Printable View
Hi,
Mori Seiki TL-5 lathe with a Fanuc 10T-E control, anyone knows how to activate the G54 cordinates? what parameters turn it on/off?
A few days ago I lost all settings/parameters and after 2 days of putting them all back manually I noticed that I not longer able to use the G54 work coordinates. Now Fapt spells out G50 X_ Z_
Thanks for any help
its one of those secret option parameters we're not allowed to talk about.
did you enter the option parameters 9100 to 9131 through the IPL?
If not follow this procedure.....
Fanuc 10 Fanuc 11 Memory Backup Procedures
If you're missing G54 you're probably missing a lot of other stuff that is there as standard.
For example G96 is an option but standard. Even the control panel and manual pulse generator are options.
Do you have separate tool wear offsets and geometry offsets? that's another option parameter but is standard on T series.
also FAPT has its own set of parameters. you can make it output G50's or it can use geometry offsets (no G50 output).
And many other things.
Thanks for your replay,
I did put in parameter(9100-9131) thorug IPL
I also have the Tool wear and Geometry offsets, and everything else that was before seemed to be there except that FATP does not gives me the G54 code when I register the program... as it used to be.
I thought that a FAPT parameter will give me the G54, but I been through all parameters that I have and they all seemed to be ok.
I just don't know how to set the work coordinates, before I used to touch the face of the work set G54 Z_ to that number and I was ready to start machining... now it is not working like that anymore... it gives me a G50X_Z_
before G50 was only for the maximun speed.
------------------------------------------------------
Quote:
Originally Posted by fordav11
ah just G54 is missing in FAPT generated programs only??? or somewhere else as well?
instead of relying on a FAPT number maybe you should set the G54 the correct way.....
can you paste here a small example of how your programs normally look? Then I can look up the required FAPT parameters.
Yes, just the G54 is missing from the generated FAPT program...everything else is fine.
I always been using FAPT, so am having hard time trying to set the G54 the correct way as you said.... I just don't know what the correct way is :(
Am at home right now... but the generated FAPT program starts with the G50 code something like this (as far I can remember):
O0001
G50 X-11. Z6.;
G00 X-11.Z6.;
.........
........
not a G54 at all... before I lost all the parameters there was a G54 at the beggining of the program and the G50 was only used to set the maximum speed .... something like this:
O0001
G50;
G50 S2000;
....
tomorrow I can get more of the "new" code.
Thanks again.
===================================
Quote:
Originally Posted by fordav11
what exactly is in your other working program with G54? a Z value as well or nothing? usually a G54 in the program has no other info with it. the machine reads G54 and reads the workshift number set up previously on the workshift screen
i.e.
G54
G50 S1000
G0 T0202
G96 S100 M3
G00 X10.0 Z0 M8
etc
however I worked several machines with FAPT over the last 25 years (mostly Fanuc 15/16 Mori ZL and SL models) and I've never seen FAPT output a G54. There's nothing in my docs about it either.
There are 2 possibilities and maybe both need to be set.
FAPT parameters relating to this are....
MTF parameter 1060
if bit 0 is 0 then it doesn't output a G50 X Z for each tool (this is what you want.... no G50 X Z output)
so 1060 should be xxxxxxx0 (only change bit 0... the right-most number)
or invert your bit if you have this already. i.e. if your bit 0 is 0 make it 1. if it's 1 make it 0
MTF parameter 1244
this sets the Coordinate System Setting G Code and is defaulted to '50' on my control
Possibly modify it to '54' may get you what you need. But like I said I never saw any FAPT machine output a G54 so your mileage may vary.
also note G54 in the program is usually not required on a lathe as it defaults to that on power-on. If you don't need multiple workshifts you don't need to have a G54 in the program. So stopping the G50 output with parameter 1060 is enough. if you must have it type it into the program manually.
There are many undefined or not-assigned parameters in FAPT depending on the machine tool builder they can be set to something or left at 0 or null. If your machine tool builder modified something you may need to contact them for the correct FAPT parameters.
NOTE! If most/all of your FAPT MTF params are 0 then you lost all of them and will need to set things up again.
If most of them are non-zero then you have not lost your FAPT params and your problem lies elsewhere.
To set the G54 you go to your workshift screen, move the cursor to the G54 Z value. Then touch the face of the part with your setting tool (a tool where the geometry in Z is 0) then type Z0 then press measure. If the face is +2mm (if you want to face off 2mm) then type Z2.0 and press measure
if you don't have a setting tool with 0 in Z geometry then in order to be able to set the workshift the best/correct way to must also set the tools using a similar methodology. The tool setting details are here in post#11
http://www.cnczone.com/forums/fanuc/..._o-t_help.html
once set this way to change to a new part using the same tools just bring the setting tool to touch the face and in the workshift page set G54 Z using Z0 measure as explained above.
Like you posted is the way Fapt would write the program with the G54
before we lost the parameter.
i.e.
G54
G50 S1000
G0 T0202
G96 S100 M3
G00 X10.0 Z0 M8
etc
Now there is not a G54 at all..only a G50 X_Z_ command
Iam on my way to work and I wil lcheck those parameter that you mention(1060 and 1224) hopefully I will get that G54 back :)
I appreciate your help..Thanks!
