Fanuc OM G54 G55 height issue

[voicurob]

Hello,

I have a machine with fanuc om controller, and when i am trying to use multiple work offsets, it does not work properly.
Specifically when it moves to G55, it keeps the height from G54, (it should go lower). X and Y position are alright in G55.
Any suggestions?

Thank you in advance

 

[GENERALDISARRAY]

Can we see your program?

 

[voicurob]

Sure.
I use fusion 360, and the post preccessor is „fanuc” the one that comes with fusion.
Also, if i export just the G55 part on its own, it work perfect.

(T3 D=5. CR=0. - ZMIN=-21.7 - FLAT END MILL)
(T4 D=8. CR=0. - ZMIN=-21.5 - FLAT END MILL)
G90 G94 G17 G80
G21
G53 G00 Z0.

(SLOT1)
T3 M06
S5800 M03
G54
M08
G00 X-1. Y-20.
G43 Z15. H03
G00 Z5.
G01 Z0.5 F348.
X-82.5 Z-0.887
X-1. Z-2.275
X-82.5 Z-3.662
X-1. Z-5.05
X-82.5 Z-6.438
X-1. Z-7.825
X-82.5 Z-9.212
X-1. Z-10.6
X-82.5 Z-11.988
X-1. Z-13.375
X-82.5 Z-14.762
X-1. Z-16.15
X-82.5 Z-17.538
X-1. Z-18.925
X-82.5 Z-20.313
X-1. Z-21.7
X-82.5
G00 Z15.
G53 G00 Z0.

(SLOT1)
G55
G00 X-1. Y-20.
G43 Z15. H03
G00 Z5.
G01 Z0.5 F348.
X-82.5 Z-0.887
X-1. Z-2.275
X-82.5 Z-3.662
X-1. Z-5.05
X-82.5 Z-6.438
X-1. Z-7.825
X-82.5 Z-9.212
X-1. Z-10.6
X-82.5 Z-11.988
X-1. Z-13.375
X-82.5 Z-14.762
X-1. Z-16.15
X-82.5 Z-17.538
X-1. Z-18.925
X-82.5 Z-20.313
X-1. Z-21.7
X-82.5
G00 Z15.
M05
G53 G00 Z0.

(2D CONTOUR1)
M09
M01
T4 M06
S5570 M03
G54
M08
G00 X-135. Y-45.8
G43 Z15. H04
G00 Z5.
G01 Z-7.2 F557.
G19 G03 Y-45. Z-8. J0.8
G01 Y-40.
Y0.
Y5.
G03 Y5.8 Z-7.2 K0.8
G00 Z5.
Y-45.8
G01 Z-3. F557.
Z-15.2
G03 Y-45. Z-16. J0.8
G01 Y-40.
Y0.
Y5.
G03 Y5.8 Z-15.2 K0.8
G00 Z5.
Y-45.8
G01 Z-11. F557.
Z-20.7
G03 Y-45. Z-21.5 J0.8
G01 Y-40.
Y0.
Y5.
G03 Y5.8 Z-20.7 K0.8
G00 Z15.
G17

(2D CONTOUR1 2)
G00 X3. Y9.664
Z15.
Z5.
G01 Z-7.2 F557.
G19 G02 Y8.864 Z-8. J-0.8
G01 Y2.622
Y-22.5
Y-42.617
Y-47.617
G02 Y-48.417 Z-7.2 K0.8
G00 Z5.
Y9.664
G01 Z-15.2 F557.
G02 Y8.864 Z-16. J-0.8
G01 Y2.622
Y-22.5
Y-42.617
Y-47.617
G02 Y-48.417 Z-15.2 K0.8
G00 Z5.
Y9.664
G01 Z-20.7 F557.
G02 Y8.864 Z-21.5 J-0.8
G01 Y2.622
Y-22.5
Y-42.617
Y-47.617
G02 Y-48.417 Z-20.7 K0.8
G00 Z15.
G17
G53 G00 Z0.

(2D CONTOUR1)
G55
G00 X-135. Y-45.8
G43 Z15. H04
G00 Z5.
G01 Z-7.2 F557.
G19 G03 Y-45. Z-8. J0.8
G01 Y-40.
Y0.
Y5.
G03 Y5.8 Z-7.2 K0.8
G00 Z5.
Y-45.8
G01 Z-3. F557.
Z-15.2
G03 Y-45. Z-16. J0.8
G01 Y-40.
Y0.
Y5.
G03 Y5.8 Z-15.2 K0.8
G00 Z5.
Y-45.8
G01 Z-11. F557.
Z-20.7
G03 Y-45. Z-21.5 J0.8
G01 Y-40.
Y0.
Y5.
G03 Y5.8 Z-20.7 K0.8
G00 Z15.
G17

