[WGoyer]

What memoryman (Hi Bill) is alluding to is that reloading a 10 control is, by design, VERY difficult. To quote my instructor when I attended one of the first 10/11 classes at the General Numeric HQ in Elk Grove, "you guys will never figure out our option scheme on this one". He was aware that everyone had figured out the options on the 6 series by then.

Anyway, after you load the options with their cryptic hex scheme, they can be easily checked by just looking at the 9100 series parameters the normal way. If these aren't like your factory list, don't even bother going on.

By the way, Fanuc has nearly perfected the option game now. Now, even the Fanuc employees need to carry a USB dongle that rotates passwords frequently. These units are only good for a few uses before they need to be sent to Japan for re-load. I know one Fanuc employee who accidentally used up three usages by mistake and was asked to write a report stating why his unit came up short.

Warren
Uptime Electronics, Inc.

[memoryman]

Hi Warren.
soonervols: listen carefully.
1: The SYSTEM LABEL is the hardware/software configuration as the control sees it, along with the OPTIONS that must match the physics of the control.
You can get to the IPL menu by holding the - and . keys while turning the control power on. This IPL menu is when the OPTIONS are entered in hexadecimal. Do not bother to proceed without the correct OPTIONS to enter.
If you don't have them, a competent technician can reconstruct them, maybe needing the available OPTION list. As Warren explained, you can verify the entered options once you are out of the IPL menu by looking at the 9100 parameters.

[soonervols]

Yes I understand starting up in the IPL screen and going thru the set up. Using parameters 9100 thru 9116. We had a copy on hand and verified thru Fanuc. Only one number was off from what we had, 9111. Our copy said 0000 0000, Fanucs copy said 0000 0001. Not sure which is correct but plan on using Fanucs copy tomorrow.

I then upload the rest of the NC parameters via a tape machine.

Once I have done this the machine WILL zero out. I then touch off a tool but that tool does not go where I want it to go. I touch that tool off in Work Shift and all remaining tools on Geometry.

[lshingleton]

So you have the machine Zero now ?
What way does the machine want to go on the distance to go screen ?
Behind home ?
Is there any values showing up when you home the machine on the position screen ---------by values i mean in the absolute value ?

On the older controls we used to put a G50 line

G00 G28 WO
G00 G28 UO
G00 G50 X0. Z0. This would cancel out absolute screen
T0100 Calls tool no offset
G00T0101X100.0Z100.0G97S500

Why not touch all tools off in Geo?----work shift very easy lost ?

Other things to try
These older controls had and Absolute incremental switch ---is there one and is in on ?-----------if you cant see it somethimes it was hidden at the end of the Diagnostic screen which would now be the location of Keeprelays on newer controls or if you have the FAPT side it may be in there ?

[soonervols]

Yes it will zero out.

Do you mean when going home or when trying to run a specific tool? As for going home it is not a problem, it goes to the numbers specified in parameter 1220. Which according to the tape is X7.6986 & Z7.0397. As for the tool, X is well above the part and Z is close but still off maybe an inch or so. Don't have exact numbers.

Values will be the numbers set in parameters in 1220 as stated above.

We use G50 as Maintain Upper Spindle Speed. Thats the way I was trained.

As for Work Shift, we use it as a master tool. And when we change to another part I just change Z in which ever direction needed. X never changes and any new tools are touched off in Geometry. Tool 2 being the master tool and its geometry numbers never get changed from 0.

As for a Absolute incremental switch, I am not sure if one exists. We have FAPT but do not use it. Therein lies another question, do I or should I load the FAPT parameters?

[memoryman]

param 9111.0 is custom macro.

[lshingleton]

So home the machine in a program
Goo G28 U0 W0
On your positon screen the machine figures should read zero -what is in the absolute screen ?
Then type in
G00 G30 U0 W0 and does your machine now move to the figures you said of x7.6 and z7.?--------rapid down and move slowly

if it does it means you are touching the tools off from a 2nd referance which is now out becasue the machine positions have moved ?

Have you any previous figures from your master tool in the GEO screen or written down

G50 was used yrs ago for 2 things
G50 S5000 spindle max cap
G50 x0.z0. absolute screen is now zero or tool geo dim/values

In these controls for alot of yrs many yrs ago people put the x and z geo distance to zero in this command line -----because at that time people dint know how to use Geo screens or the machine never came with the option

[soonervols]

With G28 the ABS read X7.5936 & Z19.0087.

G30 would not work, Improper G Code.

I have no other figures written down for anything other than what tapes we have punched for NC parameters, Tool Data, Materail Data, MTF FAPT parameters and NC directory memory.

I use G50 as the spindle max

[lshingleton]

On this control there is a parameter in the first 100 that resets the cordinate system and homing the machine -----i would say for some reason this is not on any more


If this was my machine i would home it
In Mdi mode type in G50 Xo z0 and then go to the position screen
This screen should now read --------Machine pos x0.z0.
Asolute pos x0.z0.
Now touch you first tool off as normal and run it to see where it moves to
Whiout that parameter turned on you may have to cancel the postion every tool at home with the G50 x0.z0. and T0000

Be careful as machines can do nasty things when cordinate system are not working properly -single block and rapid down

[soonervols]

G50 does nothing in MDI.

