Fanuc G07.1 cylindrical interpolation.

Can anyone please give me an example how they start G07.1 off? I keep getting G code error. I've never written a cylindrical interpolation before and I'm just having a play around. This is for fanuc 18i Puma Y 2500. Cheers.

Pauly123321 said:

Can anyone please give me an example how they start G07.1 off? I keep getting G code error. I've never written a cylindrical interpolation before and I'm just having a play around. This is for fanuc 18i Puma Y 2500. Cheers.

Click to expand...

Hello Pauly,
Its helpful if you supply the actual error code, but I suspect that its a p/s010 error. That being so, you control is not equipped with the Cylindrical Interpolation option.

Regards,

Bill

Thanks bill I'll try and get the error number. We have used G07 before but I can't find the program number in the system and the manual says it's capable of cylindrical interpolation. I'm wondering if I have to change the perimeters or whether I'm just writing it out wrong. The maths side of it looks easy but the manual doesn't show how to lay it out.

Pauly123321 said:

Thanks bill I'll try and get the error number. We have used G07 before but I can't find the program number in the system and the manual says it's capable of cylindrical interpolation. I'm wondering if I have to change the perimeters or whether I'm just writing it out wrong. The maths side of it looks easy but the manual doesn't show how to lay it out.

Click to expand...

Hello Pauly,
Post a copy of your program that is raising the error and at what point the error occurs.

Regards,

Bill

Will do bill. It's as soon as it reads G07.1 it alarms out. I've tried G7 G07 always alarms out on that line. It maybe a couple days before I get on there again as I'm running the mills. No turning to do

Pauly123321 said:

Will do bill. It's as soon as it reads G07.1 it alarms out. I've tried G7 G07 always alarms out on that line. It maybe a couple days before I get on there again as I'm running the mills. No turning to do

Click to expand...

Hello Pauly,
G7 and G07 will definitely not work to execute Cylindrical Interpolation. G07 has an entirely different function. G07.1, or G107 are the only codes that can be used. Depending on the error code you're experiencing, but if the error occurs when G07.1 is executed, its more than likely the case stated in my first Post, that being your control doesn't have the Cylindrical Interpolation option.

Regards,

Bill

Ok cheers bill. I managed to do that two start thread thread today M24X3
G0 X25 Z10
G76 P011000 Q250 R.05
G76 X20.3 Z-35 P1800 Q250 F6.
G0 Z7
G76 P011000 Q250 R.05
G76 X20.3 Z-35 P1800 Q250 F6.
M98 P9006
M1
Came out perfect Thank you.

But you were asking about cylindrical interpolation?!

Incidentally, same Q in both the blocks does not serve the intended purpose of gradually reducing DOC.

Yeah bill was helping me out from another question I had a few days back, and yes it does. First line Q is the size of each incremental cut and the Q in the second line Is the depth of the very first cut you start the canned cycle from. I've only been programming a year what does one mean by DOC?

I may of misread, what's DOC?

Pauly123321 said:

what's DOC?

Click to expand...

Depth of Cut....

Brent

Oh thank you Brent. I'm still not hip with the lingo I never thought I'd enjoy cnc programming as I'm a manual turner of 20 years but loving it

We first learn arithmetic, then start using calculator.
Similarly, if one does not know manual machining, how would he know what to do on a CNC machine.
You have the necessary pre-requisite to learn CNC programming. Some reading habit is all you need.
And, Fanuc manuals are not so bad as many people believe.

You'll be amazed how many people skip the manual side and go straight for cnc. Most cnc turners I know have never touched a manual lathe but gone straight to cnc turning. I'm glad I've done it the way I have. Now I got the best of both worlds.

Pauly123321 said:

Yeah bill was helping me out from another question I had a few days back, and yes it does. First line Q is the size of each incremental cut and the Q in the second line Is the depth of the very first cut you start the canned cycle from. I've only been programming a year what does one mean by DOC?

Click to expand...

Hello Pauly,
The big advantage of the G76 Multi-repetitive cycle is that each Threading pass takes the same volume of material resulting in a relatively constant tool loading. This is accomplished by the control doing the calculations. The algorithm used is:

DOC = SQR(N) x FD

Where:
DOC = Depth Of Cut from the Major Diameter of Thread (External Thread example)
N = The Nth number of the Threading Pass
FD = First DOC as specified by Q in the second G76 Block.

If you were to divide any number by 2 with the aim of getting to Zero, then the aim will never be achieved. Likewise, using the above algorithm will never get to the Minor Diameter (External Thread example) as specified by X in the second G76 Block. The difference between the DOC (DOC from the Major Diameter - External Thread example) of the previous Thread pass and the DOC of the current pass will get to sub Least Programmable Increments and eventually, the diameter of the Threading Pass will get to be within a Least Programmable Increment of the target X diameter, specified in the second G76 Block, at which point the control will see the two diameters being the same and the Threading Cycle will be at an end. However, many unnecessary threading passes will result, the DOC of many being so small that rubbing of the tool will result.

To circumvent the above, a Minimum DOC (difference between the Previous and the Current Threading Pass) is set in first G76 Block. Accordingly, as Sinha correctly points out, setting the Q address of both the first and second G76 Block to the same value will result in the DOC for all Threading passes to be made using the value set in the first G76 Block. The Threading Cycle will function and the Threading operation will be completed, but you loose the advantage of having a similar tool load applied throughout most of the Threading Cycle.

Regards,

Bill

thank you bill. I never realized how deep programming got. It'll be a few years before I start understanding everything on the Puma Y