(2D CONTOUR1 2)
G00 X3. Y9.664
Z15.
Z5.
G01 Z-7.2 F557.
G19 G02 Y8.864 Z-8. J-0.8
G01 Y2.622
Y-22.5
Y-42.617
Y-47.617
G02 Y-48.417 Z-7.2 K0.8
G00 Z5.
Y9.664
G01 Z-15.2 F557.
G02 Y8.864 Z-16. J-0.8
G01 Y2.622
Y-22.5
Y-42.617
Y-47.617
G02 Y-48.417 Z-15.2 K0.8
G00 Z5.
Y9.664
G01 Z-20.7 F557.
G02 Y8.864 Z-21.5 J-0.8
G01 Y2.622
Y-22.5
Y-42.617
Y-47.617
G02 Y-48.417 Z-20.7 K0.8
G00 Z15.
G17

M09
G53 G00 Z0.
G53 X0. Y0.
M30

 

[13engines]

There is no need to re-call the G43 tool offset when moving from G54 to G55. It might even be what's screwing you up.

EDIT: The statement above would be true in most circumstances, but may not be true after a G53. Seems I heard once that G53 cancels Tool Height Offset. I use G53 to go Home all the time, but it's typically followed by a Tool Change and a massive G Code infested tool startup safety line, so it never gives me trouble.

Also make sure you have the proper sign (+ / -) associated with your two work offset Z settings. And be conscious of how the Z setting in each work offset relates to how and where (and at what height) the tool(s) were measured.

 

[GENERALDISARRAY]

The only thing I see in the program is the G53 instead of G28. I dont think that is a problem.

So you can run the G55 posted program on the machine and it is right. Can you also run only the G54 program?

What surface are the tools set to? What are the Z values of 54 and 55.

 

[voicurob]

The origin on both parts is back-right-top corner. The tool height was measured on the G54 part.
I removed the G43 from the G55 part, it still does the same thing.

 

[GENERALDISARRAY]

If the tools were measured on the top of the G54 part. Why does G54 have a Z value?

If you are measuring the tools on top of the part. And the program Z zero is also the top of the part. The work offset Z value should be zero. The Z value for G55 then would be the delta from the top of one part to the other.

 

[13engines]

If you measured your tools Z height on the G54 part, your G54 Z setting should be Z0, and the G55 Z setting should be the DIFFERENCE between the G54 height and the G55 height. (With the correct sign)

The heights you measured for your tools need to be entered in your Tool Offset Tables. (Likely labeled 1-32) That's where G43 goes looking to properly set your tools.

Ha... looks like The General beat me to it. :-)

 

[voicurob]

I tried what you said and this happend

 

[GENERALDISARRAY]

Your tool offsets are wrong. Setting your tools on top of the part, will yield a big negative number. You had a big negative in you workoffset before. So i imagine you have a small value in the tool offsets.

Are you using a piece of paper/shim stock? the Z value you want when you measure the tool should come from the "machine" register. So if there is a measure/MZ function. make sure thats what you get.

This is all going off of you saying you touched the tools on top of the part. There are many ways to do tool offsets. I personally think off the top of the part is not a great way. But thats what you said you were already doing it. We can make this work and discuss further later.

 

[voicurob]

I use a 3D tester (haimer) to take work offset. When I have to register tool offset I go with the 3D tester on a surface, in this case was the part on the left (G54) and reset the Z value in relative to 0. Afterwards I measure the tools on the same surface using a gauge block, and I input the value shown into the relative coordinate system minus the height of the gauge block in the tool offset table.
Concerning my initial question, if I run only G54, or any other for that matter (G55, G56, etc) it works fine with the work offsets shown in the picture above.
The issue appears when I output multiple work offsets in the same program from Fusion360.

 

[DouglasJRizzo]

When transferring over from G54 to G55, ditch the G53 and no need to re-call the tool height.
Jack the Z axis up an inch, then let it come back down to correct Z height AFTER the G55 X-Y move. Should be OK.

 

[13engines]

With Single Block turned on and your Check Screen active, (and your finger at the ready on Feed Hold) try this. Your Fusion output only slightly changed.

Due this only if your G55 is the lower vise on the right which I think you said it was.

(T3 D=5. CR=0. - ZMIN=-21.7 - FLAT END MILL)
(T4 D=8. CR=0. - ZMIN=-21.5 - FLAT END MILL)
G90 G94 G17 G80
G21
G53 G00 Z0.

(SLOT1)
T3 M06
S5800 M03
G54
G00 X-1. Y-20.
G43 Z15. H03
G01 Z5.F250.
G00 Z15.

