rigid tapping

[Rick46]

I recently done some experimenting with rigid tapping today and my results were not good. The hole tapped fine but upon reversal out of the hole it stripped the threads out. here is an example of my code as it is output from my tap path.

 

%
O0000(T)
N100 G20
N102 G0 G17 G40 G49 G80 G90
N104 T19 M6
N106 G0 G90 G54 X0.0 Y0.0
N108 G43 H19 Z2.
N110 G95
N112 M29 S1069
N114 G98 G84 Z-.5 R.1 F.05
N116 G80
N118 G94
N120 M5
N122 G91 G28 Z0.
N124 G28 X0. Y0.
N126 M30
%

 

I am using a collet holder that is keyed at the bottom to keep the tap from slipping in the holder itself. I can use the generic tapping with no problems but rigid tapping dose not work well for me. Is it the holder that I am using or something in the machine that needs adjusted in the rigid tapping parameters. On parameter 5211 The override (Draw) is set to 200 in my machine parameters and parameter 5213 retract is set to 2000 in the machine. The machine I am using is a Toyoda FV1050s and it does support rigid tapping. I am wanting to utilize this feature so that I can go back into the same hole but a deeper depth without cross threading the holes and once I get this figured out would like to incorporate a rigid peck tapping cycle in my custom drill cycles in my post. thanks for any help.

[crazy^millman]

I recently done some experimenting with rigid tapping today and my results were not good. The hole tapped fine but upon reversal out of the hole it stripped the threads out. here is an example of my code as it is output from my tap path.

 

%

O0000(T)

N100 G20

N102 G0 G17 G40 G49 G80 G90

N104 T19 M6

N106 G0 G90 G54 X0.0 Y0.0

N108 G43 H19 Z2.

N110 G95

N112 M29 S1069

N114 G98 G84 Z-.5 R.1 F.05

N116 G80

N118 G94

N120 M5

N122 G91 G28 Z0.

N124 G28 X0. Y0.

N126 M30

%

 

I am using a collet holder that is keyed at the bottom to keep the tap from slipping in the holder itself. I can use the generic tapping with no problems but rigid tapping dose not work well for me. Is it the holder that I am using or something in the machine that needs adjusted in the rigid tapping parameters. On parameter 5211 The override (Draw) is set to 200 in my machine parameters and parameter 5213 retract is set to 2000 in the machine. The machine I am using is a Toyoda FV1050s and it does support rigid tapping. I am wanting to utilize this feature so that I can go back into the same hole but a deeper depth without cross threading the holes and once I get this figured out would like to incorporate a rigid peck tapping cycle in my custom drill cycles in my post. thanks for any help.

 

Sorry, but you want to go back into the hole and re-tap it deeper? Why not just tap it deep enough to begin with? Using a spiral tap and the proper cutting fluid on the tapped hole should allow you to go the depth needed for your application. That of course is if thread milling would not work which what I would attempt.

 

If is not coming out of the hole without stripping the thread and you feel like you have rules out the holder then it has to be a machine problem. Get on the phone to machine builder and have them do a service call on the machine. You can peck tap without coming out of the hole on some machines, but I am not sure about it on this machine. If that is possible then that might be your best approach once you get this issue worked out.

 

I was doing some tapping on a machine many years ago and it was not doing what I would expect. Owner was cussing me for everything I was worth because I could not get it to work, then he got even madder that I called the machine builder and sure enough it was a machine problem. I never got an apology for getting the machine fixed and getting it to run correctly. He was one of those types that hated CNC Machines and if you did anything better than him to make the company (Him) more money he would get pissed. Tell you I don't miss those days. I learned a lot about different types of machining, but it was most times trail by fie and getting yelled and screamed at.

