mori seiki sl-3a with fanuc 6t

so we got this machine without and manuals or programs on it actually got it wired up hit the main switch on the side then the power button on the pendant...... NOT READY... so after pressing amost every button on there we had a call a tech out to check it out. after a couple hours of him digging through the elec cabinet we call up the previous owners of the machine and it was just an additional button that we had to press then it was ready!! not sure if something is wrong with the machine itself or just the programming or maybe my offsets.. this is whats going on: a move from home position to the spindle is a positive number in the machine cords. (which is unlike our mazak and ameri seiki w/ fanuc ot-c).... so i set my offsets as a positive x and negative z... and when i go to start my program at a T0404 it indexs to tool 4 then immediately rapids to x0 z0... could this be from a G0 T0404 ??? switching into mdi mode to call up a tool or start the spindle i would type the code and on a ot-c hit input then output/start, the fanuc 6t that the mori seiki has the buttons input and start close by so i figured it would be similar, but nope guess not...
also i haven't found multiple offset pages, only one set for 1-16 tools x,z,t,r no wear page...

any help would be greatly appreciated!
thanks

So your machine was switched to a X- machine. Thats parameters and a little wiring. That was common is the really old days of that machine, early lathes were x-, so machines of that vintage were switched to use existing programs. The secondary button to start the machine is normal, any Mori service guy worth his salt should have known that. Think it was even labeled Cont or something like that. Not sure on the rapid to Zero after a tool change, sounds like an offset issue. As far as wear offsets, I'm pretty sure it was an option on later 6 controls, not available on early 6 controls. There is probably 10 years difference in the 6 VS the 0, so things will be a lot different.

any idea what parameters need to be changed?

Quote:

---

Originally Posted by cmo

so we got this machine without and manuals or programs on it actually got it wired up hit the main switch on the side then the power button on the pendant...... NOT READY... so after pressing amost every button on there we had a call a tech out to check it out. after a couple hours of him digging through the elec cabinet we call up the previous owners of the machine and it was just an additional button that we had to press then it was ready!! not sure if something is wrong with the machine itself or just the programming or maybe my offsets.. this is whats going on: a move from home position to the spindle is a positive number in the machine cords. (which is unlike our mazak and ameri seiki w/ fanuc ot-c).... so i set my offsets as a positive x and negative z... and when i go to start my program at a T0404 it indexs to tool 4 then immediately rapids to x0 z0... could this be from a G0 T0404 ??? switching into mdi mode to call up a tool or start the spindle i would type the code and on a ot-c hit input then output/start, the fanuc 6t that the mori seiki has the buttons input and start close by so i figured it would be similar, but nope guess not...
also i haven't found multiple offset pages, only one set for 1-16 tools x,z,t,r no wear page...

any help would be greatly appreciated!
thanks

---

Fanuc 6T Series were produced in two basic models, A and B, with some minor version changes to these basic models.

The major difference between the two models was that the program was able to be viewed with the B model as a whole page when in Auto Mode, whilst the A model, only the current and next block was viewable. Some of the very early 6TA controls did not have a CRT screen, but these were in the minority.

With regards to operation in MDI mode, execution of the command was made by pressing either Output, or Cycle Start; this was dependent on a parameter setting.

With regards to offsets, what you have described is all there was with the 6T control, A or B. With the machining Center control, Work Shift offsets were introduced in the 6MB control.

When executing a tool change in the form of tool number and offset, for example T0101, the slides will move by the amount registered in the offset file corresponding for that tool. This can be hazardous if the offset is relatively large. If G00 was not model when the tool change was being exercised, the command will not be completed due to the slides not being able to move the Offset amount. I believe this was the case for all 6T controls, I haven't seen one that was different to how I've described it. The better way to make the tool change is to call the tool without the offset, T0100, then apply the offset in the next move block, for example, G00 X100.00 Z10.000 T0101. This produced a seamless application of the offset without the slides moving during the actual index of the turret. The offset is canceled in a similar manner by programming the tool with out the offset on the move line back to the tool change position, for example, G00 X300.000 Z300.000 T0100.

The 6T did not have geometry offsets and Coordinate Position Set was achieved using the Coordinate Set command G50. G50 has a dual purpose, clamping the maximum spindle speed when programmed with an S value, and Coordinate Set when used in conjunction with X or Z, or both X and Z. When used to set the Coordinate System, the G50 has to be commanded with the slides at an easily repeatable position. In many cases the Zero Return position for X and Z was used, or an incremental distance away from the Zero Return position. The coordinates set by the G50 represented the distance the tool is from the Work Zero in X and Z. Particularly when used with the control in metric mode, it is good practice to use the integer component of the actual distance the tool is from X0.0 Z0.0 as the G50 command in the program, and the remainder in the Offset Registry. In this way the offset was relatively small and a whole number was used in the program.

