Must Have HMC Options

[?Mark]

This is what I do:

Place a  precision ring in HMC (top of the tombstone, vise jaws, doesn't matter). Measure the exact diameter, indicate the exact location and write a program for a depth indicator to touch it off at -90 0 an +90 deg (both directions) and then sweep it from +90 to -90 and back. This will tell you if machine is even setup right. No special codes/options needed. If this part is bad, no options are going to fix this. Fanuc has to synchro all the axis prior to using any other options.

 

EDIT:

Program from the center of rotation.

[huskermcdoogle]

37 minutes ago, g huns said:

And my 19696 bit 5 is a 0 but 19746 bit 4 is a 0 on mine. Is that bad?

Humor me and change 19746 bit 4 to 1.  That should make the machine respect the 19696 bit 5 setting.  Not sure why they have both settings but people have struggled with that setting in the past.  However, I don't think this will effect G68.2 whatsoever.

So I would tend to believe you have error in both directions...  When he zeroed the machine to X did he verify X was at zero using a test bar and indicator?  Did he also rezero the machine to reflect the -1200 in Z?  I am assuming you know how to accurately find COR in both directions.

Based on your numbers I am assuming your Z value is wrong by about .065" and you X is off by a smidge more than a .001".  Start by changing 19702 by .065" in either direction, and see if things get better, don't play with your G54 quite yet.  

By the way, are you setting your G54 in COR coordinates, or machine coordinates?  There is a parameter to toggle that, but I don't recall which one it is.  I'd have to dig.

[huskermcdoogle]

17 minutes ago, Mark @ PPG said:

This is what I do:

Place a  precision ring in HMC (top of the tombstone, vise jaws, doesn't matter). Measure the exact diameter, indicate the exact location and write a program for a depth indicator to touch it off at -90 0 an +90 deg (both directions) and then sweep it from +90 to -90 and back. This will tell you if machine is even setup right. No special codes/options needed. If this part is bad, no options are going to fix this. Fanuc has to synchro all the axis prior to using any other options.

This is a good way to check G43.4, but for what you are doing right now, a test bar and indicator will be far faster and easier.  Doing tool plane work you don't need to worry about syncing axes.

[g huns]

1 minute ago, huskermcdoogle said:

When he zeroed the machine to X did he verify X was at zero using a test bar and indicator?  Did he also rezero the machine to reflect the -1200 in Z?  I am assuming you know how to accurately find COR in both directions.

Yes, yes, and probably.

And I have his report of how much he shifted the machine zero. .0024" in X and .0555" in Z. 

[huskermcdoogle]

I am thinking he didn't do his math right on the Z....   Being off .0555" from a nominal metric number sounds fishy to me.  My experience, at least on the old mori's is that you are never off by more than about .005" in either direcction, and that's after about 10 years of maintenance fiddling with the zero's to keep the tool and pallet changers happy.  IMHO, you never move the grid shift unless the grid shift moved....  Usually they don't without a big crash.

Check his COR work, with your indicator, and your testbar.  Remember, if you are zero at 0 and 180 on the side of the bar without moving X, then go to 90, and position the z so the indicator reads 0 your z machine position should be -1200mm plus test bar length plus the radius of the bar.  If it isn't, well it's setup wrong.

But the easy thing to do, would be to just shift 19702 and see if that corrects your problem, if it does, then you need to go about setting grids again, this time properly.  Also remember, changes in Z will likely effect your pallet change.  So verify mechanically that it is working right if you shift the grid to make things nominal again.  Pallet should set down with little to no translational movement.  Just up and down.  If not, then you may need to adjust some things.  Typically, if you nut your grid COR to nominal, unless they have been played with mechanically, or use a reference position for change, everything will be perfect. 

[g huns]

14 minutes ago, huskermcdoogle said:

I am thinking he didn't do his math right on the Z....   

But the easy thing to do, would be to just shift 19702 and see if that corrects your problem, if it does, then you need to go about setting grids again, this time properly...

If he did the math wrong, he did it wrong on both machines. The other one he shifted 1.4762mm, or .0581".