[Rick46]

The reason I don't tap it to the true depth in one step is due to low spindle torque. this is why I was attempting to rigid tap on this machine today. I have done it on other machines with no problem but this machine has never had rigid tapping run on it and its supposed to be one of the strong points of this machine in particular.It was a 16.0 x 2mm tap that was giving me problems in H-13 steel. I tapped them with the generic tap to Z -.875 deep using tapping oil and it had the spindle load at 65% so I left them at that and I tapped them by hand the rest of the way to depth. So during some free time today in aluminum I thought I would use rigid tap and just go back into the hole to the required depth of -1.625 in Z and thus the problem with the stripped threads with the first depth of  Z-.875. I could have thread milled them but I wanted to utilize the rigid tapping on this machine for no one prior to me running had ever attempted it nor had a reason as to why they did not attempt it. I like to know the machine I am running can do what its supposed to be capable of when and if I choose to go the route in question. Normally I just thread mill anything over 1/2 and run a tap down the hole by hand if I cant reach my intended depth with thread mill. I was just experimenting was all. If it doesn't work then so be it but just looking for any info as to why it might not work if its on my end or something with the machine. Its due for its annual maintenance in a couple months I may just wait and ask the guy doing the scheduled machine PM and pick his brain about it if I don't get it figured out sooner. thanks for the info Ron. Again just doing some experimenting so that if rigid tapping is needed I know I can do it in the future.

[BenK]

Your feed should be 2mm or .0787" not .05" for your tap using feed per rev. If you are worried about horsepower I would thread mill anything this large. As for peck tapping, add a Q.1 to your G84 line and it will do a .1 peck.

 

 

 

Fanuc G84 Peck Rigid Tapping Cycle Format

 

G84 X_ Y_ Z_ R_ P_ Q_ F_ K_ ;

X Y – Hole position.

Z – Z-depth (feed to Z-depth starting from R plane).

 

R – Position of the R plane.

P – Dwell time at the bottom of the hole and at point R when a return is made.

Q – Depth of cut for each cutting feed (Peck depth).

F – The cutting feedrate.

K – Number of repeats (if required).

 

 

As a general rule I wouldn't try re-running a tap, it usually doesn't end well.

[mike93]

if you are using pitch on your machine i would not be right ether.

[Justin Beebe at Folsom Tool]

If you want to use feed instead of pitch use this formula:   1/(2/25.4) = 12.7 threads per inch.  Then for an example you could use S127 feed of 10. or  S1270 feed of 100........etc

[NiCu2829]

Your feed should be 2mm or .0787" not .05" for your tap using feed per rev. If you are worried about horsepower I would thread mill anything this large. As for peck tapping, add a Q.1 to your G84 line and it will do a .1 peck.

 

 

Fanuc G84 Peck Rigid Tapping Cycle Format

 

G84 X_ Y_ Z_ R_ P_ Q_ F_ K_ ;

X Y – Hole position.

Z – Z-depth (feed to Z-depth starting from R plane).

 

R – Position of the R plane.

P – Dwell time at the bottom of the hole and at point R when a return is made.

Q – Depth of cut for each cutting feed (Peck depth).

F – The cutting feedrate.

K – Number of repeats (if required).

 

As a general rule I wouldn't try re-running a tap, it usually doesn't end well.

When I use a P command on my G84 line the spindle continues to rotate at the bottom of the hole, ruining the threads. I'm working on a Doosan Puma 2600SY lathe. Also when I use M29 (rigid tapping) w/ G84 it unlocks the spindle so I'm only able to use rigid tapping on center. Any thoughts or insight would be greatly appreciated. Thanks.

[Guest MTB Technical Services]

When I use a P command on my G84 line the spindle continues to rotate at the bottom of the hole, ruining the threads. I'm working on a Doosan Puma 2600SY lathe. Also when I use M29 (rigid tapping) w/ G84 it unlocks the spindle so I'm only able to use rigid tapping on center. Any thoughts or insight would be greatly appreciated. Thanks.

 

 

You need to read your manual and properly format your code.

 

The P address on a Doosan indicates which spindle is active as in S1000 M03 P11 (Main Turning Spindle)

You need an M35 to tell the machine you are now using a live tool.

You need an M176 for Left-hand tapping and M177 for right-hand tapping.

 

M35 (Live Tooling Mode - Engage C-axis)

G28 H0.

G00 X50.0 C0.0 (Positioning the drill along the X and C axis)

M177 (Right-hand Tapping)

M29 S1000 P12 (Rigid Tap mode - P12 indicate Live Tool Spindle at 1000 RPM)

G84 Z-30.0 R-5.0 F1500 M89 (Tapping hole 1 Along Z Axis - G88 for X-Axis Tapping)

C90.0 M89 (Tapping hole 2)

C180.0 M89 (Tapping hole 3)

C270.0 M89 (Tapping hole 4)

G80 (Cancel the Tapping cycle)

M05 P12 (Stop Live Tool)

M34 (Return to Turning Spindle Mode)

[NiCu2829]

You need to read your manual and properly format your code.

