Fanuc G68.2 with rigid tapping

[huskermcdoogle]

14 minutes ago, Ben Wood said:

Is it possible its looking for pitch instead of ipm for the feedrate?

He's in G94 so I would think not.

 

1 hour ago, g huns said:

It's a 1.

I do believe that's what it should be.

 

Doing some reading. 

The SP0740 alarm is basically stating the spindle is not stopped, or is spinning.  Could you try removing the S145 M3?

The SV0410 is basically the same thing. Check the values in parameter 1829, they should be small. I would hope they aren't 0. 

There is a chance that the SV0410 is being caused when SP0740 is tripped, due to the machine entering emergency and the brake not being engaged fast enough.

But overall these should have no bearing on why it would work with G68.2 turned off and why it wouldn't when it's on. 

Can you post code that you are sure works without G68.2 active?

[Colin Gilchrist]

37 minutes ago, Ben Wood said:

Is it possible its looking for pitch instead of ipm for the feedrate?

Just for jollies, try putting a G94 before the Tap Cycle. (Should be IPM Mode on a Fanuc. G95 should be IPR)

Ok, he is in G94...

[gcode]

11 minutes ago, huskermcdoogle said:

The SP0740 alarm is basically stating the spindle is not stopped, or is spinning.  Could you try removing the S145 M3?

I think this is a winner.

I did not notice this before, but husker is right ...

All the machines I have  that use S*** M29  will alarm out if M03 is active when

S*** M29 is called

I ran into this issue last month working up a post for a VTL/millturn with rigid tapping

[Colin Gilchrist]

Ok, duh. Gcode got it.

Do not start the spindle before the G84 tap call. Gotta remove the "M3" after the Tool Change on Rigid Tap operations...

[gcode]

Just now, Colin Gilchrist said:

Ok, duh. Gcode got it.

no husker got it.. he just gave my wore out brain a kick start

[huskermcdoogle]

I haven't directly written code to tap a hole in 3 years or longer.  So I would consider my brain rusty at best.  Thinking back, I can't remember if I did or didn't have the spindle turning before M29 and G84.  Checking back in a few now, nope, no S### M3 after the tool change.  Just the M29 S###.  By chance @g_huns your code that works doesn't start the spindle?

[gcode]

1 minute ago, huskermcdoogle said:

I haven't directly written code to tap a hole in 3 years or longer.  So I would consider my brain rusty at best.  Thinking back, I can't remember if I did or didn't have the spindle turning before M29 and G84.  Checking back in a few now, nope, no S### M3 after the tool change.  Just the M29 S###.  By chance @g_huns your code that works doesn't start the spindle?

I'm confident that this cycle will run if he kills the S*** G03.

I was fighting this exact problem a month ago and removing S*** M03 from the tool change sequence fixed the problem.

We'll have to waiting a day or so to see if it works though.

It's beer:30 in ghun's neck of the woods

[huskermcdoogle]

2 minutes ago, gcode said:

We'll have to waiting a day or so to see if it works though.

It's beer:30 in ghun's neck of the woods

But I want it NOW!  I don't get no stinking beer at 3 or 4:30.  I'll be lucky to be out of here by 8 or 10 tonight.

[Colin Gilchrist]

1 minute ago, gcode said:

I'm confident that this cycle will run if he kills the S*** G03.

I was fighting this exact problem a month ago and removing S*** M03 from the tool change sequence fixed the problem.

We'll have to waiting a day or so to see if it works though.

It's beer:30 in ghun's neck of the woods

I'm confident as well.

It's always the little things with NC Code. One wrong command, and you're gonna have a bad time.

That's why I originally got into Post Processors in the first place. I wanted to be able to control exactly what the machine is doing. This is one of those situations where just a simple little Post tweak will fix the problem, once you discover what code is really needed.

[huskermcdoogle]

6 hours ago, g huns said:

And our post writer says this post works for his customers running OKK and Makino horizontals.

I'd be willing to bet OKK and Makino both kill the spindle when M29 is commanded.  IIRC Makino uses M135 instead of M29, I bet M135 commands an M5 then M29 S#### either through ladder, macro, or executable, along with some other worth while status checks before letting things proceed.  OKK is probably similar.

