Need Help!- G7.1 Fanuc 10T

[Lene Madsen]

I need to make a helical cut down a Ø10mm steel bar (think twist drill).

I have a Fanuc 10T Model A controller and have been thinking of using the G-code 7.1 to turn on cylindrical interpolation.

I have found a program example in my manual, but I must be missing some vital information because my machine brings an alarm saying improper g-code whenever I try to run it.

My program looks like this:

O0010
G96 G99 G50 S500 M9
G0 X-20.
M7
G0 Z0. M56
M6
X54. T300
G0 X0. Z-1. T303
G1 Z0. M3 S75 F.25
X8. Z3.
Z25.
G3 X13. Z27.5 R2.5
G0 X14. Z-5.
X5.
M5
G7.1 C4
G1 Z0. F50
G3 Z0. C0 R2.5
G1 Z25. C180
G7.1 C0
G0 X14. Z27.
G1 X12. Z33.5
G3 X10. Z36. I2.5
G1 Z57.5
G1 X-10.
M5
M2
M99

Can anyone see an error or does anyone have any suggestions to a better way of programming. I need 2 helix with a distance of 180 degrees.

Thanks you!

[angelw]

Originally Posted by Lene Madsen I need to make a helical cut down a Ø10mm steel bar (think twist drill). I have a Fanuc 10T Model A controller and have been thinking of using the G-code 7.1 to turn on cylindrical interpolation. I have found a program example in my manual, but I must be missing some vital information because my machine brings an alarm saying improper g-code whenever I try to run it. My program looks like this: O0010 G96 G99 G50 S500 M9 G0 X-20. M7 G0 Z0. M56 M6 X54. T300 G0 X0. Z-1. T303 G1 Z0. M3 S75 F.25 X8. Z3. Z25. G3 X13. Z27.5 R2.5 G0 X14. Z-5. X5. M5 G7.1 C4 G1 Z0. F50 G3 Z0. C0 R2.5 G1 Z25. C180 G7.1 C0 G0 X14. Z27. G1 X12. Z33.5 G3 X10. Z36. I2.5 G1 Z57.5 G1 X-10. M5 M2 M99 Can anyone see an error or does anyone have any suggestions to a better way of programming. I need 2 helix with a distance of 180 degrees. Thanks you!

That alarm normally means that the "G" code doesn't exist for the control and hence, your machine doesn't have that option. If you have the Fanuc specification sheet that came with the machine it will tell you there if the machine has the option.

Regards,

Bill

[Lene Madsen]

Thanks for your response Bill.

I have checked operators manual, controller manual and my appendices for both. There is nothing that indicates the function should not exist.
Even the papers the machine builder delivered with the machine has tables with cylindrical interpolation listed as an option.

Any other suggestions?

[angelw]

Originally Posted by Lene Madsen Thanks for your response Bill. I have checked operators manual, controller manual and my appendices for both. There is nothing that indicates the function should not exist. Even the papers the machine builder delivered with the machine has tables with cylindrical interpolation listed as an option. Any other suggestions?

Lene,
Only a couple of weeks ago I had to organize the installation of cylindrical interpolation on a client's 18i control. There is no reference in the operators manual to G07.1 being an option on this control either, but it is an option and wasn't listed in the spec sheet as being part of the build. The same alarm as you're experiencing was encountered when programming G07.1

One thing you have to be careful of when using a program that includes cylindrical interpolation, is that the function has not been previously activated by programming G07.1 with a cylinder radius specified and then not canceled it with a cylinder Zero radius, this will also give you an alarm. For this reason, its helpful to program G07.1 C0 as part of the call up blocks for the tool involved with the cylindrical interpolation. That was the next problem the client had after the option was turned on.

If the build sheet for your machine indicates that the option is included, contact Fanuc regarding having it turned on; it may have been lost at some point in the life of the machine. If you contact Fanuc or the machine builder, make sure you have the machine's serial number available.