 

The P address on a Doosan indicates which spindle is active as in S1000 M03 P11 (Main Turning Spindle)

You need an M35 to tell the machine you are now using a live tool.

You need an M176 for Left-hand tapping and M177 for right-hand tapping.

 M35 (Live Tooling Mode - Engage C-axis)

G28 H0.

G00 X50.0 C0.0 (Positioning the drill along the X and C axis)

M177 (Right-hand Tapping)

M29 S1000 P12 (Rigid Tap mode - P12 indicate Live Tool Spindle at 1000 RPM)

G84 Z-30.0 R-5.0 F1500 M89 (Tapping hole 1 Along Z Axis - G88 for X-Axis Tapping)

C90.0 M89 (Tapping hole 2)

C180.0 M89 (Tapping hole 3)

C270.0 M89 (Tapping hole 4)

G80 (Cancel the Tapping cycle)

M05 P12 (Stop Live Tool)

M34 (Return to Turning Spindle Mode)

Hello Tim,

 

First off thank you. I looked through the manual but missed the M177. I'll be sure to try it tomorrow, other than that our code looks the same. I understand the use of the P address in relation to the spindles meaning it can't be used on a G84 line?

 

Thanks again

 

Branden

[Guest MTB Technical Services]

Hello Tim,

 

First off thank you. I looked through the manual but missed the M177. I'll be sure to try it tomorrow, other than that our code looks the same. I understand the use of the P address in relation to the spindles meaning it can't be used on a G84 line?

 

Thanks again

 

Branden

 

 

You are probably still missing something.

Post your code so I can see what you have.

 

The P address is permissible but remember that it is a Dwell and the value is in milliseconds.

No decimal point.

[civiceg]

If you decide to peck tap it, you most likely will have to set the back off parameter. Most of the new Fanucs I have seen had it set to zero or something ridiculous. Also, you can setup up rigid tapping without a M29 (parameter is labeled g84). But, it will make all tapping rigid. 

 

Edit, in reference to OP mill problem only...just realized the thread was bumped and not new

[NiCu2829]

You are probably still missing something.

Post your code so I can see what you have.

 

The P address is permissible but remember that it is a Dwell and the value is in milliseconds.

No decimal point.

T0909

M90

M35

G28 H0.

G0 G54 X5. Z.25 C0.

M177

G97 S500 M29 P12

G84 Z-.5 P2000 F.0625 M89

C180. M89

G80

 

Thanks,

 

Branden

[Guest MTB Technical Services]

Your aren't positioning properly before calling the cycle.

You should be at your start point in XC and initial Z before calling the cycle.

It's poorly formatted code because you don't have an explicit Z initial position.

 

However, the fact you don't have an R word on the G84 is your problem.

You aren't telling it to retract properly.

The R-Word MUST be there.

 

The R-Word for drilling cycles is different in turning.

It is the incremental distance from the initial level to point R level.

 

If your initial position and R-Plane are the same, R0 is what you should have in your cycle.

 

If your initial position is Z1.0 and the R-Plane is at Z0.1, R-0.9 is what you should have in your cycle.

[NiCu2829]

Your aren't positioning properly before calling the cycle.

You should be at your start point in XC and initial Z before calling the cycle.

It's poorly formatted code because you don't have an explicit Z initial position.

 

However, the fact you don't have an R word on the G84 is your problem.

You aren't telling it to retract properly.

The R-Word MUST be there.

 

The R-Word for drilling cycles is different in turning.

It is the incremental distance from the initial level to point R level.

 

If your initial position and R-Plane are the same, R0 is what you should have in your cycle.

 

If your initial position is Z1.0 and the R-Plane is at Z0.1, R-0.9 is what you should have in your cycle.

 

Will it work if my initial Z position is Z.25?

 

T0909

M90

M35

G28 H0.

G0 G54 X5. Y0. Z.25 C0.

