[1strokedrs]

Hi I am new here but I have been checking out the boards here for a while and find it very informative.My problem is that I have a Hass VF-1 mill where I work that no matter what work coordinate you give it to read it always uses G54 in Z axis.X and Y axis seems to work fine but it always uses G54 Z axis no matter if you tell it to use G55-G59.
The way we do our set ups is indicate the work in usually an A axis or a chuck or both at the same time in X and Y then we touch off the first tool used in the program on G54-G59 Z(usually the A axis being G54 and the chuck a G55). Then we make sure that the tool length offset for that tool is at zero then touch off the rest of the tools needed in the program on the tool length offset page.
If we use only G54 there is no problem at all but if we use any other work coordinate(G55-G59) the first tool does fine in X,Y and Z but the following tools mess up in Z but do just fine in X and Y.Also if I make the work coordinate Z value zero and touch off on the tool length offset page the tool stops about six inches above the part.
We have another Hass VF-1 that we set up the same way and it is still doing fine and this one has always been fine until the other day I went to do a set up on it and it almost crashed because of this.
Sorry for the long post and I want to say thanks for any help.

[HuFlungDung]

Do you have general parameter #64 set the same on both machines? It says something to the effect "T offset measure uses work". I don't know what the diff is, because I have mine set to off, but from the setting procedure you are describing, it sounds like you might have it on? I never have tool offsets of zero, that's what makes me suspect this difference.

[1strokedrs]

I have tried it on and off with no change.The Z axis stops about six inches above the work if I touch it off on the tool offset page and leave the work coordinate on Z 0.0 either way setting #64 is set.I have tried it both ways.The only thing I can figure is something has gone wrong in the software or the parameters because the machine seems to repeat even though it is in the wrong place in Z and I have never had a problem with this machine in the past.It just all of a sudden started doing this.
Thanks for the help.

[Janos]

Hey there
:wave:

[Janos]

What does A axis have to do with setting up your tool lengths? Do you have a fourth axis on board?
Are you using the "Tool Offset Measure" and "Next Tool" buttons to set your lengths?

[Ken_Shea]

1strokedrs,
This may be a waste of time, however it cost nothing but a small amount of time. I have had strange happnings on my Haas from time to time (although not your problem) as well as wierd PC computor problems over the years and have done this.

Disconnect power, I mean dissconnect, not just shut off, wait 10 minuts and re-connect power. Next thing I've done is unplug and replug all the circut boards. This doesn't always work of course but it has sucessfully fixed problems on several ocasions.

Ken

[HuFlungDung]

1stroke,

If the machine powers up and homes properly, and can change a tool properly without hitting anything or dropping a tool, one would think the Z axis is functional.

If you do a long move bringing the spindle almost down to the table, and then home Z single axis, does it return all the way back up to the top? You should be on the axis displays page (where there are four sets of axis coordinates) to check the positions when this happens.

Have you changed the cadcam software you are using recently? Just wondering if you might have an error in your tool change code, perhaps the wrong G43 H offset number is being called for the subsequent tools?

[1strokedrs]

janos I do have a 4th axis in the machine I am having problems with.I also use the tool offset measure and next tool buttons.
Ken Shea that sounds like something worth trying.
Huflungdung I have not changed a thing.The programs I am running havn't even been removed from the machine since they were last run but I have double checked my tool change codes and G43 H codes anyway.Also the Z does return all the way back up from a long move as this is one of the things I checked first.
One thing I did not think of because I didn't think it would have anything to do with the Z axis is this started to happen the very next day after I replaced the Y axis servo.Also the Y axis seems to work perfectly so this should not effect the Z axis but who knows.

[HuFlungDung]

This would be a long shot, but are you using any G10's or macro programming that might change some of the macro variables? I'm not up on any of that except to guess that modifying some of those in a certain range can perhaps get saved semi-permanently.

What does Haas tech support say?

[1strokedrs]

Huflungdung Hass would not help untill I talked to my local distributer's tech and they said to check the G52 offset to make sure it was at 0 and to try and touch off on the tooloffset page instead of the work offset, but this does not work either. If the work offset is set to o, the Z axis stops about 6 inches before it is supposed to.As for the G10's or macro, we do use some programs with sub programs but I get no change between the ones with a sub and the ones without.The machine is still operable but it is taking a lot longer to do a set up if we use a work coordinate other then a G54.It is getting frustrating because this is a machine that almost every part in the plant has to go through and it has a lot of set ups in a weeks time.

