X zero, y zero issues

[cstprecision]

I recently obtained a Centroid CNC Milling machine, serial # is 20528, the machine model is M400S, it has a centroid M-series controller and the system ID is 1018051077. I've been working through programming my first part and established XYZ zero and when I go to run a program it runs shifted from where I established XYZ zero. I bought this machine used and I'm guessing it is a setting somewhere that causes it to offset but I'm not sure what would need to change to have this reference from the zero I establish.

I suspected that I may have incorrectly established XYZ zero and tried again while positioning the part on the opposite side of the vise. The program ran offset from what I established as XYZ zero by about the same amount as the first attempt. I look forward to your thoughts and help with this. Z zero seems to be correct, X and Y are off but it may just be a setting I'm not familiar with. Any direction or advice on overcoming this issue is greatly appreciated.

[tblough]

Are you setting the part 0 on the correct UCS? Post your CNC file you are trying to run. I suspect the G-code has a G55/56/57 and not the expected G54 for UCS#1.

[cstprecision]

; ICN_PATH = c:\intercon\afl rd 2.icn
; --- Header ---
N0001 ; CNC code generated by Intercon v2.72
; Description: square mach spec
; Programmer: dc
; Date: 21-Oct-2011
M25 G49 ; Goto Z home, cancel tool length offset
G17 G40 ; Setup for XY plane, no cutter comp
G20 ; inch measurements
G80 ; Cancel canned cycles
G90 ; absolute positioning
G98 ; canned cycle initial point return
; --- Tool #1 ---
;Tool Diameter = 0.4980 Spindle Speed = 1500
;.500 em
G49 H0 M25
G0 X0.0 Y0.0
N0002 T1 M6
S1500 M3
G4 P1.00 ; pause for dwell
G43 D1
; --- Rapid Traverse ---
N0003 M25 H1
X-0.7025 Y0.5
; --- Face ---
N0004 X-0.7025 Y0.5 Z0.1
G1 G91 X0.0 Y0.0 Z-0.13 F12.0
X1.405 Y0.0 Z0.0
X0.0 Y-0.15 Z0.0
X-1.405 Y0.0 Z0.0
X0.0 Y-0.15 Z0.0
X1.405 Y0.0 Z0.0
X0.0 Y-0.15 Z0.0
X-1.405 Y0.0 Z0.0
X0.0 Y-0.15 Z0.0
X1.405 Y0.0 Z0.0
X0.0 Y-0.15 Z0.0
X-1.405 Y0.0 Z0.0
X0.0 Y-0.15 Z0.0
X1.405 Y0.0 Z0.0
X0.0 Y-0.1 Z0.0
X-1.405 Y0.0 Z0.0
G0 G90 X-0.7025 Y-0.5 Z0.1
; --- Line ---
N0005 G1 X-1.02 Y-1.0 Z0.1
; --- Frame (Outside Rect) ---
N0006 G0 X0.609 Y0.639 Z0.1
G1 G91 X0.0 Y0.0 Z-0.1
X0.0 Y0.0 Z0.0
X0.03 Y0.0 Z-0.03
X-1.278 Y0.0 Z0.0
G3 X-0.25 Y-0.25 Z0.0 J-0.25
G1 X0.0 Y-0.778 Z0.0
G3 X0.25 Y-0.25 Z0.0 I0.25
G1 X1.278 Y0.0 Z0.0
G3 X0.25 Y0.25 Z0.0 J0.25
G1 X0.0 Y0.778 Z0.0
G3 X-0.25 Y0.25 Z0.0 I-0.25
G1 X-0.03 Y0.0 Z0.0
X0.03 Y0.0 Z-0.03
X-1.278 Y0.0 Z0.0
G3 X-0.25 Y-0.25 Z0.0 J-0.25
G1 X0.0 Y-0.778 Z0.0
G3 X0.25 Y-0.25 Z0.0 I0.25
G1 X1.278 Y0.0 Z0.0
G3 X0.25 Y0.25 Z0.0 J0.25
G1 X0.0 Y0.778 Z0.0
G3 X-0.25 Y0.25 Z0.0 I-0.25
G1 X-0.03 Y0.0 Z0.0
X0.03 Y0.0 Z-0.03
X-1.278 Y0.0 Z0.0
G3 X-0.25 Y-0.25 Z0.0 J-0.25
G1 X0.0 Y-0.778 Z0.0
G3 X0.25 Y-0.25 Z0.0 I0.25
G1 X1.278 Y0.0 Z0.0
G3 X0.25 Y0.25 Z0.0 J0.25
G1 X0.0 Y0.778 Z0.0
G3 X-0.25 Y0.25 Z0.0 I-0.25
G1 X-0.03 Y0.0 Z0.0
X0.03 Y0.0 Z-0.03
X-1.278 Y0.0 Z0.0
G3 X-0.25 Y-0.25 Z0.0 J-0.25
G1 X0.0 Y-0.778 Z0.0
G3 X0.25 Y-0.25 Z0.0 I0.25
G1 X1.278 Y0.0 Z0.0
G3 X0.25 Y0.25 Z0.0 J0.25
G1 X0.0 Y0.778 Z0.0
G3 X-0.25 Y0.25 Z0.0 I-0.25
G1 X-0.03 Y0.0 Z0.0
X0.03 Y0.0 Z-0.03
X-1.278 Y0.0 Z0.0
G3 X-0.25 Y-0.25 Z0.0 J-0.25
G1 X0.0 Y-0.778 Z0.0
G3 X0.25 Y-0.25 Z0.0 I0.25
G1 X1.278 Y0.0 Z0.0
G3 X0.25 Y0.25 Z0.0 J0.25
G1 X0.0 Y0.778 Z0.0
G3 X-0.25 Y0.25 Z0.0 I-0.25
G1 X-0.03 Y0.0 Z0.0
X0.03 Y0.0 Z-0.03
X-1.278 Y0.0 Z0.0
G3 X-0.25 Y-0.25 Z0.0 J-0.25
G1 X0.0 Y-0.778 Z0.0
G3 X0.25 Y-0.25 Z0.0 I0.25
G1 X1.278 Y0.0 Z0.0
G3 X0.25 Y0.25 Z0.0 J0.25
G1 X0.0 Y0.778 Z0.0
G3 X-0.25 Y0.25 Z0.0 I-0.25
G1 X-0.03 Y0.0 Z0.0
X0.03 Y0.0 Z-0.02
X-1.278 Y0.0 Z0.0
G3 X-0.25 Y-0.25 Z0.0 J-0.25
G1 X0.0 Y-0.778 Z0.0
G3 X0.25 Y-0.25 Z0.0 I0.25
G1 X1.278 Y0.0 Z0.0
G3 X0.25 Y0.25 Z0.0 J0.25
G1 X0.0 Y0.778 Z0.0
G3 X-0.25 Y0.25 Z0.0 I-0.25
G0 G90 X0.639 Y0.639 Z0.1
; --- End of Program ---
N0007 G49 H0 M25
G40 ; Cutter Comp Off
M5 ; Spindle Off
M9 ; Coolant Off
G80 ; Cancel canned cycles
M30 ; End of program

