What's new
What's new

Need help programing a simple face drilling hole pattern with Fanuc 16-TT Naka TW10

NASTYZEN

Plastic
Joined
May 20, 2010
Location
St-Colomban,Que. Canada
Hey guys!
I've been trying to get the C to reposition after drilling the first hole of three that I need to drill on the face of this part for two days now..
I tried everything in the book and more to no avail.
It drills the first hole fine but fails to rotate 120Deg to perform the next hole. Just repeats three times in the the first one.:wall:
What am I doing wrong??
I attached the examples from the manual that came with the machine.
The only thing that I changed from the examples was to substitute the M98 P9000 to call the C axis with a G91.
The controller does not recognize the P9000 sub program.
I am beginning to think that I have to change something in the ladder?
Machine is a Nakamura Tome TW-10 twin spindle twin turret lathe with Fanuc 16-TT controller.Naka C.jpgNaka C 2.jpg
 
I attached the examples from the manual that came with the machine.
The only thing that I changed from the examples was to substitute the M98 P9000 to call the C axis with a G91.
The controller does not recognize the P9000 sub program.
I am beginning to think that I have to change something in the ladder?
Machine is a Nakamura Tome TW-10 twin spindle twin turret lathe with Fanuc 16-TT controller.View attachment 322761View attachment 322762

Hello NASTYZEN,
What do you mean by calling the C axis with a G91. Are you attempting to Call program O9000 with a Custom G Code (in this case G91)? If so, that's not possible. To call Program O9000 by means other than with G65 or M98, parameter bit 6001.5 has to be set to "1" for O9000 to be called with a "T" Code only, or with G65 P9000 and M98 P9000.

When you say that the control doesn't recognize the P9000 Subprogram, is an alarm being raised when M98 P9000 is executed, indicating that the program doesn't exist? It states in your operators manual that M98 P9000 is called to engage Spindle Positioning Mode. Accordingly, if program O9000 doesn't exist, that is probably a lot of your problem.

If Program O9000 doesn't exist in your control, there may be a hard copy of it somewhere in the machine's manuals.

Post a copy of your actual program.

Regards,

Bill
 
Hello Angelw,
Wow, quick response!
Yes I get an alarm with P9000. Will look in the book for a hard copy. There is a flow chart explaining the sequence of starting what they call the CF control.
I learned to bypass the P9000 with G91 to be able to start the live tooling on the first part I ever did with the machine with the help of another member here. But I was only making one face hole and didn't notice the pattern glitch then.
I've had to make other parts using the G112 using the C to mill flats and it all works fine. Just can't get a simple hole pattern to work.
So here is one of the code snippet attempts the of what I'm trying to do.View attachment FACE DRILL OP.txt

N185M01
N190M91G50C0(C AXIS SELECT)
N200G0G40G98G97T0909M88S1200(LIVE TOOL ON SUB PROGRAM)
N205T0909(90DEG LIVETOOL #21 DRILL)
N206G28W0.0U0.0(XZ HOME POS)
N210M86(C BRAKE ON)
N215G00X1.0Z.3
N220G98
N225G01Z-.1F003.M08
N230G00Z.3M09
N235M87(C AXIS BRAKE OFF)
N240H120
N245M86(C BRAKE ON)
N250G01Z-.1M08
N255G00Z.3M09
N260M87(C BRAKE OFF)
N265H120
N270M86(C BRAKE ON)
N275G01Z-.1M08
N280G00Z.3M09
N285M87(C BRAKE OFF)
N290G00X1.6M05
N295G00U0.0
N300G28W0.0U0.0(XZ HOME POS)
N305G28W0.0U0.0(XZ HOME POS)
N310T0909M09
N315M41
N320M01
 
Last edited:
Hello NASTYZEN,
What is happening then is the 120deg Incremental move of Blocks 240 and 265 are not being executed. Going by the listing of your program, normally the "C" axis should index by 120degs, as you're not even using a Canned Cycle where you may have made an error with the syntax. Accordingly, its the lack of program O9000 being executed that's inhibiting the C axis moves.

The three examples shown in pictures in your previous Post, drilling a hole pattern with Longhand Code and using a Canned Cycle, specifically use M98 P9000 in each. Even in the second picture, showing code examples for milling and face drilling, M98 P9000 is only used when positioning the "C" axis for drilling. If you can't find a copy of the O9000 program, Post a copy of the O9000 flow chart you mentioned in your Post.

What function does G91 have with your control? Depending on the "G" Code system used by your control, G91 will normally be either Incremental Mode, or not used. The use of G98 in all three examples in the manual and in your program listing, would indicate that "G" Code System A is used with your control, therefore, G91 would normally have no function.

With G112, rapid moves can't be used whilst that mode is active. It may also be the case when not in what your manual describes as Spindle Positioning Mode.

I suspect that the following would work for Blocks N240 and N265:

N240 G01 H120 F_ _

and

N265 G01 H120 F_ _

Where:
F_ _ = A hefty feed rate approaching that of Rapid Traverse of the "C" axis.


