📷 IMAGE AREA — Setting the part X/Y zero with an edge finder and measuring tool length by touching a surface on the M70
Recommended size: 1200×630 px (16:9, hero) · WebP/JPG · <150 KB · filename: mitsubishi-m70-tool-work-offset.webp · alt: Mitsubishi M70 part zero with edge finder and tool length measurement
In this guide we cover two basic operations for a vertical machining center together: introducing the tool lengths and saving the part’s X, Y, Z zero to G54. The method described is the general one using a manual edge finder and touching the tool to the part. If the machine has an automatic tool-measuring sensor or a probe, the screen and operation sequence may differ.
1. The difference between the two zeros: tool zero and part zero
This is what beginners confuse most. Tool zero is introducing the tool’s length to the control. For example T1 face mill, T2 end mill and T3 drill are not the same length; the M70 control stores each tool’s length in an H offset number (T1→H1, T2→H2, T3→H3). When G43 H1 Z50. is used, the control accounts for the tool length in H1. Part zero is teaching the control where the program’s X0 Y0 Z0 point actually is on the real part; these values are usually saved to G54. On the M70/M700 control there are six basic workpiece coordinate systems, G54–G59.
2. The machine zero and the part zero are not the same
The machine zero is the fixed reference point set by the builder; the operator does not change it. The part zero is the start point the programmer sets relative to the part; the part’s lower-front corner, center, upper-right corner or top face can be chosen as zero. The Mitsubishi programming manual shows that the basic machine coordinate system and the G54–G59 workpiece coordinate systems are separate.
3. Preparing the machine before starting
Before setting zeros: turn on the machine, check the alarms on screen, send the axes to the reference point, clamp the part firmly in the vise/fixture, check the clamping elements do not enter the tool path, verify the tools in the magazine and match the tool number with the H number. It may not be possible to reliably create coordinates before the reference return is complete; the M700 handbook states that measurement and some moves can be blocked when the reference position is not complete.
4. Tool number and H number
| Tool | Use | Length offset |
|---|---|---|
| T1 | Face mill | H1 |
| T2 | End mill | H2 |
| T3 | Drill | H3 |
Program example: T2 M6 calls and changes the second tool; G43 H2 Z50. activates positive tool length compensation using the length in H2. To cancel compensation, G49 is used. The Mitsubishi programming manual states that tool length compensation is activated with G43/G44 and cancelled with G49.
5. Which screen is the tool length entered on?
On the M70 the general path is OFFSET → TOOL OFFSET → LENGTH/GEOMETRY. The menu names may be TOOL OFFSET, TOOL DATA, COMPENSATION, OFFSET, GEOMETRY, LENGTH depending on the machine. The tool offset numbers (H1, H2, H3, H4…) are shown; each tool’s measured length is written on its own line.
6. The basic logic of measuring tool length
All tools are touched to the same fixed surface. This fixed surface can be the machine table, a tool-setting block, a fixed master or a tool-measuring sensor. What matters is that all tools are measured against the same reference surface; measuring one tool from the table and another from the part randomly causes the tool lengths to not match each other.
7. Manual tool length measurement (step by step)
The method below is the general practice for a machine without a tool-measuring probe. Step 1 – Call the first tool: e.g. T1 M6; after the change, check that T1 is in the spindle. Step 2 – Switch to HANDLE/JOG: approach the tool to the measuring surface; come to a safe distance first, slow down in the last few mm, and use a small handwheel step (0.1 / 0.01 / 0.001 mm). Step 3 – Touch the reference surface: a thin paper or a gauge of known thickness can be placed between the tool tip and the surface; lower the tool slowly, stop when the paper is lightly pinched, and do not press into the surface. Especially on a drill tip, pay attention to which point is being measured (the real cutting tip and the cylindrical part are not the same point).
Step 4 – Select the H number: on the OFFSET screen, move to the H1 line for T1; check the cursor is on the correct line (if a value is written to the wrong H line, the program uses another tool’s length). Step 5 – Save the measurement value: the panel may have one of MEASURE, TEACH, INPUT C, CALC or TOOL MEASURE soft keys; use the relevant command while the tool is on the reference surface. Some machines need an axis selection (e.g. Z); the control computes the tool length into H1 based on the current machine Z position. (The M70 user parameters state that a confirmation message can be shown when offset data is written.) Step 6 – Retract the tool safely (in Z plus), check the H1 value formed on screen. Step 7 – Measure the other tools (T2→H2, T3→H3, T4→H4) — all must be touched to the same reference surface.
