Need Help!- Leadwell, fanuc O-T help!

[Vegabond]

Hello, i just start to learn something about our Cnc lathe....
It is a Leadwell with fanuc O-T...
When i try to set the home position, the axis goes slowly and after some seconds it came an error. Error 090 - P/S Alarm...

What can i do to not get that alarm?

Some tip?


Greetings from Robert.

[memoryman]

p/s alarm 90: REFERENCE RETURN INCOMPLETE
The reference position return cannot be performed normally because the reference position return start point is too close to the reference position or the speed is too slow. Separate the start point far enough from the reference position, or specify a sufficiently fast speed for reference position return. Check the program contents.
Param 534 sets the low speed for all axes in reference return. Try increasing that.

[DouglasR]

Originally Posted by Vegabond Hello, i just start to learn something about our Cnc lathe.... It is a Leadwell with fanuc O-T... When i try to set the home position, the axis goes slowly and after some seconds it came an error. Error 090 - P/S Alarm... What can i do to not get that alarm? Some tip? Greetings from Robert.

I had a Takisawa that did the same thing.
Check the limit switches. Sometimes, dirt, chips, moisture, coolant residue, etc can cripple a limit switch and the Fanuc will not be able to "see" the home position.

[yours_prabhat]

Try to move axis in jog mode at least 70 mm in negative direction - x, - y(in milling machine), and - z Than go for zero return press +X,+Z and +Y((in milling machine), Some times it is required to hold the +x , +z and +Y to complete the reference , The machine will be go to a reference point. If problem persist Please mail on prabhatmishra@gmx.com
Regards
Prabhat Mishra

[stevo1]

Robert,
Did this just start happening? Bill is probably right. Your decel switch is to close to the marker on the encoder. You will have to either slow it down or do a gridshift or move the decel switch. It could also be a rarity that your encoder is shot and it's not seeing the marker. If you have a scope to put on it you can see if the marker is there.

Stevo

[Vegabond]

Hello.

I need to jog long way to the - position... almost so long that the axis will crash

The cnc has not been used for 4-5 years, so im a beginner at this now.

Another question, does the fixture offset change/reset every time i turn off the machine?

When i try to figure out/learn something on the machine yesterday, i just change some x/z values, and the cnc just cut off the hole piece

Any other tip?


Greetings from Robert.

[Vegabond]

Hello again.

Here is some photos. I try to get the U/X aksis in zero when im in senter of the workpiece... How can i do that? im using the probe to...


Im a beginner, so please explain good

Thanks!


Greetings from Robert.

[angelw]

Originally Posted by Vegabond Hello. I need to jog long way to the - position... almost so long that the axis will crash The cnc has not been used for 4-5 years, so im a beginner at this now. Another question, does the fixture offset change/reset every time i turn off the machine? When i try to figure out/learn something on the machine yesterday, i just change some x/z values, and the cnc just cut off the hole piece Any other tip Greetings from Robert.

Robert,
The work shift system for your OT control is not like the work shift of later controls. On your control, Automatic Coordinate System Setting could be made viable by setting parameter #0010.7 to 1. Take a look at that parameter bit just to confirm. With this bit set, the coordinate system is determined at the time when manual reference return is executed. Doing this is the same as executing the following command G50 Xxx Zxx

You will get some unexpected results if the reference return is not made after setting a new work shift, and in particular if manual reference return is not carried out after setting the shift value and before turning the machine off. When the machine is turned back on and a reference return is executed, the coordinate system will revert to the penultimate setting. This situation was, in my opinion, not well explained in the Fanuc manual and I've seen some nasty prangs on client's machines when resuming a program after shut down of the previous day.

Regards,

Bill

[Vegabond]

Hello again.

Is it a parameter that i can change on my machine, i don`t want to write a "point" (?) after example X20. is there a way/parameter that i can change, when i write in X20 and the machine set . after the 0 automaticly.... Bad thing :P


Greetings from Robert.

[angelw]

Originally Posted by Vegabond Hello again. Is it a parameter that i can change on my machine, i don`t want to write a "point" (?) after example X20. is there a way/parameter that i can change, when i write in X20 and the machine set . after the 0 automaticly.... Bad thing :P Greetings from Robert.

