[Sump Cleaner]

Hey Guys,

I need to orientate the spindle on some mills for a job. One has a Fanuc 16i control, the other an 18i. The thing is I need to orientate it a different angles and I'm not sure haw to do this. Has anyone done this before?

Thanks,

JK

[Willydke]

Parameter 4077

[Mitsui Seiki]

This might work.
M19 S900 for 90 degrees.S1800 for 180 degrees,S670 for 67 degrees........
S is the angle.It works on some Fanuc controls.

[Sump Cleaner]

Thanks Mitsui Seiki,

I tried this out but it only orientates the spindle and then changes the speed value. Too bad it wasen't this simple on this control.

So short of writing a macro which changes the value of the #4077 parameter and then back again, is there any other simple ways of doing this?

Thanks Guys,

JK

[GEM]

Spoke to our programmer today, says he thinks Fanuc can only use the M19 position as normal.

GEM

[codyst]

You could do it with G10. I also have a macro here somewhere that lets you actually do an M19S# without writing to the actual parameter. I'll dig it up when I get home from work.

G10L50;
N4077R(SETTING VALUE);
G11;
M19;

[Sump Cleaner]

Codyst,

Thanks a million. If you can find it and send it to me that would be great!

Thanks again,

JK

[Mitsui Seiki]

Thanks Mitsui Seiki,

I tried this out but it only orientates the spindle and then changes the speed value. Too bad it wasen't this simple on this control.

So short of writing a macro which changes the value of the #4077 parameter and then back again, is there any other simple ways of doing this?

Thanks Guys,

JK

Ok, I have been doing some digging.Try M190P180 for 180 degrees.

This is what the Fanuc 18i manual says.
M190 = Orient Tool to angle required .
M190 : Spindle orientation
Execution of the M5/M3/M4 command or pressing the RESET key will release the
spindle orientation command.

[Sump Cleaner]

Thanks Mitsui Seki,

All of the machines are running gight now so I will try this out when the operators are on lunch.

Any luck finding the macro Codyst?

JK

[codyst]

It's on my work laptop. I've got one more customer to drop by, and will post when I get back to the house.

[codyst]

dug it up, but I had forgotten that I had to make some ladder edits to make it work. Explanation is below. If you're interested I could walk you through doing the edits required to make it work, but a G10 would probably be a lot easier.

O9020(MACRO FOR M119 S.....)

#5=0

#5=#19*11.3777

#1133=#5

#1100=1

M219

M19

#1100=0

G04X0.0

M99

Basically what I did was add some logic so that I could fire M119S*** to position to an angle. M119 would jump to the sub, from there I would set local variable #5 to 0, then set it equal to the value of S(#19)X the value of one pulse of the encoder(4096/360=11.377). Set #1133 equal to the new value. Set #1100=1 (ON), and this bit turns on in the ladder, fire M219, which writes the value from #1133 into a window read function and fire M19, which orients to this value. It will only orient to a specific angle when the value from #1133 is moved into the window read. I can orient to an angle, and follow it up with an M19 and go back to the original position because I'm basically just telling the PMC to look around the setting it actually wants.

[Sump Cleaner]

Codyst,

Would you mind? I think the effort would be worth it. This is going to be used on a 6 spindle transfer machine so the more bullet proof the better.

I get the concept but you lost me at the #1113 & #1100. I've never used those registers before. I take it I have to set #6080 to 119 for the M code to work and then it will pick up your macro? But the ladder stuff is pretty far over my head.

Thanks again,

JK

[codyst]

You're right about setting your 6080 to 119 for the macro. I sent you a PM with my email address. If you can, make a backup of the machine ladders you would like to be able to do this on and email them to me.