Fanuc 6T Basic Setup Process

Fanuc 6T Basic Setup Process Help Needed

Howdy Everyone,

I'm trying to teach myself how to operate a 1980's vintage Okuma NC4PS running a Fanuc 6T A control and a Traub bar feed. This machine was running production until it was replaced with a newer unit. I'm running BobCad 26 and am perfectly comfortable designing parts, toolpaths and generating the G code. However, I can't seem to wrap my head around initially setting up the machine and importing and running the program. I'm sure I am simply missing a few basic procedures but, honestly, after searching the web and reading both the Fanuc and Okuma manuals I am more confused. In following some of the basic procedures I am able to power up the machine and home it to the initial start position via G28 U0.0 W0.0 when the dial is set to MDI mode. Loading up the tools in their turret positions is simple enough. However, I am perplexed with the task of setting appropriate tool offsets and then importing and running a simple program. Here's where I'm at:

I power up the machine, flip the dial to "MDI" enter "G28" "Input" "W0.0" "Input" "U0.0" "Input". hit "Start" and the machine heads to home.

Once the machine is homed I press "POS" hit "X" then "Origin" and "Y" then "Origin". The display then shows "Relative", "Absolute", "Machine" and "Distance To Go" all at "0.0000".

I call up my primary facing / turning tool (in position 1 on the turret.. .this tool will probably never be taken out of the turret) via typing "T0100" and hitting "Input" followed by "Start".

I then flip the dial to manual I power up the chuck and using the jog lever I skim cut the dia of a bit of aluminum bar stock, stop the chuck and measure the diameter at .9880". The X axis reads -5.0860

Using the jog stick again I take a facing cut of the same aluminum stock and note the location of the Z axis at -5.3287

It is at this point where I no longer know what to do. I'd like to get this machine up and running a couple very simple parts that I have ready to go in BobCad.

Manually I've made this part literally thousands of times. It's a pin turned from 6061 AL with a major diameter of .98" and a length of 2.05". This pin also has a base that is .748" dia with a length of .75". Machining this part manually I would face the stock and use a center drill to slightly dimple the end. The chuck would be stopped, the stock advanced and the tailstock would then be brought up to support the material and the entire pin and base would be turned to diameter and parted off.... pretty basic.

Though the plan (eventually) is to load a full bar of stock into the bar feeder and follow the machining strategy listed below, right now I'd just settle for getting the machine to simply turn the part without messing around with the bar feed, tailstock and parting.

Face
Center drill
Stop chuck and open jaws
Dwell long enough for the bar feed to advance the material to the live center in the tailstock
Clamp chuck and restart
Turn the OD of the pin
Part the pin to length
Repeat the above procedure


So the questions are as follows....

How do I set the tools offsets so the machine knows there the cutting tip of each tool in the turret is located?

Once this is accomplished How do I set the machine to receive the program from my PC through the RS232 port?

Here goes.

The 6T has tool offsets. It also has a G50 that can be used as a tool offset, or a geometry offset.

I prefer to use the G50 as a work offset, even thought the 6T purists will tell you not to do it this way. The there are a few catches to my method as I will explain later.

So, on my machine, this is how I do a setup. I home it out as you have described. Then I call up T1. That is my master tool. Other tools are set from that tool for Z. Diameter is different.

So, I touch off T1 to something like the chuck face. Then I zero the DRO (press Z, then "origin"). Then I jog out and switch to the next tool. I touch it off the same way. The number in the DRO for Z is the tool offset for that tool for Z. Enter it in the offset page. T1 should be set to 0. If the tool is longer than T1, the number is positive.

To get the diameter, you can do a skim cut as you describe. After taking the cut, press X and "origin" again. Then home the X axis. Take the number in the DRO for X, and add to it the diameter of the cut you made. That is the X offset. Enter it in the Offset page. The trick is that the number should always be a negative. Every tool gets a diameter offset.

Now, we need to set the G50 for our geometry. Load your part. Call up T1 again. Touch off to the face of the part or wherever zero will be. Then home the machine in Z. That number is used in the G50 line in the program as a geometry offset.

In the program, you need a G50 line before you do any cutting. It should be something like G50 X0.0 Z10.54 S2000. This sets the Z offset (X is always zero on a lathe) and limits the spindle RPM.

Then to call the tools, you need to do it in 3 steps.
1) Call the tool - T0200. This calls the tool up, but does not apply the offset.
2) Apply the offset in your first move - G0 X3.0 Z1.0 T0202. On the 6T, the machine will move when the tool offset is applied. You can make than move seamless by applying the offset in your first rapid move.
3) Cancel the tool offset. When you are done cutting, send the machine home G28 U0. W0., and then cancel the tool offset T0200.