Hi Robert,
There is no way that the control will explicitly input a period just by typing the number, but there is a parameter that can be set so that the integer component of a number can be input and the Fanuc control interprets the number as that value. I think from memory, Fanuc describe this as Calculator Form.

Ordinarily, the control will interpret X20 as X0.020 internally (when the control is set to Metric Input). However, when the parameter is set to Calculator Form, X20 will be interpreted as X20.0, but a period will not appear in your program. Any coordinate that is not a whole number still requires the period, that is, X20.5 must still be written as X20.5; X205 in Calculator Form will be interpreted as X205.0. Unfortunately, I’m away from my office and books; accordingly, I can’t help you with the parameter and bit number for a few days. However, if you have the Fanuc Parameter manual for your control you will find it therein without much trouble. Just look for a description relating to Calculator Form, or words similar.

Regards,


Bill

[fordav11]

we had an 0-T piece of crap retro-fitted to an old Mazak Powermaster that had a 3000c on it. No one could figure it out but after some time I found an easy way to set the workshift.

But first.....

you say "I try to get the U/X axis in zero when I'm in center of the workpiece... How can i do that?"

It looks like you have not had any proper training on how to set tools?

if nothing is set do this.....

bring in the first OD tool (we will call it T1), take a clean-up cut on the face. now move up and take a skim off the diameter and move back in Z (dont move X)
physically measure the diameter with micrometer. go to the offset page in GEOMETRY. move the cursor to the tool number currently in position (i.e T1). move the cursor to the Z for T1 and type 0 and [input]. move the cursor to the X for T1. if
the part measured 100.13mm you type X100.13 then press [measure]. The first tool is set and thats the end of it.
Move the same tool back to the face and touch on it. go to workshift in z. type Z0 then press [measure]. the workshift is now set.

Index the next tool and touch the same diameter. cursor to X for that tool (i.e. T2). type X100.13 [measure]. touch the tool on the same front face as before. cursor to the Z for T2 and type Z0 [measure]
repeat for all other tools.


The way I set up the workshift was to put X as 0 and just leave it.
if the tools were set and you had a number in the X workshift just set X workshift to 0 (cursor to workshift X then type 0 and [input]). re-set all tools and the X geometry will be re-calculated and will stay there until physically changed.

Once everything is set the only shift you need to use is Z workshift. Touch your setting tool on the face at Z0, type Z0 and press [measure]. thats all you need to do.
The numbers in 'measure' on the right of the screen should also always be 0

The way I did it was to set Z0 at the face regardless of how much you want to face off the part and set all tools to that same Z0 face also.
Then at the end I measure the length of the part and if there was 1mm on the length I would simply add 1mm to the workshift Z number. i.e. cursor to the Z in workshift, type 1.0 then press [input+]. The Z0 will be set 1mm behind that face.

The O-T is a very basic control, there are no multiple workshifts (no G55, G56, G57 etc) and the measure facility is also not very advanced. Its better to have measure X and Z as 0 and workshift X as 0 and only use the Z workshift so things stay simple. Most tools should be already set once in the machine as the control uses geometry offsets which do not need to be re-set each job (unlike G50's) so all you need to do is adjust the Z0 position for a new job using the workshift function. move the setting tool to Z0 on your part and type Z0 then press [measure]

There are various ways of setting a CNC machine. This is just one way but I found its the easiest way to teach other people :-)

also if you're not doing it already, in your turret there are multiple tools set in the geometry offsets. one tool should have a Z as 0 and is called the 'setting tool'. That is the tool you use to touch on the face when your do the Z0 [measure] thing which will simply shift all of the tools in Z. The other tools are all plus or minus from the setting tool length. The X's are totally independent of each other when the workshift X is set to 0 and do not need to be re-set unless removed and replaced.

Once the geometry offsets are set properly, to go to a new job all you need to do is move the setting tool to Z0 on your part. on the workshift page cursor to workshift Z and type Z0 then press [measure]. After that you can basically just press start

[stevo1]

[QUOTE=Vegabond;989015]Is it a parameter that i can change on my machine, i don`t want to write a "point" (?) after example X20. is there a way/parameter that i can change, when i write in X20 and the machine set . after the 0 automaticly.... Bad thing :P[QUOTE]

I think the parameters you are looking for are either 15.7 or 16.3 see the attached highlighted in yellow.

Stevo