3.1 Work Coordinates and Fixture Offset Setting
Key Takeaways
Haas mill G54 through G59 select work coordinate systems. G154 P2 selects the second additional work offset.
On a Haas mill, G53 addresses machine coordinates for its own block. It also ignores tool offsets in that block.
For a 0.200-inch contact diameter, move 0.100 in from the measured centerline coordinate toward the contacted edge, with the sign determined by the approach.
For a round bore, the average of the opposing probe coordinates along an axis locates the bore midpoint along that axis when the effective probe radius is the same in both directions.
When setting work Z from a gage block, account for block height and the measurement reference. If the raw Z value describes the spindle gauge line, include the probe or tool length where applicable.
Work Coordinates and Fixture Offset Setting
The drawing and setup sheet determine where the program’s part zero belongs. Locate that origin on the actual workpiece and record it in the fixture offset that the program calls. Keep tool length separate so you can run different tools against the same work origin. The code and coordinate examples below use a three-axis Haas mill with parallel machine and work axes, no additional shifts or coordinate transformations, and inch units.
Machine Coordinates and Work Coordinates
The machine coordinate system has fixed axis references for the setup. On a Haas mill the machine zero for an axis is the position established by its zero-return procedure. It need not represent the end of physical travel. G53 references machine coordinates in the block where it is commanded and ignores tool offsets in that block. In contrast, G54 through G59 select stored work coordinate systems and remain active until changed. Optional fixture zero locations have their own registers.
| Command | What it addresses | Example use |
|---|---|---|
| G53 | Axis coordinate measured from machine zero for this block | A documented machine-coordinate retract |
| G54 through G59 | Six stored work coordinate systems | Two vises hold parts with different program origins |
| G154 P1 through P99 | Haas additional work offsets | G154 P2 addresses the second additional offset |
Read the machine and work tabs separately. If G54 X is −10.000 in and a G90 move targets work X = +1.250 in, the machine-coordinate target is −8.750 in with the stated setup assumptions. That addition is an axis calculation. A new origin can move a programmed path closer to a clamp or beyond travel, so prove out the actual setup before cutting.
Establish XY Zero from Two Faces
Suppose the part zero is the intersection of the left X face and the front Y face of an aligned rectangular workpiece. Touch the faces that the setup sheet identifies. Check that dirt, a burr or a chamfer will not move the contact point. A mechanical edge finder such as the Starrett 827A has a 0.200-inch cylindrical contact. Secure the tool in a compatible holder and follow the finder and machine instructions for speed, approach, and safeguarding. In a rotating edge-finder procedure, the cylindrical contact first runs into alignment and then moves visibly sideways as the feed advances. Use the established measurement procedure to identify the pickup point.
The coordinate at pickup describes the spindle centerline. Starting on the low-X side and moving the tool relative to the workpiece in +X, the centerline is one contact radius below the X coordinate of the face. Add the radius. Starting on the high-X side and approaching in −X, subtract the radius. Apply the same logic along Y. Distinguish tool motion relative to the workpiece from the direction the physical table appears to move.
| Face contacted | Tool starts | Correction to the measured centerline for a 0.200-inch contact |
|---|---|---|
| Low-X face | Outside on the low-X side | Add 0.100 in to X |
| High-X face | Outside on the high-X side | Subtract 0.100 in from X |
| Low-Y face | Outside on the low-Y side | Add 0.100 in to Y |
| High-Y face | Outside on the high-Y side | Subtract 0.100 in from Y |
Example: A low-X pickup reads machine X = −10.100 in and a low-Y pickup reads machine Y = −6.225 in. The corrected face coordinates are −10.000 in and −6.125 in. Those are the XY coordinates to store if the intersection is the desired origin. If the drawing instead puts zero 0.250 in to the right of the low-X face, add that drawing offset after the contact correction, giving G54 X = −9.750 in. Verify the register, signs, and the physical point before motion.
Establish XY Zero from a Hole
For a hole-based origin, identify the correct hole, remove debris and measure on the bore wall below any chamfer. A spindle-mounted dial test indicator can be used to sweep the bore under the machine’s approved stopped-spindle procedure. Compare opposite points in X, then Y, and adjust the axes to match the opposing readings. Recheck both pairs at the same depth and sweep the contour again. The acceptable variation depends on the setup and indicator. Irregular bore form, dirt, seating error and indicator geometry can leave a nonzero sweep even at the best practical center. A sweep for setup is not proof that the hole satisfies its geometric tolerance.
A calibrated work probe can locate the center and set a chosen register through its supported bore cycle. For an ideal round bore with equal effective probe radius on each side, the center is the average of two opposite pickup coordinates. If opposing X readings are −8.120 in and −7.380 in, the midpoint is −7.750 in. Repeat on Y. Enter or check both stored coordinates, and check that the selected probing cycle addresses the intended work offset.
Set Z with a Known Height
With positive Z away from the part, a gage block’s top is above the workpiece surface by its height. Determine which physical point the position value describes. If the reported machine Z describes the spindle gauge line and a 4.000-inch tool projects straight down from it, the tool-tip coordinate is the gauge-line Z minus 4.000 in. In the assumed gauge-line-based setup with the full tool length in the H register, subtract the block height as well to locate the part surface.
Example: At contact with a 1.000-inch block, the spindle gauge line is at machine Z = −10.250 in. The tool tip is at −14.250 in, and the part surface is at −15.250 in. If a measured coordinate already describes the tip, subtract the block height only. Using the same tool length in both calculations on that already-corrected display would introduce a second length correction. An electronic setter or probe has its own calibrated height and procedure. Avoid applying a separate height correction when the documented routine already accounts for it.
Sources: Haas part setup, Haas mill G-codes, Starrett 827A, and Haas wireless probing system from Renishaw.
A mechanical edge finder with a 0.200-inch contact diameter touches the low-X face while the tool approaches in +X relative to the workpiece. How do you find that face’s machine X coordinate?
Add 0.200 inches to the machine position reading
Subtract 0.200 inches from the machine position reading
Add 0.100 inches to the machine position reading
Subtract 0.100 inches from the machine position reading
Which command selects the second additional work offset on a Haas mill?
G154 P2
G54
G53
G154 P1
With Z positive away from the part, a 4.000-inch tool touches a 1.000-inch block on the top surface. At touch-off the spindle gauge line is at machine Z = −10.250 in. What is the top surface machine coordinate in this gauge-line-based setup?
−13.250 in
−14.250 in
−15.250 in
−11.250 in
On a known round bore, a calibrated work probe records opposing machine X contact coordinates of −8.120 in and −7.380 in. Assuming equal effective probe radius on both sides, what is the X center?
−0.740 in
−7.750 in
−7.380 in
−15.500 in
Sections you finish are checked off in the contents.