[g huns]

43 minutes ago, gcode said:

It's beer:30 in ghun's neck of the woods

Ghuns left the building at 2:30 eastern. He is several beers deep into celebrating Murrica's birthday. He is unable to answer any of your questions.

I'll dig up a non TWP program with rigid tapping and see how it is posted on Thursday.

Thanks for all the suggestions.

[gcode]

5 minutes ago, g huns said:

Ghuns left the building at 2:30 eastern. He is several beers deep into celebrating Murrica's birthday

We knew that!

Happy Birthday America

[Leon82]

should there be g95 instead of g94 to rigit tap?

[huskermcdoogle]

1 hour ago, Leon82 said:

should there be g95 instead of g94 to rigit tap?

You can use either, for g94 you have to calculate a feed that matches the spindle speed, for g95 you can just put the pitch in the feed, and run the spindle at whatever speed you want.  I always used G95/Pitch, I won a lunch bet over it once with a previous boss.  He always calculated out a spindle speed that would yield an even number feed without much rounding.  But the challenge with that is it limits you to a few speeds...  Anyway, he swore up and down our Mori's couldn't rigid tap using pitch for the feed...  They do it just fine.  Much more flexibility to find the right surface speed for the tap to run.

[Newbeeee™]

20 hours ago, gcode said:

I think this is a winner.

I did not notice this before, but husker is right ...

All the machines I have  that use S*** M29  will alarm out if M03 is active when

S*** M29 is called

I ran into this issue last month working up a post for a VTL/millturn with rigid tapping

In which case it must be a parameter issue?

Here's code that I ran on Robos, Chevaliers, Feelers, and a Quaser machine. All machines acted the same way (31i, 0iMC, 0iMD, 0IMF, 16iM).

They'd toolchange, spin up to 1000 rpm, rapid to 10(mm) with the spindle running at 1000, rapid to 5(mm R-Plane), where it would pause at 0 RPM, then synch to the Z starting the spindle (1000rpm) and feeding in from the 5mm to the Z- value, then rotate back out upto the 5mm and next hole.

 

N0602T6M6

M1

( M3 ROLLTAP - BRIGHT FINISH )

( A90 G55 M3 ROLLTAP )

 

G55A90.( A90 G55 M3 ROLLTAP )

G55G0G17G40G49G69G80G90X4.22Y17.75S1000M3

T1M8

G43Z10.H6

M29S1000

G84G98Z-7.R5.Q0.F500.

G80Z10.M9

G28Z10.M19

G49

[gcode]

4 minutes ago, Newbeeee™ said:

In which case it must be a parameter issue?

I can't argue with that, the problem being, only Yoda knows which parameter it is.

The MTB sure doesn't know.

If it works, eliminating M3 at the tool change is a very simple fix. 

We bought a JOBS Ever7 a several years ago.

JOBS assured us that a Fanuc 31i control would be no problem.

Nothing could have been further from the truth

It took nearly 3 years to get the machine running to it's full potential.

I got so I dreaded a visit from the techs, as some obscure parameter tweak would wipe out

6 months of post development  

[Newbeeee™]

Maybe worth a look on PM here. His machine needed rpm before tapping?

Comments by "Bill" are worth a read

https://www.practicalmachinist.com/vb/cnc-machining/first-time-rigid-tapping-fanuc-287713/

[g huns]

Here is a known 'good' program with rigid tapping and no TWP...

G90 G80 G40 G49
G91 G30 Z0.
G90
M906T154
S145 M3
T154
G56
G0 B0. 
X-2.045 Y-5. 
G43 Z3.H 154
M8
(AUTO_DRL - M12 TAP)
G94
M29 S145
G84 G98 X-2.045 Y-5. Z-.70003 R.19997F10.0000
Y5. R.19997
G80
M9
M19
G91 G30 Z0.
G90
G91 G30 X0 Y0
G90
M30
%

The S145 M3 after the tool change causes no problems.

But I also noticed we do NOT have a G17 thrown into the first line which I could see causing problems in a TWP program.