Now I believe there is up to 3 different code systems, A, B & C. It is in Code A as of now. Had it in a different code and G50 was doing something different than what had been normal for me.

[lshingleton]

Your getting on the right path now
99% of the machines from this era and control were

The 6 or 10 or even the O
The G50 ment 2 things

G50 S2000-----max spindle speed
Goo G50 X0 Z0-------absolute screen equal g50 value



M3s100g97
G00 G50 x5.0 z5.0 -the x and z value was actually your geo for your Tool

[soonervols]

Did the
M3s100g97
G00 G50 x5.0 z5.0

All it did was change the ABS numbers to 5. & 5., the turret did not move and the lights indicating home are still on.

[angelw]

Did the
M3s100g97
G00 G50 x5.0 z5.0

All it did was change the ABS numbers to 5. & 5., the turret did not move and the lights indicating home are still on.

That's all it will do. G50, when applied to an X, and or Z coordinates, set the coordinate system to the values used in the command block.

If you were to follow the G50 X5.0 Z5.0 (the G00 is not required) with G00 X0.0 Z0.0, the tool would move 5.0 units (inches or mm, depending on the whether in G20 or G21 mode respectively) in X (diameter) and Z in a minus direction.

You have to be very careful when using G50 to set the coordinate system. Irrespective of where the slides are positioned, the above example G50 command block will set the Absolute position of the machine to the values used in the command block. Accordingly, its important that this command is made from the same, repeatable position each time its executed.

You've seen that the Absolute position can be set at X5.0 Z5.0 with the slides at the Reference Return position. And commanding G00 X0.0 Z0.0, with no workpiece in place will probably be a safe move. However, if you were to move the tool to, say, 4.0" from the face of the chuck in Z, and execute the following blocks:

G50 X5.0 Z5.0
G00 X0.0 Z0.0

the tool would hit the chuck 4.0" into a 5.0" Z move.

Your machine at one time would have had a workable Geometry Offset Programming and Work Shift system. To revert back to using G50 to set the coordinate system for the tools is a retrograde step, and is tantamount to having a dog and barking yourself.

Take whatever steps that are required to regain the use of the Geometry and Work Shift system of your control and follow the advice given by Memoryman and Warren.

Regards,

Bill

[soonervols]

That is what I am trying to figure out. To get the machine back to where it was but having difficulty figuring out how.

G50 was never used for work coordinates.

Parameters 9100-9116 are correct per the tape, print out and print out sent by Fanuc/Victor.

Everytime I touch the tool off in Geometry or Work Shift the tool is above the part to high in X and tries to go beyond the collets in Z.

How do I correct this? Parameter 1220, work shift or geometry?

Sorry if I am making this more difficult than it needs to be

[angelw]

That is what I am trying to figure out. To get the machine back to where it was but having difficulty figuring out how.

G50 was never used for work coordinates.

Parameters 9100-9116 are correct per the tape, print out and print out sent by Fanuc/Victor.

Everytime I touch the tool off in Geometry or Work Shift the tool is above the part to high in X and tries to go beyond the collets in Z.

How do I correct this? Parameter 1220, work shift or geometry?

Sorry if I am making this more difficult than it needs to be

This parameter is normally set automatically by an input signal from as an external data input.

Whats set in this parameter of your machine currently? If there is a value set, note it and set to Zero. Cycle the power and see if the value is reset to the original value. If there is no value, set any value and again cycle the power to see its reset to Zero or vacant.

The above will give you a clue as to whether the parameter is being reset automatically as how it should be; albeit with the wrong value. If this is the case, you may be missing come PMC parameters. Memoryman may be able to help out in this regard.

If the parameter is not being Reset when the power is cycled, you could add your own value to correct the Work Coordinate System.

Regards,

Bill

[soonervols]

The numbers for parameter is X7.6987 & Z7.0387. These numbers came from the NC parameter tape we loaded into the machine after doing the clearing the memory thru IPL screen.

The numbers are the same after cycling the power, whether it's those numbers or zero.

I have tried correcting the numbers but it does not improve machine position.

I can run the same few lines and get a different stopping point each time. It does not repeat.

As for PMC parameters I have the same ones that Fanuc/Victor does.

