Fanuc 10T-F chamfer with C command?

tobydbaker74 · Apr 6, 2020

I have a 1985 Dawoo Puma 6s that I finally have up and running. I am trying to get it to chamfer corners or radius and am lost on what I am missing. I have posted what I wrote hoping someone can tell me what I'm missing. In this one I am trying a .01 rad. I found a M code for M76 and M77 for chamfering. I have tried inserting m76 and 77s also with C for chamfering but still cant get it to work. Any help would be greatly appreciated

Sent from my SM-G950U using Tapatalk

Vancbiker · Apr 6, 2020

Chamfer and radius by C and R is an option that may not be active on your machine. What is the content of your parameter 9103? In any case the C or R is preceded by a comma. ie ,R.01

Pretty sure the M codes you listed are for chamfering at the lead out of threading.

Fancuku · Apr 7, 2020

Chamfering with C command is an option. A lot of people don't realize that not all machines were setup the same even though they all have Fanuc controllers. A lot of it depends how much the factory guy and the buyer of the new machine knew at the time of installation/setup.

What is the tool nose radius? If it's the usual .031" then it goes like this

G1 Z0.0
X0.388
G3 X0.47 Z-0.041 R0.041

Omega · Apr 7, 2020

For a chamfer try...

G1Z0F.002
G1 X1.00 C-.01(Make sure there is a G1 and that C value is in direction of travel)

Philabuster · Apr 7, 2020

Not sure why but some Fanuc machines chamfering was designated as K and not C.

Vancbiker · Apr 7, 2020

Philabuster said:
Not sure why but some Fanuc machines chamfering was designated as K and not C.

Don't recall the exact details, but I or K, positive or negative could be used for chamfering. Something to do with major axis and direction. Have to dig out a programming manual and refresh.

barratt · Apr 7, 2020

I think it is I & K for chamfers & R for radii

N10 G00 X200.0 Z3.0
N20 G01 Z0.0 F0.3
N30 Z-30.0 R5.0 (PUTS A 5MM RAD IN THE CORNER.)
N40 X220.0

N10 G00 X200.0 Z3.0
N20 G01 Z0.0 F0.3
N30 X220.0 K-5.0 (PUTS A 5MM CHAMFER ON THE 220 DIA)
N40 Z-40.0

The move with the C or I or K has to be a single axis move.
the move after has to be perpendicular to that move.
The mode has to be G01
There can't be anything between the N30 & N40 blocks, not even a EOB. (I think).

FrankieB · Apr 7, 2020

For the chamfers just trig it. For the radius, g02 or g03 with an R. Don’t for get to double the x values where needed.

Mtndew · Apr 7, 2020

I would say you don't have the option because the line before and after the M77 appear to be fine and would put a .01r on that edge.
C and R work if you have enough movement before and after the command in the direction of the shape.

Vancbiker · Apr 7, 2020

OP went AWOL I guess. Asked for parameter info so I could tell him if he has the option or not. Crickets......

tobydbaker74 · Apr 7, 2020

I wish I went AWOL today. Would be much less stressful. I make parts for fillers, labelers etc etc. for filling sanitizers. I got called in to make several of the we need it yesterday parts. The money is good but still sucks

People without common sense constantly try to speed the lines up. It's hard for some too understand there is a max you can run before sh%$ starts failing and breaking. I say for one month run at 100 bottles a minute. Then run your way at 135 for a month and see which way makes more.

Then back to the lathe. We checked to see it the spindle had run out and it was perfect. Then checked the turret. It was out .430 in the X which I can adjust in the offset I'm guessing but the turret in the Y is out 025. Gotta pull the turret off this one I think. Pretty sure I have to do this to get to the curvic coupler gear and replace the pins. Will know tomorrow when I dig in. I will post pics tomorrow night for anyone else that has the issue with the same turret.

Sent from my SM-G950U using Tapatalk

tobydbaker74 · Apr 7, 2020

Vancbiker said:
OP went AWOL I guess. Asked for parameter info so I could tell him if he has the option or not. Crickets......

I didnt know I had any new post on this till I sat down fo finally eat lunch at 10pm tonight. Some how my notifications for tapatalk got turned off. I will check the oprion parameters tomorrow when I get back in the shop. Thanks for replying this sight has given me a ton of knowledge over the years.

Sent from my SM-G950U using Tapatalk

tobydbaker74 · Apr 8, 2020

Vancbiker said:
Chamfer and radius by C and R is an option that may not be active on your machine. What is the content of your parameter 9103? In any case the C or R is preceded by a comma. ie ,R.01

Pretty sure the M codes you listed are for chamfering at the lead out of threading.

Parameter 9103 is 0 0 0 0 0 1 0 0

Sent from my SM-G950U using Tapatalk

barratt · Apr 8, 2020

Dug out the manual.

Parameter 9103 on our puma 12L with fanuc 10TF is the same as yours
00000100

Vancbiker · Apr 8, 2020

The state of 9103 indicates the option was spec'd on the control.

If you are not using tool nose radius compensation (G41 and G42) then you will need to to add the tool radius (r) to your desired R amount for outside corners and subtract r from R on inside corners For chamfers compensate similarly with .59r to the desired chamfer amount. If you are using G41 and G42 then no adjustment to the R or C values is needed.

tobydbaker74 · Apr 8, 2020

Well hoping the turret is ok we need to find these locator pins for the tool holder. The previous owner has wrecked all 12 at some point. Any idea where to get them?? They are 15mmOD X 12mm long

Sent from my SM-G950U using Tapatalk

TeachMePlease · Apr 8, 2020

tobydbaker74 said:
Well hoping the turret is ok we need to find these locator pins for the tool holder. The previous owner has wrecked all 12 at some point. Any idea where to get them?? They are 15mmOD X 12mm longhttps://uploads.tapatalk-cdn.com/20200408/d2c6b146c757ee80642652430d801497.jpg

Sent from my SM-G950U using Tapatalk[/QUOTE]

Know anybody with a lathe?

tobydbaker74 · Apr 8, 2020

TeachMePlease said:
Know anybody with a lathe?

That made me pee my pants a little In my old age.

Sent from my SM-G950U using Tapatalk

tobydbaker74 · Apr 8, 2020

Ended up having to pull the turret. For anyone that ever needs to pull one of these run 2 bolts and it will come straight off.

Sent from my SM-G950U using Tapatalk

tobydbaker74 · Apr 11, 2020

TeachMePlease said:
Know anybody with a lathe?

Found a lathe!

Sent from my SM-G950U using Tapatalk

Fanuc 10T-F chamfer with C command?

Aluminum

Diamond

Cast Iron

Aluminum

Diamond

Diamond

Aluminum

Aluminum

Diamond

Diamond

Aluminum

Aluminum

Aluminum

Aluminum

Diamond

Aluminum

Diamond

Aluminum

Aluminum

Aluminum

Similar threads