Thanks for everybodys help

[miljnor]

dont forget g92 as being a possible cause for error.

Also just to check if the offsets are realy working but for some reason off. I would set up an alternate offset like g55 (make sure its high for crash purposes ) and then make a simple drill program. See where its stops. then add 2" to the g55 "Z" and see if it moves.

If the start doesn't move then its as you think and probably a factory visit problem. If the start point moves then maybe somethin else at work here. I would go into the settings menu on a machine thats working and make sure EVERYTHING is the same as the broken machine.

That being said your probably screwed and will have to badger the factory into coming and fixing.

Michael t.


ps: if you have a new amp you can switch it to another axis and see if the problem floats to another axis (all the amps are the same) if it does get them to warranty the problem amp (make sure you switch it back so they don't give you grief)

[gar]

051024-1146 EST USA

1strokedrs:

As has been discussed if your tool change works, then it is extremely unlikely, probably impossible, that the Z-axis servo is the problem.

In Fanuc mode tool offset from the specified source is combined with G52 Z and G5X Z to determine the reference for your Z move.

Play with miljnor's experiment.

.

[1strokedrs]

I have done what miljnor has said and the start point does not change but the offset does work.It just always wants to use G54 Z no matter if the program tells it to use G55,G56 or any of the others or even if there is no G54 at all.I have also tried a simple program in MDI and got the same result,X and Y do fine but Z does not work right on the touch off on any tool other then the first tool.Also in the past we have always run both machines in the Yasnac mode but I have tried Fanuc and Hass and got the same result.

Thanks for the help.

[gar]

051024-0853 EST USA

1strokedrs:

Assuming you have the MACROS option you may find it useful to use the #-addresses to read values and change values. You might use DPRINT to output some of these values during program execution.

Work Offsets are at:

G52 #5201-#5205 also called common offset
G54 #5221-#5225
etc.

Tool length offsets are at #2001-#2099 H geometry offsets
Tool length wear are at #2201-#2299 H geometry wear

HAAS has some typo errors in at least one of our manuals on the tool 1 addresses.
#2001, #2201, #2401, and #2601 are the tool 1 locations.

If you have the machine motions stop you can readout location with the following variables:
Present machine coordinate #5020-#5025 HAAS manual might be wrong #5020 maybe should be #5021
Present work coordinate #5041-#5045

We only use the HAAS coordinate system (setting 33). This means that the content of G52 is not reset, not even on power down. To change the value in G52 we have to manually enter the value(s), use G52, or do #5201 = constant or variable to put the constant or content of the variable in G52 X, #5202 for G52 Y, etc.

You should be able to write a small test program like the following to observe what happens if you do not have macros. Maybe it is easier than MACROS:

%
O7000

G53 G0 Z0.0 (make sure Z is home)
G90 (absolute)
G80 M09 (cancel canned cycle, and coolant off)
T01 M06 (select tool 1 and init tool change)
G43 H01 (tool len comp +, len offset 1)
S100 M03 (a low motor speed, start motor)

F100.0 (G01 won't work without a feed specified)

G52 X0 Y0 Z0 (make sure G52 is zeroed)
G54
G01 Z0.0 (should take you to machine position of the content of G54, tool 1 len, and wear)

G52 Z-1.0
G01 Z0.0 (should go 1" lower in Z)

G52 Z0.0 (rezero G52 Z)
G55
G01 Z0.0 (should take you to machine position of the content of G55, tool 1 len, and wear)

G52 Z-1.0
G01 Z0.0 (should go 1" lower in Z)

M00
M30

%

Now use graphics mode, display machine position, display program, and single step the program and record the machine positions.

Let us know what happens. Works on our 1998 VF3. You can make variations in this experiment to test other coordinates, and/or tools. Some others might check for any errors in my experiment.

.

[1strokedrs]

gar what you have suggested is interesting. We have never used G52 in a program in the past so we have always left G52 zeroed.The test program you you wrote is interesting also and I will try it when I get a chance to see what it does.

Here is a short program that I have run in the past with no problems.