Regards,

Bill

Quote:

---

Originally Posted by cmo

so we got this machine without and manuals or programs on it actually got it wired up hit the main switch on the side then the power button on the pendant...... NOT READY... so after pressing amost every button on there we had a call a tech out to check it out. after a couple hours of him digging through the elec cabinet we call up the previous owners of the machine and it was just an additional button that we had to press then it was ready!! not sure if something is wrong with the machine itself or just the programming or maybe my offsets.. this is whats going on: a move from home position to the spindle is a positive number in the machine cords. (which is unlike our mazak and ameri seiki w/ fanuc ot-c).... so i set my offsets as a positive x and negative z... and when i go to start my program at a T0404 it indexs to tool 4 then immediately rapids to x0 z0... could this be from a G0 T0404 ??? switching into mdi mode to call up a tool or start the spindle i would type the code and on a ot-c hit input then output/start, the fanuc 6t that the mori seiki has the buttons input and start close by so i figured it would be similar, but nope guess not...
also i haven't found multiple offset pages, only one set for 1-16 tools x,z,t,r no wear page...

any help would be greatly appreciated!
thanks

---

OK -

When firing up an older Fanuc it's usually "three buttons on - three buttons off". So..
Main power on
CNC power on
Control on
(ready to go)

Emerg stop (or control off on some)
CNC off
Main off
(good night)

Many Mori's way back when were "X-" machines. That meant that every X move on a diameter was X-.. and an "X" command would wreck a tool. They changed that sometime around 1990. The vast majority of these machines were converted to a more conventional format. Every so often tho...one of these comes up that was never converted, usually from a one owner machine out of its original shop.

There is no "wear" offset on a 6. That first appeared on the System 10 in 1984.

Check your parameters. On many 6's, calling a tool and the offset automatically triggers a move to 0,0 that can be stopped but I'm not sure which parameter it is. Manuals are on ebay a lot cheaper than from Mori/Fanuc.

well what i've come up with so far is this
O1234
G20 (inch programming)
G50 X-5.234 Z15.345 T0400 (changes to tool 4 and sets absolute position)
T0404 (<-- not sure if this is necessary?? maybe loads the "offset" which i believe would be the wear amount??)
now i think what is next is to change the x's in the program to negatives and hopefully should be good to go..
and ending with a G28 U0. W0.
but still would like to change the machine parameters to not be all negatives

Quote:

---

Originally Posted by cmo

well what i've come up with so far is this
O1234
G20 (inch programming)
G50 X-5.234 Z15.345 T0400 (changes to tool 4 and sets absolute position)
T0404 (<-- not sure if this is necessary?? maybe loads the "offset" which i believe would be the wear amount??)
now i think what is next is to change the x's in the program to negatives and hopefully should be good to go..
and ending with a G28 U0. W0.
but still would like to change the machine parameters to not be all negatives

---

With regards to the program format when using G50 coordinate set, its imperative that you cancel the tool offset as you send the tool back to the tool change location. Not doing so will result in a gradual shift of the coordinate set position equal to tool offset every time the tool is returned home. The G28 U0 W0 will get you back to the Zero Return position, but once there, if you then cancel the current offset the slides will move away from Zero Return by the offset amount. Accordingly, when the G50 for the next tool is commanded, it will occur with the slides not at Zero Return.

Given that you've used G28 U0 W0 at the end of the machining process for the current tool to go home, the assumption is then that the Zero Return position is being used as the tool change location. That being the case the better format is as follows:

O1234
G20
G28 U0.0 W0.0
G50 T0400 S3000 (CALL TOOL WITHOUT OFFSET AND CLAMP MAX SPINDLE SPEED)
G50 X-5.234 Z15.345
G96 S--- M03
G00 X----- Z------ T0404 M08
-------
-------
-------
-------
-------
-------
G28 U0.0 W0.0 T0400 M09
M01

Regards,

Bill

well i was able to upload a program off a laptop to the machine but i can't figure out how to start a new program right on the machine?? tried inputing in mdi an O1234 but that didn't work. have the same problem with a ameri seiki with fanuc ot-c

Quote:

---

Originally Posted by cmo

well i was able to upload a program off a laptop to the machine but i can't figure out how to start a new program right on the machine?? tried inputing in mdi an O1234 but that didn't work. have the same problem with a ameri seiki with fanuc ot-c

---

1. Select EDIT mode
2. Press the Program button to ensure the Edit screen is selected
3. Press O then the program number, eg O1234
4. Press INSERT.

A new program should now be started, with O and the program displayed at the top of an otherwise blank screen.

Depending on the model of series 6 control you have (A or B) you may be only able to insert one word at a time. The type B control allowed multiple words to be written and then inserted. Each block is terminated by an EOB.

Regards,

Bill

anyone have the parameters for a mori seiki sl 3a with fanuc 6t just had to replace the main board and now the parameters need tweeking, first the zero return was not correct, tech kinda fixed that one, but a
M42
G97 S1200 M3
line of code gets alarm error light number 2
and
M41
G97 S100 M3
the spindle actual rpm was over 1000..