Since we have no test bar, Enshu guy brought one, I'll start tweaking numbers.

Something else that may or may not be a coincidence, the amount we are off, .065", is the exact size gauge pin that fits between our tool holders bottom flange and the spindle face.

[huskermcdoogle]

Not a coincidence,  i take it you are setting lengths from spindle face not from gage length?  If so, his numbers are good and your G54 is what is off.  Adjust your G54 by .065 and see how things fall.  Add .065 to your tool length as well, (if it is measured from spindle face)

[g huns]

2 minutes ago, huskermcdoogle said:

Not a coincidence,  i take it you are setting lengths from spindle face not from gage length?  If so, his numbers are good and your G54 is what is off.  Adjust your G54 by .065 and see how things fall.  Add .065 to your tool length as well, (if it is measured from spindle face)

Yeah, I don't believe in coincidences.

We recently had a Renishaw probe and toolsetter installed one both machines. I don't have a clue where those number come from. I know we had to re-calibrate the probe after the Enshu guy shifted the machine coordinates.

But if we adjust the G54 and tool length, the B0 side will be screwed up, as it's currently right on.

[huskermcdoogle]

G54 and tool length adjustment go together.  So they would cancel.  Then everything should fall in.  

Are you datuming Z to Spindle Face or Gage Line?

[huskermcdoogle]

Z offset will be more negative by .065"

Add .065" to the tool length.

If this works, you should be able to just subtract .065" from 19702 and continue with the tool length and datum setting methods you have been using. (set g54 and length back to from spindle face)

 

[g huns]

5 minutes ago, huskermcdoogle said:

G54 and tool length adjustment go together.  So they would cancel.  Then everything should fall in.  

Are you datuming Z to Spindle Face or Gage Line?

Ah, yeah they would. Duh.

Don't know. Wouldn't that depend on how our probe/toolsetter are set up?

3 minutes ago, huskermcdoogle said:

If this works, you should be able to just subtract .065" from 19702 and continue with the tool length and datum setting methods you have been using. (set g54 and length back to from spindle face)

I'll give that a shot tomorrow. I have apparently used up our operator's supply of cooperation for the day.

[huskermcdoogle]

IMHO, all should be set to gage length.  That way if you picked up an optical or mechanical offline presetter you could calibrate using a test bar.  Tool setter is usually best setup using a calibrated test bar, and the probe calibration surface would be calibrated using a test bar.  Owning a calibrated L/D test bar is a must if you have a horizontal.  It's the only way you will be able to make programs, offsets, and fixtures easily transferable between machines.  By using a test bar you can grid shift the machines to the same nominal COR values, then by setting tool lengths based on G/L they too will be transferable.   Unless it is a dual contact spindle, the spindle face to G/L won't be exactly the same machine to machine.

[g huns]

Wow, this was a long time ago.

Our Cimatron post guy just called me up. He has a customer with shiny new OKK that Fanuc can't make work right after installing TCP and TWP. They've been trying for two weeks.

He said it's like deja vu all over again.

Had to look this up to refresh my memory.

That and I sent him some pics of the parameters we ended up with on our Enshus after Fanuc couldn't help us.

In Fanuc's defense, he did mention that he's went through this process two other times since our debacle and those Fanuc guys had the machines running perfect speedy quick.

[cncappsjames]

I just saw this. Must've been posted during my hiatus.

Interesting conversation.

Myself, I'd have TCP(G43.4) and TWP(G68.2) on an HMC if it were my machine. Dataserver, 1k Block Ahead, Jerk Control,, etc... is assumed and goes without saying. The FAST (Fina & Advanced Surface Technology) package and Aerospace Package for 4 and 5-Axis machines is what I go with.

RTDFO (G54.2)... not so much. It isn't nearly as powerful as G68.2 and requires the use of two offsets (Common/Work Offset and Dynamic Offset) whereas G68.2 and G43.4 only require 1. Of course, you have to set your center of rotation values in Parameters #19700-#19705... but the setup guy doesn't see those and usually they are set and forget unless there is an "incident".

JM2CFWIW.