Post the actual alarm number you're getting.

Regards,

Bill

[Lene Madsen]

Thank you for your help Bill.

It turned out that the option was not available with our machine after all, and we will have to try and be creative in order to get our parts done how we want them.

I now have a man investigating what it would take to get this implemented, meanwhile I try to figure out how to program a spiral without having either cylindrical nor polar interpolation available.


/Lene

[angelw]

Originally Posted by Lene Madsen Thank you for your help Bill. It turned out that the option was not available with our machine after all, and we will have to try and be creative in order to get our parts done how we want them. I now have a man investigating what it would take to get this implemented, meanwhile I try to figure out how to program a spiral without having either cylindrical nor polar interpolation available. /Lene

Lene,
Cylindrical interpolation makes possible the programming of circular interpolation on a cylindrical surface quite simple. Basically, you can unwrap the cylindrical surface and program the tool path as if on a flat surface. However, if you only have to machine a helical path you won’t need to have cylindrical interpolation; this process is not very difficult.
Regards,
Bill

[sinha_nsit]

Can use a threading cycle for a helical path with uniform pitch.

[Lene Madsen]

Originally Posted by sinha_nsit Can use a threading cycle for a helical path with uniform pitch.

I can not get it to run with pitch 50 which I need for my spiral without it pushing forward Z at colossal speed.

[angelw]

Originally Posted by Lene Madsen I can not get it to run with pitch 50 which I need for my spiral without it pushing forward Z at colossal speed.

Lene,
From your initial description of what you wanted to achieve "I need to make a helical cut down a Ø10mm steel bar (think twist drill)." I didn't think a threading cycle would be any help to you. However, if its only a helical groove that's required, you will be able to do that with the C and Z axis move without having to have cylindrical interpolation.

Regards,

Bill

[Lene Madsen]

Exactly Bill.

I need Z to push forward, while slowly turning C aswell as using a rotating tool. With a thread cycle this will not function.

I was considering simply coding the coordinates and use G1 and move Z a few hundreds of a milimeter, then C then Z again, but the program would be thousands of blocks and then I would have a memory problem

[angelw]

Originally Posted by Lene Madsen Exactly Bill. I need Z to push forward, while slowly turning C aswell as using a rotating tool. With a thread cycle this will not function. I was considering simply coding the coordinates and use G1 and move Z a few hundreds of a milimeter, then C then Z again, but the program would be thousands of blocks and then I would have a memory problem

Lene,
Correct, a threading cycle will not function in C axis mode.
Is your machine capable of C and Z simultaneously interpolation? This is quite different to having and using the cylindrical interpolation option. If so, once the milling tool is positioned at the X, Z, C start position, try programming C and Z together, ie the angular (C) and Z move to the end of the helix.

Regards,

Bill

[angelw]

Originally Posted by Lene Madsen Exactly Bill. I need Z to push forward, while slowly turning C aswell as using a rotating tool. With a thread cycle this will not function. I was considering simply coding the coordinates and use G1 and move Z a few hundreds of a milimeter, then C then Z again, but the program would be thousands of blocks and then I would have a memory problem

Lene,
Another problem you will have doing it the way you're considering, using many small moves, is that you will not achieve anything near the feed rate that would be reasonable. With a 10T control, I'd expect that you may only achieve a feed rate of maybe 30mm or 40mm per min. maximum, notwithstanding that you program something much higher.

The reason for this is that the motion will actually decelerate to Zero at the end of each move and must try and accelerate up to the programmed speed at the commencement of the next move. However, with very small moves, there will be insufficient length in the move for the motion to reach the programmed speed before having to start the deceleration ramp to the end of the motion block. Accordingly, the motion will reach what velocity it can and that's it.

You can get around the length of the program issue by running the program as a DNC exercise from a PC, but if cycle time is at all important, the feed rate will be an issue.

Regards,

Bill