Regards,

Bill
 
I hesitate to get involved in any thread that Bill is actively posting in because I'll most likely make a fool of myself, but here goes anyway...

Don't you need a period after each H120? I'm thinking that the control is reading those lines as .012 degree incremental moves and drilling the holes at seemingly the same place.

Also, is the OP mistakenly referring to the M91 in the second line as G91? That could be creating some of the confusion. I do agree, though, that it would be good to get a copy of the O9000 program that the book refers to.
 
Don't you need a period after each H120? I'm thinking that the control is reading those lines as .012 degree incremental moves and drilling the holes at seemingly the same place.

Hello wmpy,
Good point with regards the omitted period for the C axis move. Via parameter, the control can be set to what Fanuc refers to as Pocket Calculator Mode and in doing so, numbers specified without a period are treated as Integers. However, Pocket Calculator Mode is not the Fanuc default setting and therefore, if the Least Linear Command Increment is 0.0001", Degrees will be 0.001, an incremental C axis move of 0.120deg at X1.0 (0.5 Rad), the out of position relative to the first hole is only 0.00105" and 0.00209" for the third hole relative to the first. In this case, a drill would easily follow the first hole without any complaint and appear as no index had occurred.

Regards,

Bill
 
.........In this case, a drill would easily follow the first hole without any complaint and appear as no index had occurred.

Regards,

Bill

The position display of the control would show .120 at the second hole and .240 at the third hole. This seems to me to be hard to overlook and a powerful clue in figuring out what is going on.
 
The position display of the control would show .120 at the second hole and .240 at the third hole. This seems to me to be hard to overlook and a powerful clue in figuring out what is going on.

Hello Kevin,
!00% agree, but you need to be looking. If the missing periods in the program listing are not typos when presenting it to the Forum, then the OP could miss the position display. But now that it's been suggested, it would be easy for the OP to prove for sure.

Regards,

Bill
 
Hey guys, we have a winner!
I could not get in the shop to play with this problem over the weekend as I was set to WP1. (wife priority one) as you all know, this command overrules all other ongoing OP programs..

Wmpy put his finger on it. The period after the H120. did the trick. The position display did in fact move by .120 and .240 We now have a three hole pattern going on. Noob mistake on my part for not checking the pos display.:ack2:

Bill, I believe the P9000 sub program C axis call-up or what they call CF control is erroneous and actually called by the M91 which is selection of the C axis in the books G code list. Already sent me down the rabbit hole previously.
Thanks for all the help guys!
Next and final op, getting a tapping cycle to work on these holes.

Cheers
Claude
 
Wmpy put his finger on it. The period after the H120. did the trick. The position display did in fact move by .120 and .240 We now have a three hole pattern going on. Noob mistake on my part for not checking the pos display.:ack2:

Cheers
Claude
Hello Claude,
Kudos to you for following up on your Thread and reporting the cause of your issue; this can be a big help to others that may have a similar problem and have been following your Thread.

All too often a fix will be suggested by a Forum Member then Zero feedback from the OP leaving others wondering was that the fix or not.

Regards,

Bill
 
Hey guys!
I've been trying to get the C to reposition after drilling the first hole of three that I need to drill on the face of this part for two days now..
I tried everything in the book and more to no avail.
It drills the first hole fine but fails to rotate 120Deg to perform the next hole. Just repeats three times in the the first one.:wall:
What am I doing wrong??
I attached the examples from the manual that came with the machine.
The only thing that I changed from the examples was to substitute the M98 P9000 to call the C axis with a G91.
The controller does not recognize the P9000 sub program.
I am beginning to think that I have to change something in the ladder?
Machine is a Nakamura Tome TW-10 twin spindle twin turret lathe with Fanuc 16-TT controller.View attachment 322761View attachment 322762
Good afternoon, my name is David Toloza from Colombia. I am new to these forums but I need help. I bought two Nakamura lathes. I took tw10 Fanuc 16TT control. axis c since I get a 411 alarm, the engineer tells me that we have a wrong parameter, could you help me?
 

Attachments

  • WhatsApp Image 2024-02-08 at 08.31.36 (3).jpeg
    WhatsApp Image 2024-02-08 at 08.31.36 (3).jpeg
    105.1 KB · Views: 2
  • WhatsApp Image 2024-02-08 at 08.31.36 (4).jpeg
    WhatsApp Image 2024-02-08 at 08.31.36 (4).jpeg
    181.2 KB · Views: 2
Good afternoon, my name is David Toloza from Colombia. I am new to these forums but I need help. I bought two Nakamura lathes. I took tw10 Fanuc 16TT control. axis c since I get a 411 alarm, the engineer tells me that we have a wrong parameter, could you help me?
 

Attachments

  • WhatsApp Image 2024-02-08 at 08.31.36 (3).jpeg
    WhatsApp Image 2024-02-08 at 08.31.36 (3).jpeg
    105.1 KB · Views: 1
  • WhatsApp Image 2024-02-08 at 08.31.36 (4).jpeg
    WhatsApp Image 2024-02-08 at 08.31.36 (4).jpeg
    181.2 KB · Views: 1








 
Back
Top