G41/G42 compensating to the wrong axis.

[vcutcd]

Hello,

I ran into some problem trying to mill a gearing wheel on my Doosan Puma 5100LMA with Fanuc Oi-F software. The machine consists of 4 axes (X,Z,C1 and C2).
I have a driving tool that is parralel to the Z-axis and i am trying to mill out the gearing teeth.

N6 
G54
M5P11
M35
G28U0
G0Z300T0G40G98 
T02002 
G97S3000M3P12
G28H0
M08
G0X190Z10C0
G1Z-31F1000
G42X168
X168C-5.44 
X141.5C-9.94 
X141.5C-30.06
X168C-34.56
X168C-45.44
X141.5C-49.94
X141.5C-70.06
X168C-74.56
X168C-85.44
X141.5C-89.94
X141.5C-110.06 
X168C-114.56 
X168C-125.44 
X141.5C-129.94 
X141.5C-150.06 
X168C-154.56 
X168C-165.44 
X141.5C-169.94 
X141.5C-190.06 
X168C-194.56 
X168C-205.44 
X141.5C-209.94 
X141.5C-230.06 
X168C-234.56 
X168C-245.44 
X141.5C-249.94 
X141.5C-270.06 
X168C-274.56 
X168C-285.44 
X141.5C-289.94 
X141.5C-310.06 
X168C-315.56 
X168C-325.44 
X141.5C-329.94 
X141.5C-350.06 
X168C-354.56 
X168C-360
G1G40X190
G0Z20

The problem i'm getting with this program is that G41 or G42 compensates it's radius in the Z-axis. On default the machine is using the XZ plane (G18) but whenever i try to use G17 or G19 it is returning an error (Illegal plane select).

Is there something wrong with my code? Or might there be a parameter that is not set right?

 

[Rick Finsta]

You need to call the tool radius compensation type for the tool nose position; the FANUC manuals for your controller specify these.

EDIT: So you know, this is what the "T" column in your tool offsets page is for.

 

[vcutcd]

Thanks for the reply, but as you could see in one of te attachements tool radius compensation type is set to 7. And in the program im calling T02002 which would call tool 2 with offset table 2.

Or am i doing it wrong?

 

[Nerdlinger]

hmmm, I don't do a lot of C-axis "machining" but when I do I would use G12.1/13.1 (polar interpolation/"mill mode") whereby you would program the cut for that gear just like you would in a mill but instead of X...Y... you program X...C... where C is the would-be Y coordinate in a mill. I KNOW cutter comp works there is all but I'm just not sure if there is an "XC" plane select. Hopefully you can figure that out instead of having to rewrite your code. Good luck!

 

[chad883]

I thought end mills are always set to "0" setting. I always have them set for that, but do not program in degrees. I use polar milling.

 

[Rick Finsta]

I'm 99% I always used 0 for live tooling as well, whether radial or axial, and then had to have the actual radius of the tool in the comp table.

I would also use G112/G113 for this if your lathe will do it since you can post out of any CAM pretty easily and copy/paste the code changing Y to C.

Is that a typo "T02002?" I don't know enough to say if that is a proper tool offset call but I thought you only had four digits maximum.

 

[Nerdlinger]

OH one more thing, if you go the G12.1 route I have always had to double the “X” word as if you’re still programming in diameter like in a lathe, even thought you are in “mill mode.” That one’ll gitcha!

 

[SeymourDumore]

Can't help you on the Doosan implementations, but..

Endmills are typically Direction 0 as mentioned earlier.
I am guessing M35 is your C axis connect function.
Did you try to put in G17 before or after the M35?

I have a Y axis machine so it will always allow a G17, but perhaps yours needs to see the C axis first....

 

[vcutcd]

Thanks for the replies guys, ill try to set the tool cutter compensation type to 0/9 first. This drawing is from another company and we only have this to work with so using G12.1 i have to contact my client to give me the polarised dimensions.

ill give it a try. Thank!

 

[Rick Finsta]

You shouldn't need the polarized dimensions - the controller will convert a standard XY Milling path that you'd use on a 3-axis VMC into the polar coordinates for you using the G12.1/G112 polar interpolation. Depending on parameters, it will also set you feed rates correctly from IPM input.

 

[tonymor]

The conversational programming makes a shape like this pretty easy to program also. +1 on setting tool to 0