Need Help!- FANUC 18-M

[PICMAN]

Hello,
I have two machine with the 18-M control. When I call up G55, G56, G57, G58, & G59 and set my ref position, I press reset and the machine defaults back to G54. My other Fanuc does not do this.... Now, if I touch off my tools and press Z input calculate it reads a huge number that will crash my machine. I am having to type in the number instead of using input calc. My other Fanuc does not do this either.... I've looked at the parameters of both machine #1201 to make them the same, but still does not fix the problem. If anyone has a suggestion, I would be grateful.
Thanks,
Picman

[Dan Fritz]

Check parameter 3402, bit 6 (7th bit from the right). It should be "0". A "1" causes the RESET button to clear ALL the G-codes to their power-up state.

[PICMAN]

Do you know about the input calculate function?

[angelw]

Originally Posted by PICMAN Do you know about the input calculate function?

If you're referring to its use in combination with setting G54 to G59, many machines have a Soft Key "Measure". Your machine may have Calculate, if we're talking about the same function. If so, proceed as follows:

1. Access the Work Shift page and position the cursor on the focus Work Shift Offset (G54 - 59)

2. Input the Axis Address and current position of the the Axis. Lets say you have touched off the side of the workpiece in the X Axis and, taking in the radius of the touch off instrument, the X slide is at X-50.123 (mm system) relative to the workpiece X Zero. In this case you would input X-50.123, then Calculate (Measure). The control makes a calculation based on the Machine Position Coordinate and writes the value to the focus X Work Shift Offset.

3. Repeat as in 2 for the other Axes.

Regards,

Bill

[fordav11]

16/18 series has additional functions for tool setting (the CALC for X/Y depends on where your home point is left or right of current position which you should select before pressing CALC) and there are probably parameters used in conjunction with it or at least some reference values are used (it is calculating the length based on another pre-set number)

first what is the reference value in Z? (or post a pic of your workshift page here) and what is the physical tool length of one of your tools, your 'calculated' length for that same tool and your G54 Z value. i.e. more info is required to see where the error is originating.

also if you have a different Z in G55/56/57/58 etc and you are in that coordinate system when you set tools it will affect your tool lengths. The Z reference in the other workshifts should be set to the same Z value as G54 except where you are using specific tools for that other workshift and those tools are set with that workshift active. basically all tools are set in one work coordinate system and the Z workshift will take care of the Z shifts in other work coordinate systems so all tools should be set with only G54 active. That's one of the reasons the leave a certain "What-Reset-Does" parameter alone so you can press reset and kill all workshifts before setting tools.

There are several ways to set tools on a mill (pre-configured lengths or set in the machine to the top of the job or using a setting probe) and that method directly relates to how the machine has been configured with regards to setting tools and the reference method used.

usually a mill will have a fixed length and all tool lengths are set to/from the same position/face. the fixed length is usually the position from the face of the spindle taper at zero return (Z+ maximum) to the table face or center of a chuck/rotary axis set at 90 degrees to the spindle or some other fixed position on the machine. the tool length offset is the difference between that fixed length and the length of the tool extended from the spindle or reference point used in the workshift.

on an old 6M I worked years ago the Z reference was 0 (G92 X-something Y-something Z0) and the tool length offset was the position from home to the face of the part for each tool. If you talked to 10 different machinists working on mills they would likely all give you a different answer on how they set the tools/reference

to summarize, if you set tools and the tool length offset is incorrectly calculated it means your Z reference value is wrong.

[PICMAN]

My ref tool (T1) is always my face tool. I am not reffering to the work shift page but my off-set page. On my other Fanuc control, in my work shift i set Z0 measure, no matter the work shift number (G54 G55 G56....) I always leave my "off-set" value for Z tool (1) 0.000. Once I have my work shift set, I touch my following tool (T2,T3,T4...) When I am on the part, satisfied with the tool touch, I press Z then (below on the soft key says) input calc. When the the number is input it matches exactly what my position reads on the screen. My other control does not react the same way. It calculates a BIG number that does not match. It does the same thing with all of my work shift numbers, so I figured it was a parameter issue

[fordav11]

yeah that's the reference numbers I'm referring to above. most likely maximum stroke in all axis and other similar big numbers.
the calculation would be :
big reference number minus movement of your axis equals smaller number put into geometry or tool length offset. so reference or stroke parameters are wrong?

did it ever work properly? if so has anyone messed with the parameters? If not then your problem could be something else.

assuming it is a parameter issue, you may be able to find the number. you said when you set the tool your position and offset are the same number. if you set a tool on your (bad) machine and calculate the error you should be able to find that 'error amount' number in the parameters?
Maybe? ;-)

Another way... punch all parameters from both machines and compare the files in a PC. it should be clear where the problem is if a large number in a parameter is wrong.

[PICMAN]

I will try that and let you know what I find, by the par 3402 was the fix for my other problem. Thanks Dan......