Problem with G84

Hi Guys,
We have recently put in our first VMC and have run into a problem with rigid tapping.
I am a complete noob when it comes to programming.
Machine is a 2006 AMS MCV500
Fanuc Oi-MC control.
Code is being run as generated from Fusion 360.
Using DNC from the PCMCIA slot.
Operating in metric.

The machine runs the tapping cycle, retracts and then gets hung up once the tool reaches the retract height. There is no alarm or message. The controller sticks on the G80 line of code. The threads are fine.

After stopping the cycle i then get a message saying that the rigid tapping cycle was interrupted and to press lube inch to clear the message.

Other canned cycles work fine.

This is the code:
(DRILL6)
N900 M09
N905 M01
N910 T6 M06
N915 T1
N920 S500 M03
N925 G54
N930 M07
N935 G00 X32. Y-15.875
N940 G43 Z15. H06
N945 G00 Z5.
N950 M29 S500
N955 G84 X32. Y-15.875 Z-33.75 R3.25 P500 F750.
N960 G80
N965 Z15.

Thanks in advance,
Ueee

Ueee said:

Hi Guys,
We have recently put in our first VMC and have run into a problem with rigid tapping.
I am a complete noob when it comes to programming.
Machine is a 2006 AMS MCV500
Fanuc Oi-MC control.
Code is being run as generated from Fusion 360.
Using DNC from the PCMCIA slot.
Operating in metric.

The machine runs the tapping cycle, retracts and then gets hung up once the tool reaches the retract height. There is no alarm or message. The controller sticks on the G80 line of code. The threads are fine.

After stopping the cycle i then get a message saying that the rigid tapping cycle was interrupted and to press lube inch to clear the message.

Other canned cycles work fine.

This is the code:
(DRILL6)
N900 M09
N905 M01
N910 T6 M06
N915 T1
N920 S500 M03
N925 G54
N930 M07
N935 G00 X32. Y-15.875
N940 G43 Z15. H06
N945 G00 Z5.
N950 M29 S500
N955 G84 X32. Y-15.875 Z-33.75 R3.25 P500 F750.
N960 G80
N965 Z15.

Thanks in advance,
Ueee

Click to expand...

As just a test, edit the program as follows to see if it still hangs.

N945 G00 Z5.
N950 M29 S500
N955 G84 X32. Y-15.875 Z-33.75 R3.25 P500 F750.
N960 G00 Z15.0

"G00" is a valid code to cancel a Canned Cycle

Regards,

Bill

Chuck in a G94 (feed per MM) after the G80 might help.

Sent from my SM-N960F using Tapatalk

smachservices said:

Chuck in a G94 (feed per MM) after the G80 might help.

Sent from my SM-N960F using Tapatalk

Click to expand...

Hello smachservices,

I very much doubt that the control was in Feed per Rev mode and feeding at 750mm, as specified in the G84 Block, per revolution.

Regards,

Bill

You might need a G98 or G99 next to your G84. As far as I can see you have nothing telling it where to return to in Z after it taps the hole.

Sent from my SM-N960U using Tapatalk

cb750chris said:

You might need a G98 or G99 next to your G84. As far as I can see you have nothing telling it where to return to in Z after it taps the hole.

Sent from my SM-N960U using Tapatalk

Click to expand...

Hello cb750chris,
The OP's programming form is not great. Its good practice to specify either G98 or G99 with a Canned Cycle, just so you can see at a glance what to expect of the program. However, it will be one or the other; it can't be neither.

When the clear state bit 6 (CLR) of parameter 3402 is set to "1", the Modal G codes are placed in state when Power Up, or Reset is pressed. In this case G98 would be in state.

Regards,

Bill

I hadn't thought about it being modal. I've just always been in the habit of putting it on the specific line so I know what it's doing. Good to know! I'll have to look and see if my machine does that just out of curiosity. It's a Milltronics, so not a fanuc control, but uses basic fanuc codes with some exceptions.

Sent from my SM-N960U using Tapatalk

could it be your P value is in seconds, and it's waiting?
Run it high with no P and see what happens

That canned cycle looks funky to me.
I always write mine like this:

S1000 M03
M08
G84 G99 Z-5. R3. F(50?) L0
(hole locations in X,Y)
G80
G00 Z20.


Must be a Fusion thing.....

Larry Dickman said:

could it be your P value is in seconds, and it's waiting?
Run it high with no P and see what happens

Click to expand...

That might be it. I think on my control the P is in seconds (I never use it as I don't tap at high speeds), so if that's the case it would wait for over 8 minutes (P500) after it taps the hole before moving on to the next line. Would explain why there's no error code either.

Sent from my SM-N960U using Tapatalk

Usually a P in a canned cycle is a dwell at the bottom. On a tapping cycle it would allow an extension holder to extend before reversing.
On a spot drill I use it on really big chamfers for consistency in size ie:
G82 G98 Z-.3 R.1 F10. P250

On a soft tapping cycle, yes. But on rigid tapping it's a dwell at the top to allow the spindle to reverse before going on to the next hole. At least that's the case with my mill.

