[joe1970]

Hello fellas,
Iam new to the site and love it...... I recently bought a tong-tai lathe (hatachi-seki off chute) at a bargin basement price. It did not include any manuals. I am having a problem with feed I want to use the standard of inches per rev. but it will only feed in inches per min. even when I use a g99 code. I tried absoulte and incremental (G90 &G91) to see if this has any effect but no good. I can deal with the math to figure out the speeds and feeds but my other lathes will take a G99 and apply it proplerly. I am wondering if anyone out there knows of a parameter setting ?? am missing to something to get this to work properly? I have ran and programed fanuc for years and never ran into this problem maybe someone out there can share some of there wisdom with me??? thank-you

[Al_The_Man]

Does the spindle have an encoder? if not it won't have constant surface feed.
Al

[Factory Guy]

If it has a spindle encoder try G95. Are you trying to use css or just inches per rev? I work mostly with 15, 16, 18, and 21 Fanucs, but I might have some 0-T manuals at work. I'll look Monday.

[joe1970]

the spindle does have an encoder. I tried the G95 contol says the code is invalid.I always use css (unless I am threading or grooving) I think just a G-code list for the O-T control would help if anyone has one there has to be something simple I am missing I always program with a G90,G99 and G96

[CAMCRASH]

I program for a 0T at work
I will copy a G-Code sheet and will try to post it here
The Machine I prigram for is also a Tong-Tai machine
It is a Galaxy version unsure of the modle #
I will also try to look at the parameters and see which one controls the feeds
Tong Tai is great for forgeting books with there machines
The company I work for has one mill and one lathe
The mill came with a operators manual but no parts manual
The lathe came with a parts manual but no operators manual
Neither came with fanuc manuals which is not a big deal but when you are missing multiple it realy sucks to trouble shoot machines

[joe1970]

that would be great camcrash sounds like we have the same machines mine also is a galaxy.(1996)

[MMT]

F riggin
A merican
N o
U nderstand
C hinese

[CAMCRASH]

joe I have not forgot this week started with a lot of fires I have been trying to put out I will try to get this info ASAP

Sorry,

[Factory Guy]

Joe1970,

I sent you an email, but I might be able to post them here. Codes are for a 0T and 0M.

Hope this helps, Daryl

[Factory Guy]

I brought the books home if you need more info.

[joe1970]

thank alot daryl i sent e-mails to the shop and see if they will help I am getting sick of converting fpm to fpr I do about 10 set-ups and programs a day all small runs and this is costing me time and money so your help is greatly appreciated this one has got me perplexed I thought I had seen it all but buy used equipment and live and learn...

[A L]

Can i ask anyone,

When you do G95 for the first time, say with a G01, then type in your XYZ and your Feedrate, for the first time in your code, is that the only time you'll need to use G95?

Or do you need to specify mm/rev (G95) every time that your cutting?

This is for FANUC 6MB controller system...(i don't have access to a machine, its just for a university assignment)...

[dcoupar]

Can i ask anyone,

When you do G95 for the first time, say with a G01, then type in your XYZ and your Feedrate, for the first time in your code, is that the only time you'll need to use G95?

Or do you need to specify mm/rev (G95) every time that your cutting?

This is for FANUC 6MB controller system...(i don't have access to a machine, its just for a university assignment)...

G94 and G95 are "modal", so when you program G95, it puts the control in feed-per-revolution mode, and it remains that way until it reads a G94. So if you always program in G95, put one in the beginning of the program and it will stay active for the entire program.

[beege]

G94 and G95 are "modal", so when you program G95, it puts the control in feed-per-revolution mode, and it remains that way until it reads a G94. So if you always program in G95, put one in the beginning of the program and it will stay active for the entire program.

Also, the default turn-on mode is set by parameter, so you may "turn on" in G95 or in G94 (on my lathe its G98/G99)

[dcoupar]

the spindle does have an encoder. I tried the G95 contol says the code is invalid.I always use css (unless I am threading or grooving) I think just a G-code list for the O-T control would help if anyone has one there has to be something simple I am missing I always program with a G90,G99 and G96

Check parameter 007 bit 5. If it is 0, your control is set for "Standard G Codes", which uses G98 and G99 for FPM and FPR. If it's 1, the control will use "Special G Codes" which uses G94 and G95.

[dcoupar]

Also, the default turn-on mode is set by parameter, so you may "turn on" in G95 or in G94 (on my lathe its G98/G99)

Parameter 007 bit 2 selects which code G94 (G98) or G95 (G99) is active at power up.

[beege]

Thanks for the info dcoupar!

[dcoupar]

Not a problem. That's why we all hang out here!