Fanuc 18-MC with Dataserver and Renishaw issue

[ddanutz]

Hello everybody,

I have to work with a CNC Fanuc system, it is Fanuc 18-MC with
dataserver and connected to a Renishaw toolprobe.
I am not very familiar with CNC Fanuc, and have some difficulties in working with it. Maybe some of you guys can help me:
1. The controller have 3 coordinate system: relative, absolute and machine.
How can i setup absolute values acording to my needs, for example to
put zero on a workpiece? the relative values can be changed, but this doesn't help me much. My gcode partprograms are in absolute coordinates.
2. What is the way to use MDI, or what is MDI in the first place? I want for example to start spindle at a 3000rpm, to input S3000 and M03 and start it, not make a program for it.
3. How can i setup the Renishaw toolprobe coordinates, and what are the items to follow to measure tool-length?

Thank you!
ddanutz

[Ozemale6t9]

1. Move tool to job datum position - Press Tool Offset - Work Offset Softkey - Highlight Work Offset to be used (eg. G54) - Type X0 - Press Measure softkey. This will calculate the current X Axis position as X0. Repeat for Y Axis. It is also possible to set other positions. For example, if you are touching the left side of your job with a 20mm cutter and you want the side of the job to be X datum, you can enter X-10.0 and press Measure softkey and the machine will calculate X0 at the left side of the job. Likewise for Y axis. To calculate Z datum, you need to know the length offset for the tool you are using, or (as most of my customers do) use one tool as a datum tool and have zero offset on that tool. Bring the tool down to touch the datum surface, and type Z? (? = the tool offset) and press Measure softkey. If you need to allow for machining allowance simply add that amount when calculating the Z work offset.

2. MDI is manual data input. Select MDI mode - press PROG key - Press MDI softkey - Type S3000 M03 EOB - Press Insert - Press Cycle Start.

Sorry, can't help you with number 3.

Regards, Oz

[Ozemale6t9]

Also, depending on your parameter settings, the display may not update the Absolute Position display after setting your work zero until the next buffer read. If this is the case, you can force it to update by entering G54 (or whichever you set) in MDI.

regards, Oz

[Skipppi]

About Renishaw probes with Fanuc 18.
It looks like You mean a toolprobe TS27R. Everything depends on software You use for toolsetting. If You use a standard Renishaw software You should find in Your program list in Fanuc controler theses macros:
O9799
O9850
O9852
O9853
Coordinates for toolprobe are automaticaly set-up through calibration proces and stored in macro variables #520 - #531. This is descripted in programming guide for theses macros. Do You have something like this?
regards, Skipppi

[ddanutz]

Oz and Skipppi,

Thank you for your kind reply, this is very helpful.
Yes I have those macros on CNC memory and DataServer. I do not know how, but i succeded measuring a tool, no 2 for example, but when another one come to measure, it stops above the Renishaw probe and outputs Probe fail, or when it comes to low, it says Probe open. Maybe i should deal with parameters a little bit more.
Now i have other problem on my head. I succeded making DataServer work with a PC through FTP. i can transfer partprograms both ways. I registered them in NC memory by calling O****, but guess what?! I have filled the memory of NC, and realised that i cannot delete part programs!!!!
In Edit mode, i write for example O0001, hit [Delete] and [Exec] and i get this error: "FORMAT ERROR". I do not know what to do anymore, i tryed with PWE changing, with shutoff, in Memory mode, but i just cannot delete theese programs registered in memory of NC. Could you please indicate a solution to do that?

Thanks,
ddanutz

[Ozemale6t9]

You need to type O0001 and hit delete key on MDI keypad. I think Delete/EXEC softkeys delete current program in memory without entering program number. Not 100% sure though, as I always use other method.

regards, Oz

[ddanutz]

Thanks Oz,

Ohhhhhhh, it is working !!!!
In Edit mode, under DIR, i enter O0001 and hit the Delete key on the keyboard, and the
part-program is gone! This is something i just didn't try.

Many,many thanks Oz,
ddanutz

[ddanutz]

Here i am again,

1. Renishaw:
Here is my setup:
Renishaw head(the touching zone) is at the following machine coordinates:
X=670; Y=-71.5; Z~-507(this negative Z value is aproximate, measured
from the spindle bottom edge, where it faces toolholder);
I have put a 4mm tool with a total length at about 115mm from the upper edge of toolholder on T2 and 100mm on T1.

I made the following program:
O0001 #520=20.;
#523=670.;
#524=-71.5;
#525=-50.;
#526=20.;
#530=2;(this is because Renishaw orientation, it is located on the upper right corner of the table);
G65 P9853 B1. T2. ;
G65 P9853 B1. T1. ;
M30;
%

Still it says: probe fail! I must say that i enter 520, 525 and 526 values totally random, i do not know what to follow!!
Is this the method of measuring the tools, a program that calls O9853 for every tool, with the values for the variables #520-530 entered on the beginning of the program?
What is actually the way it works?
#520 it is Z calibration value(for nonrotating tools); -> what does it mean?
#521 is it Z calibration value(for rotating tools);
#522 is stylus size for diameter measuring ?!
#523 and 524 seem to be the center of the probe on X and Y respectively;
#525 is Z aproach position; What value should i follow here, is it in machine coordinates?
#526 is Z clearence postion; also, machine coordinates?
#527 tools rotate above this!!
#528 max cutter diameter size
#529 tool offset type.

G54 is working OK. I have positioned the tool on a virtual piece, entered a virtual X-5., hit measure and start a G54 on MDI. Absolute coordinate value for X is now -5. aluminium chips are now much, much close !!

Thank you so much,
ddanutz

[ddanutz]

Oh,

sorry for that, macros of Renishaw deal with all the parameter setup!
I just had to run them one by one, and parameter were automatically updated.

Thanks,
ddanutz

[Skipppi]

Hi ddanutz,
Macro variables #520 to #524 has to be set automaticaly through calibration process, otherwise results of measuring wil be unaccurate.
#525 is applicable just in macro O9853. It is distance from top of the probe styli to the nose of the tool where rapid move stops and "safety" move is used.
#526 again just in macro O9853. It is clearance over stylus, when tool moves around it (let say for diameter measuring).
Nonrotating tools means tolls which You don't have to rotate when You measure length (drill...)
Error messages Probe fail and Probe open means that You put into tool table unmatched approximate length ot the tool (what You have to for automatic measuring).
Can You let mek now some email adress where I can send You a programing manual for toolsetting ?

hope it helps...
cheeers
Skipppi

[ddanutz]

thank you, skipppi,

i have sent you my adress.

Regards,
ddanutz