

 

[Rocketmachinist]

Did you make sure you have repeat tap turned on? Setting 133

[So not a Guru]

3 hours ago, Roger said:

Would this video help?

That's the one I check that our code matched with.

[So not a Guru]

2 hours ago, Rocketmachinist said:

Did you make sure you have repeat tap turned on? Setting 133

Yes, we made sure setting 133 was on.

[navsENG]

2 hours ago, Rocketmachinist said:

Did you make sure you have repeat tap turned on? Setting 133

This, if repeat rigid tap setting is off, it will blow the hole out. 

[civiceg]

Increase your R-plane. Make it .3 above the top of the hole for troubleshooting purposes. (Haas recommends a minimum of .2)

Are you using a retract multiplier? Shouldn't matter, but I would change it to 1 to troubleshoot. Setting 130 or add a J1 to your G84 line. 

[So not a Guru]

1 hour ago, civiceg said:

Increase your R-plane. Make it .3 above the top of the hole for troubleshooting purposes. (Haas recommends a minimum of .2)

Are you using a retract multiplier? Shouldn't matter, but I would change it to 1 to troubleshoot. Setting 130 or add a J1 to your G84 line. 

I'll try this in the morning. Thanks

[htm01]

are you sure you have that option?

[So not a Guru]

6 minutes ago, htm01 said:

are you sure you have that option?

Yes

[BrianP.]

Double check that rigid tapping is enabled by going to parameter 57 and look for rigid tap and be sure there is a 1 there. Curious as to why you are peck tapping every .03? Material? I rigid tap in Haas all the time and never an issue.

[So not a Guru]

49 minutes ago, BrianP. said:

Double check that rigid tapping is enabled by going to parameter 57

The machine we have been testing this on appears to be the only production Haas machine we have that parameter 57 is 0. Why the heck would the control allow setting 133 to be set to 1, if the option is not available? We're going to try it on one of the other machines. Thanks Brian

[civiceg]

Yea, that will do it. I guess you have been float tapping on it?

[BrianP.]

1 hour ago, So not a Guru said:

The machine we have been testing this on appears to be the only production Haas machine we have that parameter 57 is 0. Why the heck would the control allow setting 133 to be set to 1, if the option is not available? We're going to try it on one of the other machines. Thanks Brian

Manually set it to a 1 to enable it. Turn setting 7 to off. Estop the machine. Change 0 to a 1 and you should be good to go if your machine is capable. Turning it on and off keeps the spindle from having to orient every cycle.

Edit: It is standard on some models from the Haas web site. Just need to turn it on.

[civiceg]

You still need an access code on newer non NGC machines, regardless if its a paid option. It can be found in the txt file that is shipped with the machine. Or call into your local HFO for the code.

[So not a Guru]

2 hours ago, civiceg said:

Yea, that will do it. I guess you have been float tapping on it?

Yes, but not intentionally! And not with floating tap[ holders either. might be why this machine has a history of breaking taps! 

We're trying to get the option purchased right now.

[So not a Guru]

3 hours ago, So not a Guru said:

We're going to try it on one of the other machines. Thanks Brian

It works great! 

[civiceg]

Could have sworn it was standard on a UMC. 

[So not a Guru]

2 minutes ago, civiceg said:

Could have sworn it was standard on a UMC. 

Yeah, I'm getting conflicting info on that. Our sales rep said he couldn't find where it was ever not an option on the UMC. But the service tech, who is out here today on another matter, check our serial number in the database & says we don't have the option. 

[civiceg]

It might have been added as standard when the NGC came out, and it was a paid option previously, This is an older one correct? (two years old)

[So not a Guru]

1 minute ago, civiceg said:

This is an older one correct?

Yes, 2014

[Flycut]

Do you have macro variables enabled on your machine?

[So not a Guru]

1 hour ago, Flycut said:

Do you have macro variables enabled on your machine?

I would assume so, since we run probing macros