[lshingleton]

Send the machine home
Type in
Goo G50 xo.o zo.o in MDI
All this will do is cancel the absolute screen/or set to zero
Before the machine can be setup these screens have to be empty
Mahine x and z=zero
Absolute x and z=zero
Now move your machine down and touch off as normal in the workshift and geometrics
All i am trying to tell you is how to get past the parameter or settings that are not there now
()
This is where alot of machines crashed in the old days becasue people never paid atenshion to these screens and dependant how the machine builder or the parameters had been set up to cancel the Tool offsetts and machine corodinate system
()
Now adays they all come standard or about 99% to do it for you

Program example
O1000(MACHINE PRORGAM 1990)
GOO G28 WO
GOO G28 UO
G00 G90 G40 G80 G50 XO.ZO.S2000
T0100(TOOL ONE OD)
GOO X10.0 Z5.0 G97 S100 M3 T0101
G0 Z1.0 F.008 M8
G00 Z5.0
GOO G28 WO U0 M5
()
(TOOL 2 ID)
GOO G28 WO
GOO G28 UO
G00 G90 G40 G80 G50 XO.ZO.S2000
T0200
()
GOO X10.0 Z5.0 G97 S100 M3 T0202
G0 Z1.0 F.008 M8
G00 Z5.0
GOO G28 WO U0 M5
()
M30



This becomes the start up block for each tool and should remain the same whatever works on this machine
GOO G28 WO
GOO G28 UO
G00 G90 G40 G80 G50 XO.ZO.S2000
T0200


Thios become the end block and should reamin the same for each tool
G00 Z5.0----safe retract from the part
GOO G28 WO U0 M5


Hope the helps or hope yu can get the original settings from some where

[angelw]

The numbers for parameter is X7.6987 & Z7.0387. These numbers came from the NC parameter tape we loaded into the machine after doing the clearing the memory thru IPL screen.

The numbers are the same after cycling the power, whether it's those numbers or zero.

I have tried correcting the numbers but it does not improve machine position.

I can run the same few lines and get a different stopping point each time. It does not repeat.

As for PMC parameters I have the same ones that Fanuc/Victor does.

Disregarding whether the tool is going to the correct position just for the moment, are you saying that if the following code is executed a number of times, that the physical position of the tool after the G00 G54 X0.0 Y0.0 block completes, varies from cycle to cycle? If so, I believe that is a different problem to a Machine Coordinate System issue.

%
O0001
G28 U0.0 W0.0
T0101
G00 G54 X0.0 Y0.0
M00
G28 U0.0 W0.0
M30
%

If the position of the slides (tool) is consistent from cycle to cycle, then you should be able to compensate for the error in the Machine Zero Point by modifying the value in parameter #1220. Of course, I'd only do this as a work around until you determined the reason for the error.

Parameter #1220 is the External Work Coordinate System parameter, and is an offset from the Machine Zero Point. All Work Shift Offsets (G54 to G59 - standard set) will offset from this External Offset.

1. When you perform a Manual Reference Return, does the Machine Position Display read X0 Z0?
2. If you bring a boring bar holder to spindle center line (using a dial indicator off of the main spindle to position the bore of the holder) and
i. Use the Machine Display Value as the X Geometry Offset for that tool.
ii. Reference Return the X slide
iii. Via program or MDI, execute the following command
G54 (make sure there is a X0.0 value in G54)
T0101 (or whatever the tool number is for this tool - make sure there is a Zero value registered in the Wear Offset of this tool - applicable if Tool Offset Memory B is set)
G00 X0.0
does the center line of the tool holder coincide with the Main Spindle center line?

If not, you should be able to put value of the error between Main Spindle center line and boring bar holder center line into the X component of parameter #1220. (This should also be available as the G53 offset in the Work Shift Offset page)

Using G50 to set the Coordinate System of the machine locks you into having to start the machine from a consistent position, as G28 U0.0 W0.0 will achieve before executing the G50 block, and it takes away much of the flexibility available with this control when using the Geometry and Work Shift Offset system.

Regards,

Bill

[lshingleton]

If the stuff me or Bill has told you doesnt work try going after the Absolute incrmetal switch -------Ask victor where it is on the dia screen if it doesnt have a switch -------last thing i can think of could cause it -----------The stuff i wrote for you is not the fastest but is the last resort to getting this machine running
Good Luck

[soonervols]

Good morning and Happy Monday

After running my program Saturday and not getting it to repeat, I came in this morning and tried Bill's program. Here is the results.....

Parameter 1220 @ X7.6986 Z7.0387, which is also the readings on Work Shift, also tool as not been touched off to make sure it doesn't crash.

After zeroing machine out manually and rapiding to random point....
Relative position X-.3496 Z-2.0165, ABS 7.2030 Z7.2865, Machine X14.082 Z-159.060

1st G28 line, Relative X-.9040 Z4.2457, ABS X6.6486 Z13.5487 Machine X0 Z0
G54 Relative X-7.5526 Z-9.3030, ABS X0 Z0, Machine X-168.874 Z-344.137
2nd G28 line, same as 1st G28 line.

Repeated 3 times and got same numbers all 3 times.

Started from zero for next run...
G28 Relative X-.9040 Z4.2457, ABS X7.6986 Z7.0387,Machine X0 Z0
G54 Relative X-8.6026 Z-2.7930 ABS X0 Z0, Machine X-195.544 Z-178.783
G28 Same as 1st G28

Repeated couple times same numbers

Zero out and random rapid move...

ABS numbers changed on 1st G28 from X6.6486 Z13.5487 to X6.0186 Z11.6587

G54 changed from Relative X-7.5526 Z-9.3030 to X-6.9226 Z-7.4130and Machine from X-168.874 Z-344.137 to X-152.872 Z-296.131

Thanks to everyone for their help so far!!