M177

G97 S500 M29 P12

G84 Z-.5 R0. P2000 F.0625 M89

C180. P2000 M89

G80

 

I greatly appreciate the insight Tim.

 

Thanks,

 

Branden

[Guest MTB Technical Services]

Will it work if my initial Z position is Z.25?

 

T0909

M90

M35

G28 H0.

G0 G54 X5. Y0. Z.25 C0.

M177

G97 S500 M29 P12

G84 Z-.5 R0. P2000 F.0625 M89

C180. P2000 M89

G80

 

I greatly appreciate the insight Tim.

 

Thanks,

 

Branden

 

 

Sure.

 

However, a rapid approach with all axes is something i avoid like the plague.

 

G00 G28 U0 V0

G00 G28 W0

Txx00

M01

 

T0909

M90

M35

G28 H0.

G0 G54 X5. C0. (Y0 isn't needed)

Z.25

M177

G97 S500 M29 P12

G99 (Explicit UPR Mode Call for Tapping with Pitch for Feedrate)

G84 Z-.5 R0. P2000 F.0625 M89

C180. P2000 M89

G80

[NiCu2829]

Sure.

 

However, a rapid approach with all axes is something i avoid like the plague.

 

G00 G28 U0 V0

G00 G28 W0

Txx00

M01

 

T0909

M90

M35

G28 H0.

G0 G54 X5. C0. (Y0 isn't needed)

Z.25

M177

G97 S500 M29 P12

G99 (Explicit UPR Mode Call for Tapping with Pitch for Feedrate)

G84 Z-.5 R0. P2000 F.0625 M89

C180. P2000 M89

G80

 

Tim,

 

It's easy to see why people say you're the "best resource for these machines." THANK YOU.

 

 

Sincerely,

 

Branden

[Guest MTB Technical Services]

Tim,

 

It's easy to see why people say you're the "best resource for these machines." THANK YOU.

 

 

Sincerely,

 

Branden

 

 

I appreciate the kind words but that's really not the case.

 

When it comes to Doosan, Bob Appleton at Doosan HQ is the best there is.

[NiCu2829]

I appreciate the kind words but that's really not the case.

 

When it comes to Doosan, Bob Appleton at Doosan HQ is the best there is.

 

I recognize the name.

 

I tried the code today to no avail. The P address worked as it should but the spindle still unlocked once it read the M29. I had the M89 on the G84 line and the machine wouldn't continue on. I deleted the M89 and it would run but the spindle would unlock. I should also mention that if I type in M35 in MDI the spindle locks but when I put it in handle it unlocks. So I can not manually rotate the C axis in handle mode. Not sure why? I know that M89 is set in the parameters for clamping but I didn't check M289/M389?

 

Best regards,

 

Branden B.

[Guest MTB Technical Services]

I recognize the name.

 

I tried the code today to no avail. The P address worked as it should but the spindle still unlocked once it read the M29. I had the M89 on the G84 line and the machine wouldn't continue on. I deleted the M89 and it would run but the spindle would unlock. I should also mention that if I type in M35 in MDI the spindle locks but when I put it in handle it unlocks. So I can not manually rotate the C axis in handle mode. Not sure why? I know that M89 is set in the parameters for clamping but I didn't check M289/M389?

 

Best regards,

 

Branden B.

 

 

You should call Doosan because your machine is not acting normally.

You'll want to check if M289 is on by default.

If it's not, you'll need to command M289 before the G84 canned cycle call.

 

Why do you want a 2 second dwell at the bottom of the tapped hole?

I've never done anything like that with rigid tapping.

I never use a dwell with tapping at all.

[NiCu2829]

You should call Doosan because your machine is not acting normally.

You'll want to check if M289 is on by default.

If it's not, you'll need to command M289 before the G84 canned cycle call.

 

Why do you want a 2 second dwell at the bottom of the tapped hole?

I've never done anything like that with rigid tapping.

I never use a dwell with tapping at all.

I'll give them a call. I've never put a dwell at the bottom of a tapped hole either. I was curious as to why someone would use that feature and I wanted to figure out why it wasn't working like it was supposed to. I got this number from their website 1-888-9Doosan(936-6726). Is this the best number to contact them or should I e-mail technical support? Thanks for all your help Tim.

 

Best regards,

 

Branden B.