Fagor 8055 Lathe Z axis Soft Limit Overrun error

[ohsnapfit]

Hello,
I am getting a Clausing MultiTurn 2000MR with a Fagor 8055 up and running and am hitting a wall. It hasn't run in a few years since it came with a company merger.

It is giving me a Z axis soft limit overrun error as it tries to run the tool change (Line 16) and looks ahead to (line 21). This would make sense if G0 X3.7 Z5.061 was in machine coordinates as the soft limits for Z are (+10, +40), but it is not, it is in G54 (line 17).

I obviously don't want to program my part in machine coordinates.

I have homed the machine.

I have tried replacing lines 14 and 15 with

• N14 G74 X
• N15 G74 Z

So far, nothing. And I do not want to simply remove the soft limits.
If you have encountered anything like this, I would very much appreciate your input.
Also, for what it's worth, programed in Fusion 360 with a mostly stock Fagor 8055 turning post.




%Test,MX,
N10 G90 G95 G18
N11 G70
N12 G151
N13 G92 S1000
N14 G53 G0 X0.
N15 G53 G0 Z20.
;FACE2
N16 T1 D1
N17 G54
N18 M8
N19 G90 G94 G18
N20 G97 S600 M3
N21 G0 X3.7 Z5.0095
N22 G0 X2.9
N23 G1 X2.5 F4.8
N24 X-0.0625
N25 X2.9
N26 G0 Z4.9695
N27 G1 X2.5 F4.8
N28 X-0.0625

 

[604Pook]

I have never had that happen with my Maxcut lathe with the same control.

I know there is a spot in the control to set your tool change position, where that tool change position is, is listed on the main screen on my control.

Do you have the manuals?

 

[ohsnapfit]

I have never had that happen with my Maxcut lathe with the same control.

I know there is a spot in the control to set your tool change position, where that tool change position is, is listed on the main screen on my control.

Do you have the manuals?

Hi Pook,
1) Yes, I have the manuals.
2) I did just the tool change and it works.
%Test,MX,
%Works
N10 G90 G95 G18
N11 G70
N12 G151
N13 G92 S1000
N14 G74 X
N15 G74 Z
;FACE2
N16 T1 D1
N17 G74 X
N18 G74 Z
N19 M30
%

3) I did just the G0 X3.7 Z5.0095 and it gives the soft limit error:
%Test,MX,
N10 G90 G95 G18
N11 G70
N12 G151
N13 G92 S1000
N14 G74 X
N15 G74 Z
;FACE2
N16 G54
N17 G0 X3.7 Z5.0095
N18 G74 X
N19 G74 Z
N20 M30
%

3) I found in the Fagor Manual that I can type (ORGX54=##.###, ORGZ54=###.###) to update the table. This is obviously convoluted and error prone, but it did update the G54 table (whereas typing G54, hitting X, 0, enter (are you sure? /yes) did not.
This still did not allow for the program in bullet point 2 to work.

 

[alphonso]

Change your soft limits to something greater than actual travel. May need to restart control for change to take effect. Whatever you do, DO NOT "initialize" parameters. One of my Fagor flatbed machines has 80 inches of Z. Kinda hard to home when tailstock is at 48 inches. I changed parameters to not require homing. You can download all the manuals from Fagor USA or Fagor Korea.

I don't understand why you have the G53/G54 in your program.

Snippet of proven program:

N10 T1 D1;(WNMG 432)
N20 M43
N30 G97 S311 M03
N40 G0 X4.29 Z28.6
N50 G92 S663
N60 G96 S350
N70 F.02 M08
N80 G68 X2.39 Z28.5 C.1 L.02 M.005 H.01 S1810 E1990
N90 G97 S311
N100 M09
N110 G0 X0 Z29. D0
N120 M01

 

[ohsnapfit]

Alphonso,
I operate mills with the assumption that softlimits save machinery.
Do I understand correctly you are saying to just run this without softlimits?
How do I know that at some point in the future, me or another user won't try to run a profiling cycle for a 6in part with 5in stock sticking out of the jaws?

 

[ohsnapfit]

OK I got things working.
I ditched G53, G54, and G74. To park in a safe tool change position, I do it based on the "work coordinate" and cancel out the tool offset so that it goes to the same place for every tool using D0.

Thanks everyone.


%Face and Turn,MX,
N10 G90 G95 G18
N11 G70
N12 G151
N13 G92 S900
N14 G0 X5. D0
N15 G0 Z10. D0
;FACE2
N16 T1 D1
N17 M8
N18 G90 G94 G18
N19 G97 S600 M3
N20 G0 X3.7 Z0.0266
N21 G0 X2.9
N22 G1 X2.6131 F4.8
N23 X2.5 Z-0.03
N24 X-0.0625
N25 G0 X3.7
;PROFILE ROUGHING2
N27 G0 X3.3 Z0.1969
N28 Z-0.015
N29 X2.44

etc etc