Sent from my SM-N960U using Tapatalk

cb750chris said:

It's a Milltronics, so not a fanuc control, but uses basic fanuc codes with some exceptions.

Sent from my SM-N960U using Tapatalk

Click to expand...

IIRC the Milltronics assumed G98, but neither is actually needed in the code: although, it has been almost 8 years since I sold mine.

Doug.

doug925 said:

IIRC the Milltronics assumed G98, but neither is actually needed in the code: although, it has been almost 8 years since I sold mine.

Doug.

Click to expand...

I looked in the book and it appears that 98/99 are one shot, not modal, and neither are active on startup. I dont know if that's the reality in actual use though, since I always put it on the canned cycle line anyway.

Sent from my SM-N960U using Tapatalk

cb750chris said:

On a soft tapping cycle, yes. But on rigid tapping it's a dwell at the top to allow the spindle to reverse before going on to the next hole. At least that's the case with my mill.

Sent from my SM-N960U using Tapatalk

Click to expand...

Hell cb750chris,
With a Fanuc Control such as the OP's Oi Control, in Rigid Tapping the "P" address specifies a Dwell time at the bottom of the hole and at point R when a return is made.

Generally its not required and although the resolution of the "P" address is 0.001 seconds and shouldn't be the issue with the OP's program, I can't see any good reason for it to be included in his program.

If the "P" address were to be the issue, ie P500= 500 seconds, then the program should also be appearing to hang at the bottom of the tapped hole.

Regards,

Bill

angelw said:

Hell cb750chris,
With a Fanuc Control such as the OP's Oi Control, in Rigid Tapping the "P" address specifies a Dwell time at the bottom of the hole and at point R when a return is made.

Generally its not required and although the resolution of the "P" address is 0.001 seconds and shouldn't be the issue with the OP's program, I can't see any good reason for it to be included in his program.

If the "P" address were to be the issue, ie P500= 500 seconds, then the program should also be appearing to hang at the bottom of the tapped hole.

Regards,

Bill

Click to expand...

Hi Bill,

I'm not overly familiar with fanuc on mills, mostly ran lathes with it. I do know that on my particular mill the P value is in full seconds. Not much help to the OP I realize, just trying to give some ideas where to look. Also, the dwell on mine only applies to the top of the hole in a rigid tap cycle. I know why you would want one at the bottom during a soft tapping cycle when using a TC holder, but why would you ever have one in a rigid tap cycle? As I understand it, the Z axis is electronically "slaved" to the spindle and slows down as the spindle slows and speeds back up to match the spindle in reverse. Hence the need for a spindle encoder for rigid tapping. Just wondering what situation might call for that dwell, for my own knowledge.

Chris

Sent from my SM-N960U using Tapatalk

Hello Chris,
A copy and Paste from Fanuc Manual.



Regards,

Bill

Command G80 twice in two consecutive blocks.

Thank guys,
I will try the G00 and the extra G80 when i'm in front of the machine tomorrow.
I doubt the P value is the problem as said it would cause a pause at the bottom of the hole, but i will try with no P value.
I would assume that G98 is active since it does return to the start point of the cycle. I can see why having it in the block is good practice though, so you you know exactly what to expect at a glance.
Thanks again for your help,
Ueee

Ueee said:

Thank guys,
I will try the G00 and the extra G80 when i'm in front of the machine tomorrow.
I doubt the P value is the problem as said it would cause a pause at the bottom of the hole, but i will try with no P value.
I would assume that G98 is active since it does return to the start point of the cycle. I can see why having it in the block is good practice though, so you you know exactly what to expect at a glance.
Thanks again for your help,
Ueee

Click to expand...

Hello Ueee,
The use of G00 Z15.0 instead of G80 is a bit of a Clutch at Straws on my part, as your program looks like it should function. But its well documented that a Canned Cycle can be cancelled using a Group 01 G Code instead of G80. To see this in motion, program G00 in the any Block after the Cycle Call and instead of Drilling, or Tapping to depth at each specified X/Y location, the Spindle will move to each location at rapid speed and the program move to the next Block without executing the Cycle. Whatever Group 01 G Code was active before the execution of the Canned Cycle, will be active when the Canned Cycle is canceled. In your case, G00 was active before the Cycle, with N945 G00 Z5.0 and therefore, would be active after cancel. However, any axis coordinate specified before the Cycle is cancelled (without a Group 01 G Code specified) will just update the axis coordinate to use in the current Canned Cycle.

Its as if the Rigid Tapping Cycle is not being cancelled by G80 and because the next Block has a Axis Coordinate without a Group 01 G Code specified, the Z data of the cycle is being updated. In this case, I would expect the cycle to use Z15.0 as the next Z Target. But because its specified as a plus value, or without either an X or Y, or both, may be confusing the control.

The inclusion of the Dwell specified with "P" is unlikely to be causing an issue. As you have noted, it should have also caused an issue at the bottom of the hole due to any dwell specified is executed at the Bottom of the Hole and at the R Plane when the tool is retracted. The speeds and feeds being used in your program are quite benign, therefore, there is no need whatsoever for inclusion of a dwell.

Regards,

Bill