Talent 6/45 Reference Issue Fanuc oi-T Controller

Full disclosure I am not that experienced with CNC but I am out of ideas as to why a certain line of G-Code is causing issues. The problem is as follows. After referencing the machine to its zero position using the controller I start a code that repeatedly wants to run the turret into the spindle if I don't hit cycle stop. The line of code causing issues is G0 X.9082 Z6.2. Which I think should be a rapid move to the start of the work. I have checked tool and work offsets however the controller always thinks the work is ~12 inches past the spindle ie there is always a foot of distance to go listed on the controller when the edge of the tool is 1" from the chuck. The only way I have prevented this from happening is to reference to machine zero engage machine lock out and in handwheel mode set the absolute z and x to zero to match the machine zero. When the same code is run again it doesn't want to crash the lathe rather it appears to reference way above (12") where the work would be toward the tailstock. If anyone needs more information I'll post the full code tomorrow when I can get access to the CNC computer. Appreciate the help at this point I'm stumbling around in the dark here.

What offsets....( tool & work offset ) are active when that line of code is executed ?
Put up the NC file

Z setting
I have set our lathe machine origin, so that chuck face is work zero origin, and the value I input on G54 Z is the distance from chuck face to the part origin ( generally the stock size )
- tool ZERO offset is the turret face, so that any tooling offsets can be physically measured with a rule to verify that the tool has been set ( it'll be close anyway )

X setting
Dial indicator is held by spindle to clock inside ER32 ( must be zero T.I.R ), so that any X0.0 (zero) offset on a tool for drilling on the spindle centreline

Here is the NC file.

Code:

---

%
O0007
(PROGRAM NAME - THREADED PART_0304)
(DATE=DD-MM-YY - 04-03-16 TIME=HH:MM - 17:10)
(MCX FILE - C:\USERS\MELABUSER\DOCUMENTS\EXP2\THREADED PART.EMCX-9)
(NC FILE - C:\USERS\MELABUSER\DOCUMENTS\MY MCAMX9\LATHE\NC\THREADED PART_0304.NC)
(MATERIAL - STEEL INCH - 1030 - 200 BHN)
G20
N0101
(TOOL - 1 OFFSET - 1)
(LROUGH OD FINISH RIGHT - 35 DEG.  INSERT - VNMG-431)
G97S1000M03
G0T0G30U0.W0.
T0101
G0X.98017Z6.2
G1G99Z6.1F.005
Z2.90854
X1.
X1.14142Z2.97925
G0Z6.2
X.96034
G1Z6.1
Z2.90854
X1.
X1.14142Z2.97925
G0Z6.2
X.9405
G1Z6.1
Z2.90854
X.98034
X1.12176Z2.97925
G0Z6.2
X.92067
G1Z6.1
Z2.90854
X.9605
X1.10193Z2.97925
G0Z6.2
X.90084
G1Z6.1
Z2.90854
X.94067
X1.08209Z2.97925
G0Z6.2
X.88101
G1Z6.1
Z2.90854
X.92084
X1.06226Z2.97925
G0Z6.2
X.86118
G1Z6.1
Z2.90854
X.90101
X1.04243Z2.97925
G0Z6.2
X.84134
G1Z6.1
Z2.90854
X.88118
X1.0226Z2.97925
G0Z6.2
X.82151
G1Z6.1
Z2.90854
X.86134
X1.00277Z2.97925
G0Z6.2
X.80168
G1Z6.1
Z2.90854
X.84151
X.98293Z2.97925
G0Z6.2
X.78185
G1Z6.1
Z2.90854
X.82168
X.9631Z2.97925
G0Z6.2
X.76202
G1Z6.1
Z3.99811
G3X.77Z3.98435R.02565
G1Z3.96194
Z3.00484
Z2.98437
Z2.90854
X.80185
X.94327Z2.97925
G0Z6.2
X.74218
G1Z6.1
Z4.00716
G3X.77Z3.98435R.02565
G1Z3.96194
Z3.00484
Z2.98437
Z2.90854
X.78202
X.92344Z2.97925
G0Z6.2
X.72235
G1Z6.1
Z4.00994
G3X.7622Z3.99795R.02567
G1X.90361Z4.06868
G0Z6.2
X.70252
G1Z6.1
Z4.01
X.71874
G3X.7424Z4.0071R.02565
G1X.88377Z4.07783
G0Z6.2
X.68269
G1Z6.1
Z4.01
X.71874
G3X.7225Z4.00995R.02565
G1X.86394Z4.08064
G0Z6.2
X.66286
G1Z6.1
Z4.01
X.70269
X.84411Z4.08071
G0Z6.2
X.64303
G1Z6.1
Z4.99142
G3X.645Z4.98435R.02564
G1Z4.04119
Z4.01
X.68286
X.82428Z4.08071
G0Z6.2
X.62319
G1Z6.1
Z5.00535
G3X.645Z4.98435R.02566
G1Z4.04119
Z4.01
X.66303
X.80445Z4.08071
G0Z6.2
X.60336
G1Z6.1
Z5.00954
G3X.6432Z4.9911R.02566
G1X.78461Z5.06182
G0Z6.2
X.58353
G1Z6.1
Z5.01
X.59374
G3X.6234Z5.0053R.02565
G1X.76478Z5.076
G0Z6.2
X.5637
G1Z6.1
Z5.01
X.59374
G3X.6035Z5.00955R.02565
G1X.74495Z5.08024
G0Z6.2
X.54387
G1Z6.1
Z5.01
X.5837
X.72512Z5.08071
G0Z6.2
X.52403
G1Z6.1
Z5.01
X.56387
X.70529Z5.08071
G0X1.005
G97
G0T0G30U0.W0.
M30
%