(SLOT1)
G55
X-1. Y-20.
Z15. (The Z portion of your G55 Offset should not become active until this move.)
G01Z5.
G00 Z15.
G53 Z0.M5
M30

If this doesn't work then there is something wrong with your settings. Be it Tool or Work offset I'm not sure yet.

 

[voicurob]

I tried what you said 13engines, it did not work.
Also I changed the set up, i put 3 parts in the same z plane and when it moves to G55 and G56 also it has a +z offset. I think this was the case before also, but because of the height difference between the vises it seemd to keep the same z value as G54.
Thanks everybody for the help

 

[13engines]

Hello Voicurob,

Sorry to see you're having to revert to alternate setups to get the job done. Your original setup should work if setup properly.

Two things.

1) Make sure your Manual/Absolute switch is on and stays that way. The one on my OM even has a cover over it.

2) In all the years of running Fanucs, including my OM, never once has any of my machines made a single move that it wasn't told to do. That has to be millions of moves by now without an error that wasn't my fault.

My point being..., it is highly unlikely that something is wrong with your machine control or even the programming you provided. (except the extra G43 stuff)

Something somewhere in the setup process is not being done correctly.

Just for shits and giggles... try these steps. We'll use G57 - G59 so you don't have to change your current stuff. Pretend G57 is your G54.

Either enter these numbers or run this program.

%
0100 (SET WORK OFFSETS G57-G59)

G90G10L2P0X0Y0Z0 (SET SHIFT)
G90G10L2P4X200.Y-300.Z0. (SET G57)
G90G10L2P5X250.Y-300.Z-25. (SET G58)
G90G10L2P6X300.Y-300.Z-50. (SET G59)
M30
%

I'm assuming you have a 25-50-75 block handy.

1) Set your 25-50-75 block somewhere upright so the 75mm side is presented to the spindle.
2) Take a tool, any tool, and bring it down and touch off the tool to the top of the block. (not critical to touch it exactly)
3) Go to your POSITION screen and write down the Z coordinate shown by the MACHINE COORDINATE display. Do not use any other number.
4) Enter that number just like you see it into the TOOL OFFSET REGISTER for the tool number you're using.
5) Run the following in SINGLE BLOCK MODE. Obviously you have to be sure you're working in a safe area. Adjust the Offset setting program 100 to suit the current conditions on your machine. Also set correct tool number. If your machine will allow feed moves with a dead spindle, remove the M3.

%
O101 (WORK OFFSET TEST)

(TEST TOOL)
G17G21G40G49G57G80G90G98

G0X0.Y0.
G43Z25.H#S100M3 (SET TOOL OFFSET NUMBER HERE (#) REMOVE M3 IF OK )
G1Z0.F250.
G0Z25.
G58X0.Y0.
Z25.
G1Z0.
G0Z25.
G59X0.Y0.
Z25.
G1Z0.
G0Z25.
G53Z0.M5
M30
%

If everything is working, this will simply move the tool up and down 25mm and to the right 50mm as it steps through each offset change. Each offset should exhibit a Z0. that is 25mm lower then the previous one. All verifiable by checking with your 25-50-75 block.

There are many ways to set up tool offsets. I just want to show you that your machine will act properly if the tool is set up properly. Use what you might see and learn here to adjust your current process. Sorry if this all seems elementary. I have no idea what your experience or skill level is. Hope it helps. Time to get back to work...

 

[voicurob]

Well the machine works fine, until now I posted the program to do the machining with one tool on all parts, then change to the next tool and so on, this, to have only 2 tool changes instead of 6. When i post my program this way, it does that weird thing. I posted the program with one part ( 6 tool changes) at a time and it works just fine. Is annoying, but still better than one part at a time.

I do not have much experience, i started the machine shop at the end of 2019 with a Haas Minimill (I still have it), and I am self-taught. The fanuc O-M machine it has around 6-7 months in my shop. So I greatly appreciate all the help I get

 

[Fancuku]

I have a feeling you need to cancel tool length offset with G49 after you send the spindle to machine home position G53.
Add a G49 below every G53 line and see if that works.

 

[voicurob]

I will try it tomorrow. i forgot to mention that i use a dnc to drip feed the program to the machine.

 

[voicurob]

I treid the G49, it does not work. For now, i will work like this because i have to finish this parts.
Thanks everybody. If i find the solution to this i will update the post

 

[sinha]

I may not have understood your problem, but if you are able to correctly use all the tools with G54, it means that G54 work offset as well as all tool offsets (H01, H02 etc) are correct. However, if the same is not true with other work offsets (G55, G56 etc), it means that the offset procedure for G55 etc is not correct.
For G55, for example, first execute G55 in the MDI mode, and repeat the offset procedure, without pressing the RESET key.