You cannot skip any of those steps.

The draw backs of this method are: The G50 line has to be read any time you want to run the program. The machine forgets it as soon as the program ends or you reset. So, to restart the program in the middle, you have to read the G50 line before you skip ahead to the tool you want. Also, the negative numbers in the X offsets will mess with the constant surface speed. When you send the machine home, it will ramp up to max diameter. That won't hurt anything, but it is opposite of what you expect to happen.

Some other warnings for all 6T machines: Always start the program from the home position. These machines are dumb and don't know where they are without going home first. Program restarts have to be done with caution. Always cancel the tool offsets. The control will start adding them together if you don't clear them out when you change tools.

That's about it. The 6T can do all the things you really need. Canned cycles, threading, sub programs, etc.

Thanks!

I think I'm starting to understand the setup. I'll have to play around with the code exported in BobCad/Predator to see how it handles the G50 command.

In looking at my display, the "Relative", "Absolute" and "To Go" axis are listed in inches (xx.xxxx) while the "Machine" axis displays in mm (xxx.xxx). Is there a way to change this to inches? Or is it even necessary to do so?

How are you setting up your control to receive a program through the RS232 input?

Machine is always in mm. It makes no difference.

Does your machine have an RS232 port? I just made up a standard cable and plugged it in. To transfer, you just send from the computer, then go to edit and type the O and the program number, then hit "read". Sending out is pretty much the same except you use "punch".

Yup, I've got a cable that plugs into the back of the machine. Of course, it uses a parallel port on the PC side. Off to get a USB to parallel adaptor now....

In looking at the tool offsets the factory had, they were all quite small (-.125, 1.34, -.57) etc... Mine are all much larger. I know it's all relative, but there has to be a way of just setting the offsets and not having to use a G50. This is the code I generated for my pin. It's really just a basic test at slow speed to make sure everything works.

(BEGIN PREDATOR NC HEADER)
(MCH_FILE=LATHE.MCH)
(LTOOL T0101 M0100 S1 O30. I.25 A55 C.0156 H0. D0. N1)
(SCYL S3 X0 Y0 Z-3.2 D1. L3.25)
(HCYL S3 X0 Y0 Z-3.2 D0. L3.25)
(END PREDATOR NC HEADER)

O100
(JOB 1 Face Basic Finish )
(TOOL #1 Kennametal Top Notch )
G20 G40 G99 G0
(REQUIRED ENVIRONMENT STRING)
M41
G28 U0 W0
G50 X0.0 Z0.0
N1 G50 (XDATA,ZDATA)
T0101
G0 G97 S500 M03
( START SPINDLE S500 RPM)
G50 S1000
G0 X1.5 Z.25 M08
G96 S500
G1 X1. Z0. F.015
X0.
X-.25
G0 Z5.
X10.
M09

(JOB 1 Turn Rough )
(TOOL #1 Kennametal Top Notch )
G0 X1.2 Z0. M08
G96 S500
G0 X.9
G1 Z-.74 F.015
X.9437
G3 X1. Z-.7681 R.0286
G1 Z-2.8
G0 Z0.
X.8
G1 Z-.74
X.9
G0 Z0.
X.7425
G1 X.7518 Z-.0063
G3 X.768 Z-.0304 R.0405
G1 Z-.74
X.8
G0 X.968
Z-.6956
G1 X.768
G3 X.7221 Z-.7211 R.0257
G1 X.7094 Z-.722
G2 X.7168 Z-.74 R.0094
G1 X.768
G0 X10.
Z5.
M09

(JOB 1 Turn Basic Finish )
(TOOL #1 Kennametal Top Notch )
G0 X1.2 Z0. M08
G96 S500
G0 X.6885
G3 X.7467 Z-.026 R.031 F.015
G1 X.748 Z-.1489
Z-.513
X.7479 Z-.6892
G3 X.7432 Z-.7038 R.026
G1 X.6943 Z-.7462
G2 X.7145 Z-.7497 R.0166
G1 X.9432 Z-.7499
G3 X.9695 Z-.7558 R.0264
G1 X.9772 Z-.7624
X.9792 Z-.7659
X.9799 Z-.78
X.9796 Z-2.8
G0 X10.
Z5.
M09
M30

You need the G50. They were probably using a different G50 line for each tool. That way they can use the tool offset page like wear offsets. I think that way is a pain in the ass.

I don't know if the USB converters work with RS232. I have always made my own cable using the RS232 on one end, and serial on the other. It's getting harder to find computers with serial ports. You only actually use 4 or 5 of the wires, so it's easy to splice one up.

The 6T can load comments, but you can't use any lowercase letters. You have 3 G50 lines. You can do it all in one.

