Fanuc SYSTEM 5/Mori lathe set-up

[HapSmo19]

Fanuc SYSTEM 5/Mori lathe set-up

This non-crt control is all new to me and not very confidence-inspiring. I'd hate to see system 1 through 4.(not intended to offend the creators of Fanuc systems 1 through 4)

Anyway, I was just thrown at this pile and I'm having a tough time setting tool geometry. Whats left of the manual is virtually useless as far as procedure goes so I was hoping someone here could run through it for me please or refer me to a web site that might relay this info. I will be googling it right after this but for time's sake I thought of here first.

Any help will earn the helper(s) immunity from spell-checking, by me, forever.
And tons of gratitude.

Thanks

[dcoupar]

Here's how I learned. There's other methods, but this should get you started.

Zero return the machine, then index to the tool you want to set.

Take a cut on the OD and record the X machine position (i.e. -10.500) and add it to the diameter you just cut (i.e. 3.000)... this total (13.500) is the G50 X value.

Take a facing cut and record the Z machine position (i.e. -22.000) and add it to the amount of stock left on the face (i.e. 0.030). This total (22.030) is the G50 Z value.

In the program:

G28 U0 W0 (HOME X AND Z)
G00 G97 S250 T0300 M03 (INDEX TO TOOL 3 & START SPINDLE @ 250 RPM)
G50 X13.5 Z22.030 S1200 (SET X/Z OFFSETS & MAX RPM 1200)
X3.1 Z0.1 T0303 (RAPID TO PART & ACTIVATE OFFSET)
G96 S400 (TURN ON CSS @ 400 SFM)
G01 Z0.0 F0.015
X-0.06
G00 X3.0 W0.005
G01 Z-3.0
G00 X3.0
G28 U0 W0 T0300
M01

Repeat for remaining tools. If you don't start and end each tool at machine zero, you should return it to it's starting coordinates. In that case, replace the G28 U0 W0 T0300 with X13.5 Z22.03 T0300 in the above example.

Good luck.

[HapSmo19]

hey dcoupar, check your PM's.

[Dan Fritz]

There is no Fanuc system 4 (or 14, or 24). In Japan, the number "4" is considered unlucky, like our number "13"

The important thing to remember about the Fanuc 5T is that the tool offsets take effect (and the slides MOVE) when you give it the T-code. For example, T0101 selects tool #1 and activates the X, Z, and radius offset #1. T0100 cancels the offset (and the slides move back). Some machines use 4-digit T-codes (first digit = tool number, second digit = offset), but most machines use 4-digit T-codes, where the first 2 digits are the tool number and the last two digits are the offset.

We used to program a G50X---Z--- statement after every tool change, which set the "zero" point for each tool. This compensated for the big differences between the various tools, and let you use tool offset numbers that were very small. Others like to use one G50 statement to set a zero point that is common to all tools, but then you need big numbers in the offset registers. Either way, the job gets done, but I never liked those BIG moves coming from a T-code.

The 5T is a pretty good control, but it is harder to operate than the later 6T because it has no CRT. The biggest problems are:

Batteries go dead, causing loss of parameters. Batteries last about a year. Replace the batteries with the power ON and you won't loose anything.

Molex connectors on power supply overheat, turn brown, and need replacing

Some special Fanuc hybrid IC chips on the main "A" board sometimes get flaky. Fanuc service guys can give you a few.

IC reed relays on the "B" board go bad. These are easy to replace by anyone who can solder ICs.

[Paul Pippenger]

I read most of the problems on here that pertain to the 5T and especially to your replys ,your comment on this matter caught my attention.
i am now having a problem with my control not executing any command from the memory or from MDI.I recently did a lot of solder joint repair on both A and B boards ,now you mention Reed Relays on the b board gettin flaky,
could a relay like that cause the command to not reach the machine side??
Every other aspect of the machine works fine in jog ,no alarms ,just no motion in MDI ,or from memory. i am replacing the PC07 when it gets here but I really dont feel that is it.Its more like the command cant get thru the B board to the machine.
thank for listening
Also I never heard a peep out of anyone about my post on larger offsets for the 5T ,HMMMM.
Peace Paul

[NZ_Jase]

Would the Machine Lock switch result in this problem? I'm pretty sure my ML switch inhibits movement in manual jog/rapid too come to think of it, but there could be diagnostic bits you can quickly check that all the dry run, single block and ml switches are where you think they are when you switch to mdi mode?

Jase.

[Paul Pippenger]

I found the problem ,and posted to the fact under 5T5M sub catagory ,
My machine doesnt have a lock ,but kinda wish i did sometimes LOL.
thanks for you consideration.
Peace P