FANUC CONTROLLER

[ARP]

I've been reading the message board for awhile but never posted anything so this is my first time. I'm wondering if anyone has any suggestions for using G41/G42 cutter comp in the control when using a Fanuc Series O-M contol. I've only been on this machine for about 6 weeks (joined new company) and can't seem to figure out the cutter comp. I was using a Haas and it was clear where to put the cutter diameter value but I can't even find where to put a D value in the Fanuc. Is it in the parameters somewhere? I want to program circles with Mastercam and set the cutter comp to "control" so I can circle mill and adjust the diameter of the cutter to size the bore accordingly. We are using a Dahlih MCV1020B vertical mill with Fanuc O-M controller from 1994. Any help is greatly appreciated

[Tim Johnson]

After chaining the geometry you will go into the tool parameter page. Look for dia. offset and put the number you want there. When you post, the g41/g42 will show on the first go1 x-y line.

[Brendan P]

Welcome to the forum.

Some fanuc controllers do not have the "D" and "H" designated.

Just a bunch of offsets that are numbered.

I would try to put it in offset #50 and use your D50 in your program and see if it works.

[Noel]

If I am not mistaken it will read the d as an h. the diameter values are taken as h in the geometry store so i usualy make the diameter offset for tool 1 h21 tool 2 h22 tool 3 h23 etc.I am also using a dahlih 1020 so it sounds like exactly what i am doing.You can use whatever h value you want i just find it easier to get the opperators in the habit of always having a diameter offset equal to 20 more than the tool #. I beleive if you leave a d value in the program it will look to the h value anyway.

 

 

Hth Noel

[chris m]

Fanuc controls don't have 'H' and 'D' offsets the same way that Haas or Okuma controls do. The offset register merely stores values that can be accessed for either purpose. The typical way to handle this is to use, say H1 for tool #1 and D51 for tool #1. If you use comp in control put the cutter radius value (typically) for T01 in offset 51.

 

C

 

[edit] Noel beat me to the punch [/edit]

[Tim Johnson]

After rereading, are you talking about where to put cc in the machine itself? If so, go to your offset screen, push work, go to the number you want, insert the radius.

 

Note: the length offset (H) and the diameter offset (D) must be different numbers in fanuc "O"

controls

[Tim Johnson]

sorry, instead of work, you want geo (going by memory)

[Noel]

That doent happen very often Chris.

 

 

Noel

[ScottyB]

We have about the same vintage O-M controller. Here's a sample...

 

(T5=30mm cutter)

N105 M341 (VACUUM ON)

N110 G90

N115 S15 M03

N120 M06T5

N130 M13

N140 M11

N145 G56 G0 X-39.7596 Y-15.6174

N150 G64 G43 H5 Z.25

N155 G0 Z.1

N160 G1 Z-.375 F100.

N165 G41 D15 X-39.9752 Y-15.7438 F300.

 

As mentioned, you enter the values associated with H5 and D15 in the offset screen of the controller. The O-M controller is a scaled down Fanuc...but you'll get used to it. I'm guessing you also have the scaled down keyboard that doesn't have all the keys...that's fun.

 

I'm happy to hear of another O-M. I was starting to think they only made 1...ours.

 

Good Luck

[Brendan P]

I ran a new Chevalier(Tiawan made)cnc mill that had a Fanuc OM,and it did have (2) seperate pages with D and H offsets.

[Frank]

I always use WEAR in Mastercam that puts a G41, or G42 and depending on the machine, our Monarchs will only accept cutter comp, when moving a linear move, it won't accept a G41, G42 on an arc, so I have to use the lead in lead out and make sure I have something in there.

[ARP]

Thanks to the "members of the board" for the info. I tried it out and as long as I use the radius value of the cutter being used everything works great. I tried reading the manual but didn't get too far. Next time I have a problem I'm posting on the board and leaving the book in the drawer.

 

Thanks loads!

 

Any idea if I can skip to the D21 offset I'm using (ie: T1, H1, D21) quickly or do I have to cursor to it by page?

[ScottyB]

quote:

---

Any idea if I can skip to the D21 offset I'm using (ie: T1, H1, D21) quickly or do I have to cursor to it by page?

---

Page UP/DOWN??? It should get you there in 3 or 4 clicks...

 

Our Fanuc manual works well as a dust collector. It collects at least .25" of dust every 6 months. I just have the ALARM pages tabbed. I love to see dust on the book...that means everything is running well.

[heeler]

ARP,

 

You should have a Parameter you can change to use a radius value or a diameter value. On the Fanuc 18 it is Parameter 5004 bit 2 ODI "The cutter compensation value is a radius value (0)/diameter value (1). Probably some useless trivia, but feels good to use some of that expensive training that the company sent me to.

 

HTH

Glenn

[heeler]

ARP,

 

Also on the 18 you can enter the offset number say 51 and it will bring up a soft key for # search and when you push it you go right to the offset #. Don't know if it is the same on the O control, but worth a try.

 

HTH

Glenn

[SLJ]

on our fanucs we use wear comp in mastercam, and set "job setup" to add 30 to the tool #. At the machine, just set the offset to "0" till you need to cut more material. Then set the offset for the amount you need to take out. Our param. set for radial, and setting the offset minus tells the control the cutter is undersize, meaning it will move over to take more out of the hole. Clear as mud, right?

Steve