[cnckeith]

I would start by reviewing these Mill training videos.
viewtopic.php?f=61&t=2118

[cncsnw]

1) After you get done setting your part zero location, jog or use MDI to move X and Y both to zero, then jog Z down.
Is the tool tip where you expect it to be?

2) Use F8/Graph to view a graphic preview of your CNC program. In the 2D Top view (the initial default view), note the X and Y rulers along the bottom and left sides of the graphic window. Use the cursor arrow keys to make the pan/zoom crosshairs appear, then move the crosshairs to X0 and Y0.
Are the crosshairs over the point on the toolpath where you expect X0 and Y0 to be?

3) Start the program running. When it gets to the tool change position (at X0 and Y0), press Cycle Cancel, then jog Z down.
Is it still over the place where you set your part zero location?

[ghack]

I dont see a wcs in that code.

[tblough]

I don't see a WCS callout, but I do see some weird things with tool offsets:

Code: Select all

G43 D1
.
.
.
N0003 M25 H1

First there's a tool length compensation using a diameter offset, and then a move Z home callout with a length offset. I wonder if those could be causing the problem.

[ghack]

I noticed that also but i have never studied my intercon generated programs. they have always worked graphically so i go with it and i have never had a problem.

[cncsnw]

While the ordering is a little odd, there is nothing wrong with those codes.

Remember that G43 mode, and the D_ and H_ numbers, are modal values. They take effect on the line they are on, and remain in effect until changed.

So, the earlier line that says "G43 D1" means:
1) Activate tool height compensation with the current H offset (which is probably H0, resulting in no offset yet)
2) Set the active D offset number to D1 (which will have no effect until a subsequent G41 or G42)

The later line that says "M25 H1" means:
1) Set the active H offset to H1. Since G43 is already in effect, we will now start applying the value of H1 to Z moves.
2) Move the Z axis to its home/tool-change/G28 position

For reasons that are now ancient history, the post-processor defers the H value until the first line that specifically moves the Z axis.

The program would run just the same if it just said "G43 H1" on the line with the Z move, or just before it.

The program would cut just the same if the D value did not appear until any G41 or G42, but I think having the D value appear early (just after the tool change, regardless of whether G41/G42 is going to be used) allows the Run-time Graphics display to show an appropriately sized circle for the cutter.

[ghack]

Thats fine but the issue is no wcs?