For your cable configuration

25 pin CNC 2-2 PC 9 pin
25 pin CNC 3-3 PC 9 pin
25 pin CNC 7-5 PC 9 pin

25 pin CNC 4-5 (jumper 4 and 5 together)
25 pin CNC 6-8-20 (jumper 6,8 and 20 together)

I recommend a MOXA brand USB to serial port adapter if your computer does not have a native serial port. You'll need some kind of data transfer program. Some CAM software packages come with one. Hyperterm that comes with Windoze will work but is not terribly friendly. Procomm is great but intimidating for a new user to set up. I recently tried DNC4U and initial impression is very good.

ben_smith said:

Yup, I've got a cable that plugs into the back of the machine. Of course, it uses a parallel port on the PC side. Off to get a USB to parallel adaptor now....

Click to expand...

Hi Ben,
Save your money, as a USB to Parallel will not work. The comms connection to your machine needs to an RS232 connection using the Serial Port, not the parallel port. If you're going to uses a USB adapter, it needs to be a USB to Serial. The DB Connector on the end of the USB adapter will be Male. Use the cable pin-out suggested in Vancbiker's Post #7.

As your control is a Model A, the following parameters are set as shown. Series 6 Model B (including level up controls) use different parameters to the Model A.

Parameter
000 bit 5 = 1
002 bit 5 = 1
024 bit 0 = 1 (for 2 stop bits)
025 = 11101111 (4800 Baud Rate)
026 bit 7 = 0

Computer Software settings
Handshake Method = Xon Xoff
Data Bits = 7
Parity Bit = Even
Stop Bits = 2
Baud Rate = 4800 (to match the setting of the control)

Regards,

Bill

Thanks everyone! I did misspeak, though. The input port on the back of the machine is a Honda 20 pin male connector. The cable that came with the machine has a corresponding female Honda 20 pin connector on one end and a 25 pin male connector on the other. This 25 pin connector looks identical to what was used to transfer data to a printer a looooooong time ago. I'll pull the old tape panel off the machine tomorrow to see if it was unhooked and a new board with a BTR was installed. From the limited info I have been able to find online, it wasn't unusual for data for this type of control to be sent via parallel port. At least this is the impression I have gotten. I would assume installing some sort of parallel port into my PC would solve this problem? I built my PC a bit over a year ago and am comfortable working inside it. Of course I installed a flood of USB ports but nothing else.

ben_smith said:

Thanks everyone! I did misspeak, though. The input port on the back of the machine is a Honda 20 pin male connector. The cable that came with the machine has a corresponding female Honda 20 pin connector on one end and a 25 pin male connector on the other. This 25 pin connector looks identical to what was used to transfer data to a printer a looooooong time ago. I'll pull the old tape panel off the machine tomorrow to see if it was unhooked and a new board with a BTR was installed. From the limited info I have been able to find online, it wasn't unusual for data for this type of control to be sent via parallel port. At least this is the impression I have gotten. I would assume installing some sort of parallel port into my PC would solve this problem? I built my PC a bit over a year ago and am comfortable working inside it. Of course I installed a flood of USB ports but nothing else.

Click to expand...

Hi Ben,
Your last Post makes my reply and that of Vancbiker irrelevant. An RS232 is an optional device on the Series 6 Model A but it was seldom not supplied. Mostly it was the very early Series 6 Model A controls, those that didn't have a CRT screen, where the RS232 interface was omitted.

What you're now describing is the 4070 Facit Parallel Punch Interface. Because of the relative abundance of free Editor/Comms software available using RS232 data transfer, you would be better off fitting a BTR (if one is not already fitted) and Send/Receive files via that device using RS232 protocol. The added advantage, although not so much with a Lathe compared with Machining Centre, is that DNC with the control will be possible.

Regards,

Bill

I'll dig into the machine when I am back in the shop later this morning. Aside from manual programming, how would this cable with these connectors have been used in the past to load data into the machine? I assume simply installing a parallel port into my PC wouldn't facilitate data transfer?

Well it looks like the tape drive is still hooked up. Since this is still wired in, I am guessing there isn't a BTR installed? I've attached a few pics of the system. I'm just left wondering how the heck the previous owner used a PC to operate this machine. My impression is that all but the simplest programs would have to of been drip fed from a dedicated PC? So... in light of the images, what would my best option be to avoid having to manually program this machine? I'm running BOBCad V26 and their Predator editor. Ideally, I'd like to be able to load a few dozen programs into the machine and let it run. I could also cable a dedicated PC to this machine to drip feed it as well. I do have a Daewoo VMC arriving shortly running Fanuc OM controls (early 90's vintage). I'm sure these are all basic questions, however I was unable to find many answers through a few online searches. Purchasing newer machinery would have been a much more user-friendly experience, but these machines didn't bust the budget.

