Fanuc 18i question

[STKSHFTR]

We have used insert tooling on our router for some time and simply posted out using computer comp. More recently, we have begun to use solid carbide and would like to post out using wear, but for the life of me I can't find the info in the Fanuc manuals that describes how to access the proper input screen.

Also, I'm confused as to whether the D value is the cutter diameter or the radius. Any help would be greatly appreciated.

 

Marv

MasterCam Router Pro

ICON Design LLC

[Greg Williams]

Marv,

 

The D value will be a Radius.

This value lives in the offset register next to the coresonding offset number that you have used in the program

EG G41 D2

offset screen number 002 = (Cutter Radius)

If you are going to use wear compensation then this value will be the difference between the programmed radius of the tool and the actual radius of the tool

[Lars Christensen]

I am not a Fanuc guru, but I believe your D offset will be in you offset page as 50 values.

D1 = 51

D2 = 52

 

I believe also believe that it is radius, but that is something that could be changest in a parameter.

 

HTH

Lars

[Lars Christensen]

Hi Greg,

Up early?

There you go Marv, a Fanuc guru.

 

Lars

[STKSHFTR]

Gentlemen,

Thanks! I'll give it go tomorrow.

 

Marv

 

MasterCam Router Pro

ICON Design LLC

[Tom Dorgan from American Precision]

The D value is your amount of offset. If you set your parameter to wear and have the correct tool diameter in your setup then the D value only needs to be the amount you want to adjust the cut size. One thing you have to look out for is to always have a lead in/lead out. If you don't then you will get a lot of errors. Fanuc 18i cannot apply cutter comp on an arc. The way I test my program visually is to look at the line the cutter comp is on and if the G41/G42 is on the same line with a G02/G03 then it will fail every time if there is any comp in the offset table. I will adjust the amount of Lead in/Out until it comes out on a G01 line. Your G41/G42 must be on a G01 straight line move. BTW... We build CNC Routers with the Fanuc 18i control. I always program with comp set to wear.

[Guest CNC Apps Guy 1]

Well it depends on the "Type" of Comp you have. Type "A", "B" or "C".

 

"A" means you essentially have to offset your "D's" H1 & D51, H2 & D52, etc.... or something similar

 

"B" means you have the ability for your H & D's can be the same, H1 and D1, etc...

 

"C" means the same as "B" BUT you have "Wear" Comp for both H and D. So all together for Type C you have an H and Wear COmp for H, a D and Wear Comp for D. C is far superior to the others IMHO.

[crazy^millman]

We use the +20 or +50 for our Fanuc's. I wear but remember Fanuc need some kind of comp line to turn no the comp. If you were cutting the end of a part and you did not have say an arch or tanget move in which the cutter comp would be turned on then Fanuc's will trun the cutter comp on along the whole move to mek the end cut. So if you were applying .01 to the tool for say a reground tool then the edge close to the start would be +.01 and the edge clode the end would be 0 to the desired cut. I have a mr switch in our post to add +50 if anyone needs it but out post defaults +20 to all D'd so no matter what we machine we program for be it a Fadal,Haas, or what ever all you need to do is post the base Mastercam program and you have good code for whatever machine.

 

HTH

[heeler]

One more note, I know that on a Fanuc 18M, and 21i that Parameter # 5004 bit 2 selects " The cutter compensation value is a radius value (set to 0)/ a diameter value (set to 1).

 

So it could be a radius, or diameter depending on this parameter.

 

HTH

Glenn

[STKSHFTR]

Glenn,

 

This may be the bit of info I've been looking for. I can enter H values, but simply haven't found the screen to enter this and D values. A review of the control parameters might help here.

 

Thanks to all. The breadth of knowledge exhibited here and the willingness to help make this place hard to beat.

 

Marv

[crazy^millman]

Ok let me see if I can shed some light on this subject for you. The page that is the tooloffset parameters on a fanuc is all the parameters to the height and dia offsets. So to give you an example if you were to make you H99 and you D1 and say you are running a true cutter comp and it is a .500 dia tool and you have figured out that the Z offset needs to be -13.487 tool then you would put in number 1 offset .500 and in offset 99 you would put -13.487 and you would have the same results in running the program with these offsets H1 and D99 and had them with the coresponding numbers in thiese place and it works fine. A machine like a HAAS, Fadal, Mazak, Okuma, or most non Fanuc's clearly tell you that you height offsets and tool offsets where as on a fanuc you have them all in the same place and have to program your program to make it look to 2 numbers to make the 2 things you need to use height and dia/rad offsets work. Cool thing is that most machines need parameter or things changed to run different D for one tool Fanuc does not and does it very seamless and easy.

 

HTH

[heeler]

STKSHFTR,

 

James Meyette

 

Said

----------------------------------------

"A" means you essentially have to offset your "D's" H1 & D51, H2 & D52, etc.... or something similar

 

"B" means you have the ability for your H & D's can be the same, H1 and D1, etc...

 

"C" means the same as "B" BUT you have "Wear" Comp for both H and D. So all together for Type C you have an H and Wear COmp for H, a D and Wear Comp for D. C is far superior to the others IMHO.

 

-----------------------------------------

 

What this means is that you prolly have an "A" control. Our 21i are this. You only have 1 offset registar, So you have to come up with a "process" of assigning your other offset. We have 99 offsets that we can use on our 21i's. So we chose to add 50 to the radius/dia. offset. In our program you will see a G43Z1.00 H1 to apply the length offset for tool #1 and a G41/G42 X1. Y1. D51 to apply the radius/dia. offset for tool #1

 

 

HTH

 

Glenn

 

P.S. Our 18M are a C control so we have all 4 offsets on one line for offset #1. So we have an H1, and D1 in the code for running on this control.