---

From what you suggested I think the line "G0X.98017Z6.2" should be "G54 G0X.98017Z6.2" to select offset 1. From what I can tell on the controller the machine origin is the turret reference position back towards the tailstock not sure how to change this though. Also could you elaborate on how to set T.I.R? I broke a center drill one afternoon since this was not correct. Thanks for the help.

Quote:

---

Originally Posted by hinshelwood

From what you suggested I think the line "G0X.98017Z6.2" should be "G54 G0X.98017Z6.2" to select offset 1. From what I can tell on the controller the machine origin is the turret reference position back towards the tailstock not sure how to change this though. Also could you elaborate on how to set T.I.R? I broke a center drill one afternoon since this was not correct.

---

I don't think it is the G54......use MDI to change to G55, look at what is active, then hit RESET....it should revert back to G54, which is normal, but be aware that everything should be programmed in G54
I'm thinking that you have not set the work offset correctly, or you have not got good "safety codes" at the beginning of the program

Here is a link to my Hardinge machine & post.......I can see you are using Mcam
( it has a better NC program startup, goes home before any toolchange, no G54 uses G28 reference return .... checkout the Misc Integers page #1 & #3 fields


Trueing the Turret
Sometimes a tool may take a knock, causing the turret to be misaligned, ( a centring tool or drill is NOT laying on the X axis plane, any movement in X cannot bring that tool to the correct position, it is either above, or below spindle centre )
- is usually means the turret needs to be placed back into its correct position, where the centring tool is inline with the spindle axis.

To loosen the turret, there is 8 bolts & 2 dowels in the turret face, ( dowels can be removed, screws loosened to bring a drill holder onto the X plane
- use a lever dial indicator ( mounted to the spindle, the indicator clocks the drill holder true by rotating the turret & moving the X-axis together until the holder is in correct position
- tighten the turret screws very tight, check manual for correct torque pressure........ ( I have found that you need to go higher than specified )
- record X absolute position, set the tool offset for the tool station you have just trued to X0.0000, activate that offset, the absolute position should be X0, if not you have to adjust the machine origin so it does read zero
- any value that is input is not updated until you re-actives that offset
- any tool offset that is set to X0, and if you program a tool to go to X0 should be putting that holder onto the spindle centreline

- as you have adjusted machine X origin, you would need to re-gauge all tools again

You were right. I was not setting the work offsets correctly. On this machine I had to reference the machine on the control side to machine zero. Upload the code. Set work and tool offset. Return to machine zero then run the code. Been so busy turning parts I forgot to update the thread.