I have found there are a few different ways you can handle "G50" in the 6-T. I do it differently than Wes. The G50's in my code always read "0.0". Then I just touch the tools off normally. You have to do the math when touching X though. Position plus the dia. you touch is what goes in the offset register (as a negative value). I find this to be the least confusing method as it is closest to what you may find in a newer machine. I also notice in your picture, It looks like your X direction is normal. My Nakamura came as X+ was towards center, and X- was towards home. I promptly paid somebody to reverse that!!!!

Here is an example of a simple program I run occasionally if you want to get an idea of how the code needs stacked:

O1234
( 001 301 LATHE OPS )
( ROUGH FACE FACE2 )
G28 U0.0 W0.0
G50 X0. Z0. S2500
T0300 (CNMG-431 )
M42
G99
G96 S1000 M03
G00 X4.1688 Z0.3442 T0303 M8
G01 X1.0688 F0.012
Z0.41
G00 X4.45
M05
M9
G28 U0.0 W0.0
G00 T0300
M01

( FINISH BORE BORE2 )
G28 U0.0 W0.0
G50 X0. Z0. S3000
T1000 (3/4 BORING BAR )
M42
G99
G96 S1600 M03
G00 X1.4432 Z0.43 T1010 M8
Z0.0923
G01 X1.1837 Z-0.0374 F0.006
X0.9981 Z0.0554
G00 X0.9654
Z0.43
M05
M9
G28 U0.0 W0.0
T1000
M30

I deleted a whole bunch of moves out of T1 to shorten it up. But you can see what Wes was talking about with the 3 different tool call outs, and the G50 line doing 3 things at once.

Thanks Everyone (again and again!)
I'm still trying to determine the best method of uploading my G Code generated by BobCad/Predator from my PC to the machine and am open to all suggestions. Outside of that, I figure I'll simply input the above code generated by BobCad manually. Another horribly basic question... how do I enter an entire program manually? The fanuc manual lists the procedure for importing a program on tape but nothing for manually inputting all data. In MDI mode I am able to input the appropriate codes to power the spindle, move the axis, open & close the chuck, etc... but in this mode only one line of code can be executed at once. What is the process to input an entire program??

Go to "edit" and type O1000 and press "input". That will create program O1000. You can then start typing. You have to input each command individually. You cannot just type out a whole line.

wheelieking71 said:

I have found there are a few different ways you can handle "G50" in the 6-T. I do it differently than Wes. The G50's in my code always read "0.0". Then I just touch the tools off normally.

Click to expand...

How do you handle moving your program zero? Meaning, if you program from the end of the part, how do you change from a part that is 2" from the chuck to a part that is 3" from the chuck? Wouldn't you have to change all the Z tool offsets?

I use the G50 as much like the G54 as I can. It makes more sense to me that way. My machine also has a movable home switch for the Z. So, I can move it close to the chuck for short parts. I have to reset the G50 values in the program when I do that.

hmmmm... I must be doing something wrong. Dial pointed to "Tape Edit", press "Command" button, page up to "Next Block" appears then type in O1000 and then "Input". Nothing happens. Tried hitting "Program" then O1000 "Input" with no results either.

ewlsey said:

How do you handle moving your program zero? Meaning, if you program from the end of the part, how do you change from a part that is 2" from the chuck to a part that is 3" from the chuck? Wouldn't you have to change all the Z tool offsets?

I use the G50 as much like the G54 as I can. It makes more sense to me that way. My machine also has a movable home switch for the Z. So, I can move it close to the chuck for short parts. I have to reset the G50 values in the program when I do that.

Click to expand...

Yes, I always re-touch Z. It makes more sense to me that way. It is never the same from part to part anyways. And neither are the tools. The CNMG is just about the only constant. G50 in the 6-T is nothing like G54. And how long does it take to touch off a tool anyways? Takes me about 20 seconds per tool. I can do the whole turrets worth of Z in well under 8 minutes.

I am envious of your adjustable Z-home, and distance between centers!!!

I like using the G50. I set all the Z offsets relative to my T1 trigon. Then I just run it down where I want it, zero the Z read out, and home the machine. The number in Z is the number I put in for the G50.

If the parts are a little long or short, I just adjust that G50 number. I've got a few tools that rarely need to change, my trigon, the top notch groove tool, and the laydown threading tool. The drills and bars change a lot.

Must be a peculiarity with the Okuma machine. I need to hit "Insert" to drop the code into the new program. I still need to figure out how to move down to enter a new block of code, though.