And according to the book, G84 is a tapping cycle and G84.2 is a rigid tapping cycle.

I almost NEVER program this kind of stuff for these machines, so I'm a little oblivious to the problems we are having. But for some reason, I'm the guy who has to figure them out.

A couple of other tidbits; we had two operators recently leave for greener pastures. Since they left, the kid running the Enshus has been a tap breaking fool. I chalked that up to inexperience. But I also recently changed a parameter that was effecting our drilling cycles. Drills were starting to move in Z before the spindle arrived at the programmed speed. Parameter 3708, bit #0 was changed from 0 to a 1. Not sure if that's causing us trouble with breaking taps.

The kid should be out of work tomorrow and I should have time to play around and see what's going on.

[Newbeeee™]

#1 = check your coolant. Clarity and strength...

[Newbeeee™]

On ‎03‎/‎07‎/‎2018 at 8:11 PM, g huns said:

 

I'm glad someone understands it. I feel like a total dumbarse every time I try to make any sense out of it.

 

http://www.google.co.uk/url?sa=t&rct=j&q=&esrc=s&source=web&cd=3&cad=rja&uact=8&ved=0ahUKEwi__r321YjcAhUCUhQKHaoNCeoQFgg3MAI&url=http%3A%2F%2Fheim.ifi.uio.no%2Fmatsh%2Finf4500%2Fcnc%2Ffanuc.pdf&usg=AOvVaw2hlEFS3eR5UgQ0JvjLCXgZ

 

+1

But the above may be of some help too. I don't think it will help your current problem, but it looks a rather well put together document.

For a change...

[g huns]

On 7/3/2018 at 4:22 PM, gcode said:

I'm confident that this cycle will run if he kills the S*** G03...

 

On 7/3/2018 at 4:26 PM, Colin Gilchrist said:

I'm confident as well...

No such luck.

Finally got back to this. We found some weird, unrelated post issues that had to be worked out. And we had ZERO actual work to do in these machines. Which you'd think would be a great time to test things. But instead the operators just go home.

Our rigid tap works with the M03 SXXX before the M29 SXXX as long as we're not using G68.2. But just for fun we removed it and tried with G68.2, still hates it.

As somebody recommended, stuck a G17 in for S&Gs, also no dice.

On 7/3/2018 at 3:47 PM, huskermcdoogle said:

...Check the values in parameter 1829, they should be small. I would hope they aren't 0...

Here you go...

[huskermcdoogle]

3 minutes ago, g huns said:

No such luck.

Interesting.

4 minutes ago, g huns said:

On 7/3/2018 at 2:47 PM, huskermcdoogle said:

...Check the values in parameter 1829, they should be small. I would hope they aren't 0...

Here you go...

Well they aren't zero, so in theory that shouldn't be the cause.

I think someone at Enshu USA needs to get a hold of whoever is in charge of the controls department at Enshu Japan, they should be able to get this solved in about 30 minutes tops.  I think that if it was back channeled this way it would get resolved quickly, worst case they use their contacts at Fanuc Japan to get a deeper answer.  They may need a full control SRAM backup to look into it though.

[gcode]

G90 G80 G40 G49
G91 G30 Z0.
G90
M906T154
S145 M3
T154
G56
G0 B0. 
X-2.045 Y-5. 
G43 Z3.H 154
M8
(AUTO_DRL - M12 TAP)
G94 <<<<<  G95
M29 S145
G84 G98 X-2.045 Y-5. Z-.70003 R.19997 F10.0000   change to pitch
Y5. R.19997
G80
M9
M19
G91 G30 Z0.
G90
G91 G30 X0 Y0
G90
M30
%

 

I would try these edits next

[g huns]

1 minute ago, gcode said:

I would try these edits next...

But I don't wanna use pitch.

I recently had a visit from a couple big shots from Enshu Japan. I sent another email to their US support guys and cc'd the Japanese bosses. See if that gets me some traction.

[huskermcdoogle]

18 minutes ago, g huns said:

But I don't wanna use pitch.

Too funny.  Why people fight pitch for tapping is so far beyond my comprehension I just cease to care.