======================================
QUOTE=fordav11;1047413]what exactly is in your other working program with G54? a Z value as well or nothing? usually a G54 in the program has no other info with it. the machine reads G54 and reads the workshift number set up previously on the workshift screen
i.e.
G54
G50 S1000
G0 T0202
G96 S100 M3
G00 X10.0 Z0 M8
etc
however I worked several machines with FAPT over the last 25 years (mostly Fanuc 15/16 Mori ZL and SL models) and I've never seen FAPT output a G54. There's nothing in my docs about it either.
There are 2 possibilities and maybe both need to be set.
FAPT parameters relating to this are....
MTF parameter 1060
if bit 0 is 0 then it doesn't output a G50 X Z for each tool (this is what you want.... no G50 X Z output)
so 1060 should be xxxxxxx0 (only change bit 0... the right-most number)
or invert your bit if you have this already. i.e. if your bit 0 is 0 make it 1. if it's 1 make it 0
MTF parameter 1244
this sets the Coordinate System Setting G Code and is defaulted to '50' on my control
Possibly modify it to '54' may get you what you need. But like I said I never saw any FAPT machine output a G54 so your mileage may vary.
also note G54 in the program is usually not required on a lthe as it defaults to that on power-on. If you don't need multiple workshifts you don't need to have a G54 in the program. So stopping the G50 output with parameter 1060 is enough. if you must have it type it into the program manually.
There are many undefined or not-assigned parameters in FAPT depending on the machine tool builder they can be set to something or left at 0 or null. If your machine tool builder modified something you may need to contact them for the correct FAPT parameters.
NOTE! If most/all of your FAPT MTF params are 0 then you lost all of them and will need to set things up again.
If most of them are non-zero then you have not lost your FAPT params and your problem lies elsewhere.
To set the G54 you go to your workshift screen, move the cursor to the G54 Z value. Then touch the face of the part with your setting tool (a tool where the geometry in Z is 0) then type Z0 then press measure. If the face is +2mm (if you want to face off 2mm) then type Z2.0 and press measure
if you don't have a setting tool with 0 in Z geometry then in order to be able to set the workshift the best/correct way to must also set the tools using a similar methodology. The tool setting details are here in post#11
http://www.cnczone.com/forums/fanuc/..._o-t_help.html
once set this way to change to a new part using the same tools just bring the setting tool to touch the face and in the workshift page set G54 Z using Z0 measure as explained above.[/QUOTE]
Set parameter 1060 to xxxxxxx1 and got rid of the G50 Z_ X_ now only use the G50 to set the maximun speed(G50 S1000).
Parameter 1224 is set to -1 set it to 1 and also to 0 and nothing seemed to change (-1 is what my parameter sheet calls for).
Notice something else in the System(Configuration) parameters from 9103 to 9131 are "locked parameters" and can't changed them.... am curiors about parameter 9113 which if am not wrong it will turn G54 on/off, right now is set to 0 and my parameter sheet call for 1, how can I unlock those parameters to set them as per my sheet?? ...would that parameter make a difference?
Another thing I noticed, when I zero return the machine, the Absolute reading is whatever is set on my G54 coordinate and the Relative reading is 0on both axis... it used to be the other way around 0 on Absolute.
At this time I can run a program as long I start the proccess right fron the zero return and it will worlk fine as long I don't move the turret on either axis manualy...I mean by this for example, if the proccess stops at the M01 and I move the turret to get it out of the way for whatever the reason, then I must start the next procces again right from zero return... something I never had to do before because the machine would pick up the proper reading from whatever it was moved to...if I don't? the X and/or Z will be off....any ideas why?
These is how FAPT spells the programs now:
G50 S0500 M08;
M41;
G97 S0300 T0101 MO3;
G00 Z0,1;
X-4.94;
G96 S0300;
GO1 Z-15.032 F0.012;
....
....
I add a G54 at the beggining but it does not seemed to do anything.
parameters from 9000 upwards are machine configuration parameters (options).
G54 workshift is just another option. I think on 10 series you need to enter that in the IPL mode (in hex) and also check any others that your machine came with from the factory as per your hard copy parameter sheet. you must enable that to have G54 functionality otherwise a G54 in the program does nothing.
If the IPL mode does not allow it PM me and Ill explain more of the secret stuff that we can't post publicly ;)
I was always under the impression that G54 was not in the options, it was included in the basic package?
I cannot find it in the 10 options or any other control come to that?
Al.
If I enter the parameters on IPL mode... would I lose all the settings/parameters?? and have to start all over again inputing the paramaters including the FAPT?
By inputing the parameters on IPL you mean start the machine pressing 7, 9 and then..if I remember correctly typing 99?... I think after inputing the settings it will ask to clear the files and lose all settings..am I correct?
Thanks!
Quote:
Originally Posted by fordav11
as far as I know yes you have to start again on the older series controls. newer controls you can change any of them much easier (I can't say how publicly).
you can also try something else first before clearing (PM me for the info)
Al, G54 is standard but its still an option and must be turned on if not enabled like in this case
PM sent.
Al.
Hi Fordav..Quote:
Originally Posted by fordav11
Can you tell how in 15tf to save system parameter and mtf parameter after inputing ? I'had initialized the fapt memory beforehand. It's confusing to me as the language is japanese..
awaiting reply
Thanks a lot