%
O1210 (121 CAPS )
T1 M06 (.390 CARBIDE DRILL)
G00 G55 G90 X3.06 Y0. M08
S2300 M03
G43 H01 Z0.125
G04 P1.
G83 Z-0.75 Q0.075 R0.125 F10.
X1.53 Y2.65
X-1.53
X-3.06 Y0.
X-1.53 Y-2.65
X1.3414 Y-2.7503
G80
Z4. M09
M05
M01
T2 M06 (.500 CARBIDE COUNTERSINK)
G00 G55 G90 X3.06 Y0. M08
S550 M03
G43 H02 Z0.125
G81 Z-0.19 R0.125 F6.
X1.53 Y2.65
X-1.53
X-3.06 Y0
X-1.53 Y-2.65
X1.3414 Y-2.7503
G80
G00 Z4. M09
M05
G91 G28 Y0.
M30
%
This will not work now unless I change the G55's to G54 and touch the first tool in Z on G54.

[gar]

051025-0846 EST USA

1strokedrs:

Maybe Z0.125 on the same line as G43 is a problem.

Remove it from the G43 line. Then do this

G43 H01
G00 Z0.0
G00 Z0.125

Now run in the graphics mode displaying machine position and program. See if this corrects the problem. Your code gave me strange results on our machine.

The G00 Z0.0 line is only so you can directly see the results from G55.

A suggestion: put your hole location points in a subroutine, this reduces errors and clutter.

G83 ..........
M97 P500
G80
..
..
..

G81 ..........
M97 P500
G80

..
..
..

N500
X1.53 Y2.65
X-1.53
X-3.06 Y0
X-1.53 Y-2.65
X1.3414 Y-2.7503
M99

..
..

.

[gar]

051025-1043 EST USA

Notes on G52.

If at setting 33 you are not in HAAS mode, then the contents of G52 are automatically reset to 0 on the occurance of certain commands and power on reset. See the HAAS manual.

A way that we set tool offsets, and we always operate the mills in HAAS mode, is:

If the machine has at least one vise, then we use a homemade 1.000" gage block, homemade to make the top surface larger, to set all the tool lengths to 1.000" above the left vise rear jaw. This is effectively the same as using a tool setting probe somewhere on the table. Except with the tool probe the tool length is set relative to the position ZT above the table where the probe triggers.

If we work with no vises and have a large plate, then the 1.000" block is used from the top of the plate. Seldom do we do any castings. In the case of castings we would probably use the table top for the 1.000" block reference.

The reason for the 1.000 block is that it can be quickly slid sideways to test tool position. This avoids accidently jamming the tool into something solid.

We normally use G52 X and Y at zero. Also all Z values in G54 thru Gmax are set to zero. Then the value in G52 Z is used to move the working Z=0 plane up and down for all tools and all G5Xs.

If there is need for a different Z=0 plane relative to each G5X, then we would make changes in the G5X Z values.

The neat thing you can do with G52 Z is to easily move the working plane above your work to do a dry run. Any of the G5Xs can do this also, but if you use multiple G5Xs within a program, then the use of G52 Z applies to all G5Xs.

.

[Geof]

When you are entering tool offsets using TOOL OFFSET MEASUR does the value entered for each tool correspond to the Z POSITION shown at the bottom of the screen. If there is a value in the Z column for G54 it will be subtracted from the Z position when setting 64 (Tool Offset Measure Uses Work Zero) is on.

[gar]

051025-1515 EST USA

Geof:

We always operate with setting 64 off. This means you can easily relate to machine absolute.

.

[1strokedrs]

Gar what I do not understand is why this program ran fine in the past with no problems then all of a sudden one day it will not work unless I change the G55 to G54 and use work coordinate G54 when nothing has been changed in the programs,settings or parameters. I also agree with using sub routines but that one program only uses one work fixture so it is not to bad.Most of the time we use more then one fixture at a time and use sub routines to keep the clutter down.

We also have a super max max-8 mill with fanuc controls that has to be set up similar to what you described but we have always run both of our Hass VF-1's in yasnac mode and touched the first tool in the program off on G54-G59 in the Z column and left that tool offset number zero on the offset screen then touch the rest of the tools off on the offset screen. Also we have tried turning setting 64 on and off with no change in the current condition of the machine.

P.S wouldn't you think if the G43 H01 Z0.125 was messing with it I could just change it to this
G43 H01
Z0.125
Thanks for the help.