Older Fanuc OM control-feed rates

Hi Guys(and Gals)I'm new to your forum and I have recently purchased my first cnc for private use. I have some machining experience from 20 years ago and am now retired. I think I got a deal on a 1994 Excel 810 VMC with a fanuc O control. This was O.K. by me, that's what I was used to.I was a turning machine man with a little exposure to mills, WOW! what a difference! Sooo....I have been doing o.k. programing so far,but what I can't seem to figure out is why it does not seem to pick up commanded feed rates???????? The only way to control this seems to be manually over riding with jog feed rate selector.....Could this be a parameter problem or am I not getting the G95 and feed rates in the right place? I sure could use some help please/thank you !

Change the G95 to G94
G95 is feed per rev
G94 is feed per min.

Here is a snippet of Om milling code for just a straight line to get you going.

N25 G00 G20 G17 G40 G49 G80 G94


N35 ( FACE FINISH FC1 )
N40 T1 M6
N45 G00 G54 G90 X5.615 Y-1.26 S5820 M03
N50 G43 H1 Z1.05 M08
N55 Z0.15
N60 G01 Z0. F131.0
N65 X-1.575
N70 G00 Z1.05
N75 M5
N80 G91 G28 Z0 M09
N85 G49 G90 X0. Y0.
N90 M30

Welcome to the forum

g-coder05 said:

Change the G95 to G94
G95 is feed per rev
G94 is feed per min.

Here is a snippet of Om milling code for just a straight line to get you going.

N25 G00 G20 G17 G40 G49 G80 G94


N35 ( FACE FINISH FC1 )
N40 T1 M6
N45 G00 G G90 X5.615 Y-1.26 S5820 M03
N50 G43 H1 Z1.05 M08
N55 Z0.15
N60 G01 Z0. F131.0
N65 X-1.575
N70 G00 Z1.05
N75 M5
N80 G91 G28 Z0 M09
N85 G49 G90 X0. Y0.
N90 M30

Welcome to the forum

Click to expand...

Line n45, You have a blank g after g00.

Sent from my SM-G930V using Tapatalk

chip_maker said:

Line n45, You have a blank g after g00.

Sent from my SM-G930V using Tapatalk

Click to expand...

Good catch, I tend to leave the work offset out till I know where i'm puttin them on the table.

g-coder05 said:

Good catch, I tend to leave the work offset out till I know where i'm puttin them on the table.

Click to expand...

Thank you for your replies! I have tried G94 and set feeds accordingly but it still seems to feed at about 5 IPM on any axis. Here is a sample, please correct me if I'm wrong..


N05 G00 G20 G17 G40 G49 G80 G90:
G94 G91 G28Z0.0;
N10 T02 M06;
S1000 M03;
G00 G90 G54 X0.0 Y3.45
G43 H02 Z1.0 M08;
G01 Z.1 F15;
N15 G99 G81 Z-.25 R.1 F4.0
( remaining coordinates for 5 holes )

Could it be as simple as missing the decimal or period after the feedrate? Your second to last line with "F15" needs to have the ".", at least on my OM it has to be there....

Add a decimal point after your feed rate. I see F15, make it F15.

Sent from my SM-G930V using Tapatalk

macgyver said:

Could it be as simple as missing the decimal or period after the feedrate? Your second to last line with "F15" needs to have the ".", at least on my OM it has to be there....

Click to expand...

lol, got me by a minute.

Sent from my SM-G930V using Tapatalk

chip_maker said:

lol, got me by a minute.

Sent from my SM-G930V using Tapatalk

Click to expand...

Sorry, thats just my typing ability. I have not miss placed any decimals or periods. Just got the control manual for this machine and I guess I have some reading to do! Thanks all!

Parabellum said:

Sorry, thats just my typing ability. I have not miss placed any decimals or periods. Just got the control manual for this machine and I guess I have some reading to do! Thanks all!

Click to expand...

Hello Parabellum,
Does the Rapid Moves in your program travel at the Rapid speed when the Rapid Override is at 100%?

Parabellum said:

it does not seem to pick up commanded feed rates????????

Click to expand...

Do you mean by this comment that the actual Feed Rate of the machine is wrong, in that it is way too slow, way to quick and everything in between, depending on the position of the Feed Override, or is it just way too slow irrespective of the position of the Feed Override?

You will find a switch on the control panel that is the Dry Run Switch. Its used to give complete control of both the Rapids and Feed Rates via the Feed Override Switch. Rapid rates can be controlled from Zero to a moderately Fast Feed Rate and Feed Moves controlled from Zero to much faster than the programmed Feed Rate. This mode is used for proving a program at the machine whilst maintaining complete control of the axes motion.

You may have to decipher the hieroglyphics if the control panel switches are identified by icons, rather than Text. If no such switch is found on the control panel, this and other functions can also be set via a Setting Screen of the control; its up to the MTB as to how these functions are implemented.

I've had many clients caught out with the Dry Run Switch over the years; it can be a trap for new players.

Regards,

Bill

Bill, Thank you for taking time to help me out. to answer, yes the rapid moves at the correct speeds per position on the rapid override switch. What I seem to be experiencing is while programming to move at a feed rate of say 2 IPM or slower, the machine just keeps moving G01 2-3, at the same rate which is about 5 IPM near as I can tell by watching the Position screen while running at 100 on the feed over ride. I set a higher Z work offset and have run this several times to confirm. I did not mess with the dry run button much, I tried it once to run in auto but it never lights up. I know I have a lot to learn so I really appreciate any help I get.

Craig

You Sir, are a genius! As it turns out the bulb indicating "Dry Run" is burned out. I now have full control of my feed rates !!!What a relief! Thank You!

Craig