Fanuc OM Tool Change Height parameter

[samstain]

Does anyone know what parameter number sets the tool change height with a fanuc OM controller (YCM 3 axis mill).

I lost all my parameters when I had a comms fault. I have since managed to fix the fault and reset the origins etc so that it now all fires up ok without any overtravel alarms etc.

But when I tell it to go to the Z home the spindle is not aligned with the ATC arm. I am assuming there is a parameter somewhere that defines a offset from Z Home to go to when doing a tool change?

[angelw]

Originally Posted by samstain Does anyone know what parameter number sets the tool change height with a fanuc OM controller (YCM 3 axis mill). I lost all my parameters when I had a comms fault. I have since managed to fix the fault and reset the origins etc so that it now all fires up ok without any overtravel alarms etc. But when I tell it to go to the Z home the spindle is not aligned with the ATC arm. I am assuming there is a parameter somewhere that defines a offset from Z Home to go to when doing a tool change?

More likely than not, your machine will tool change via a Custom Macro program. In this, the tool change position is made by executing G30, 2nd reference point command. G30 is defined as a distance away from the Machine Zero, and for an OM control this is set in parameter #0737.

If the machine does use G30 for the tool change position, following is a procedure for determining the correct value to set for Z G30.

1. Place a tool holder in the tool change mechanism.

2. Using a height gauge, or similar measuring instrument, measure from the table to the underside of the the tool change ring, or other convenient to measure to face of the tool holder, and note the measurement.

3. Perform a manual Zero Return operation, or execute G91 G28 Z0.0 via MDI.

4. Place the same tool used in 1 and 2 above in the spindle and repeat the measurement procedure to the same face as described in 2 above.

5. Calculate the difference and direction of difference between the the dimensions obtained in 2 and 4. This value is then stored in parameter #0737.

6. After carrying out the above, executing G91 G30 X0.0 will position the tool at the correct height for tool change.

Regards,

Bill

[tc429]

if its usually changing tools AT home, adjust grid offset at parameter 510, if it usually moves up a few inches from home, some use the g30 position(param 737 i think)

[tc429]

oops, simultaneous typing

[samstain]

Thanks Bill, that process to calculate the offset required makes sence. is the value entered in 1/1000's of a mm? ie if I calculate it is 4.35mm do I enter 00043500?

Here is a bit of code from an old program with a tool change - it does appear to use G28

%
O7001
N1G17G80G40
G54
S3000M3
G90G0X12.7Y-5.6
G43Z80.H2
M8
Z5.
G81G98X12.7Y-5.6Z-1.R5.F200.
G80
M9T10
G91G28Z0.
M5
M6
N2G17G80
G54
S3000M3
G90G0X12.7Y-5.6
G43Z80.H10
M8

Does the value in N0737 then get stored somewhere else? I happen to have a print out of my old parameters, and also the parameters that are currently in there (coppied from an identical machine). Both 737 and 510 = 00000000 in both machines. Should I be expecting to see a non zero number in one of these if it is an offset?

511, 512 and 515 are different though - is there somewhere I can download a list of what each parameter is (or at least the commonly changed ones).

[angelw]

Originally Posted by samstain Thanks Bill, that process to calculate the offset required makes sence. is the value entered in 1/1000's of a mm? ie if I calculate it is 4.35mm do I enter 00043500? Here is a bit of code from an old program with a tool change - it does appear to use G28 % O7001 N1G17G80G40 G54 S3000M3 G90G0X12.7Y-5.6 G43Z80.H2 M8 Z5. G81G98X12.7Y-5.6Z-1.R5.F200. G80 M9T10 G91G28Z0. M5 M6 N2G17G80 G54 S3000M3 G90G0X12.7Y-5.6 G43Z80.H10 M8 Does the value in N0737 then get stored somewhere else? I happen to have a print out of my old parameters, and also the parameters that are currently in there (coppied from an identical machine). Both 737 and 510 = 00000000 in both machines. Should I be expecting to see a non zero number in one of these if it is an offset? 511, 512 and 515 are different though - is there somewhere I can download a list of what each parameter is (or at least the commonly changed ones).

Although your part program has a G28 therein, it does not necessarily mean that G30 is not used in a Custom Macro program.

Normally you can determine if a Custom Macro program is being used and called by M6 by looking for the value 6 registered in any of the parameters #0230 through to #0239. These parameters link respectively to programs O9020 through to O9029. But given that the parameters have been lost and replaced with parameter setting that appear to be different to the originals, then its dubious that any of the parameters #0230 through to #0239 will tell you anything.

First up you need to determine if your control is equipped with the User Macro function. The easiest way is to look for a Macro Variable page accessible via the Offset Key, then Soft Keys at the bottom of the screen. If the control has User Macro, you should find a Soft Key labeled MACRO to access the Macro Variable page.

If the control does have the User Macro option, look to see if there are programs registered under any on the program numbers O9020 through to O9029. If yes, and if you're not able to determine if its a Tool Change program, post it here so the Forum can assist you.

Whether G28 or G30 is used may or may not be irrelevant, and depends on the type of tool changer, carousel (tools hanging down pointing towards the table), or side mounted on the machine. At the end of the day, its usually a proximity switch that will confirm for the PMC (PLC program) that the spindle is in position for a tool change. How it got to that position can be irrelevant. Many Carousel Type tool change mechanisms use G30 to raise the spindle clear of the tool after the tool change mechanism has grabbed the spindle tool, hence the reason for possibly both G28 and G30 being used in the tool change sequence.

Grid shift for the Z axis and therefore the G28 position is parameter #0510. Accordingly, if G28 is used to gain the correct tool change position in Z, then the same procedure for obtaining the amount to set for G30 can be used to obtain the value to alter parameter #0510 by.

The value set for G30 in #0737 will be applied + or - from the Zero Return or G28 position.

The setting range in #0737 is 0 to + or - 99999999 in units of 0.001 and 0.0001 for mm and inch respectively. Accordingly 4.35mm would be registered as 4350

Post more information regarding the tool changer type and what you find with regards to the program numbers referred to above.

It could be also that you machine does not use a Custom Macro program. It depend greatly on the the PMC program used, and how much of the Tool Change work is executed by it.

Regards,



Bill

[tc429]

does the tool arm usually grab the tool at home, or does the z slide usually go up past home?

if it grabs AT 'home', adjust parameter 510 to fudge the home position a little as needed. there can be more to switch/encoder/offset when considering grid offset, but as your machine was ok before, simply fudging the parameter should put it back with everything else still in proper adjustment.

grid offset values can be goofy- its in detect units, but cmr/dmr/hires encoders all screw with the ratios...home it up, put a indicator on it, put -100 in 510, cycle power/home it up see what it moves...most smaller machines will move 1:1 in least command increments, so it should move .1mm - but if its got a odd screw or high res, it might move .5 or 1~2mm... note grid offset is only used to fine-tune home position within one rev of the screw...so if toolchange is not at home, dont mess with it...

a lot of our carousel style machines grab at home like that, then theres a incremental move up(or a G30 +3~4") in the TC program to raise the slide so the carousel can index under the spindle to the next tool, then back to g28 for the clamping of the new tool...

random access arm type atcs usually are aligned at home with parameter 510 also, but the slide dont need a g30 as the arm pulls the tool clear...slide just sits at home the whole atc cycle...

hope everyone has a great Thanksgiving
Tim