8. Checking the tool length table
After measurement, values like H1 −450.250, H2 −472.630, H3 −410.125 may be seen. Whether the values appear positive or negative depends on the machine’s coordinate structure; do not compare the sign with another brand/machine. The real check: has a very short tool appeared very long, is there an excessive difference between tools of similar length, was a value written to the wrong line, is the decimal point in the wrong place? For example if the expected value is about −450.000 but −45.000 is written, there is an error.
9. Tool radius / diameter compensation (D)
The tool length is entered in the H field, and the cutter’s diameter/radius usually in the D field. For example if T2’s diameter is 10 mm, depending on the control setting, 5.000 (radius) or 10.000 (diameter) may be entered in D2 — whether it is diameter or radius depends on the machine parameter and builder implementation. In the program, G41 D2 or G42 D2 is used. This is different from tool length measurement: length is held in H, diameter/radius in D.
10. Setting the part zero and the G54 screen
After the tool lengths are introduced, the part’s X, Y, Z zero is set. In this example we take the program zero as the part’s left edge (X0), front edge (Y0) and top face (Z0) and write the values to G54. General menu path: OFFSET → WORK OFFSET → G54 (may be COORD, WORK, COORDINATE, WORKPIECE OFFSET, G54–G59 depending on the machine). The G54 line has the X, Y, Z (and A/B/C if present) axis fields.
11. Setting the X part zero with an edge finder
We will make the part’s left edge X0. Step 1: mount the edge finder in the spindle (its number and size must be known). Step 2: for a mechanical edge finder, run the spindle at the low speed recommended by the maker; if an electronic probe/3D taster is used, the spindle is not run. Step 3: in HANDLE mode, approach the left edge on X, stop when the edge finder reacts/kicks out, and read the machine position (e.g. X −350.000). Step 4 – account for the edge-finder radius: if the diameter is 10 mm, the radius is 5 mm; since the left edge is touched from outside, there is 5 mm between the center and the real edge. Adding/subtracting the radius in the wrong direction makes the zero off by 5 mm; so use the M70’s MEASURE / CALC / EDGE function if possible. Step 5: go to the G54 X field, type X0 and apply MEASURE/INPUT C — meaning: take the tool center’s real position, with the edge-finder radius accounted for, as X0 in the G54 system. If the machine does not auto-calculate, the computed machine coordinate is entered by hand.
12. Setting the Y part zero
We will make the part’s front edge Y0; the operation is the same as X: approach the front edge with the edge finder, stop at the reaction point, account for the edge-finder radius, select the Y line on the G54 screen, apply MEASURE/calculation with Y0, and check the resulting G54 Y value. After X and Y zeros are set, you can move the tool center to X0 Y0 and visually compare with the part corner — but this move must be done at a safe Z height.
13. Making the part center X0 Y0
If the program zero is the part center rather than a corner, two edges are measured. On X, the left and right edges are measured and the center is (X left + X right) / 2; on Y, (Y front + Y back) / 2. The found center values are saved to G54 X and Y. Some M70 machines have a center-calculation function (its name varies by builder).
📷 IMAGE AREA — M70 WORK OFFSET (G54) screen: X/Y/Z fields and saving a value with MEASURE
Recommended size: 1200×675 px (16:9) · WebP/JPG · <150 KB · filename: mitsubishi-m70-g54-work-offset-screen.webp · alt: Mitsubishi M70 WORK OFFSET G54 screen X Y Z and MEASURE
14. Setting the Z part zero by touch
We will make the part’s top face Z0; here the tool length compensation and the part Z zero must work correctly together. For the Z zero you can use a reference tool, the cutter to be used, a precise gauge, paper, a Z-setting block or a touch measuring device. Step 1: call a tool whose length is measured (e.g. T1, its length saved to H1) and check it is really T1 in the spindle. Step 2: at a safe position, per the machine procedure, activate G43 H1 via MDI (on some machines with Z, G43 H1 Z100.) — only at a safe distance and with the correct H number checked. Step 3: in HANDLE mode place paper/gauge/setting block between tool and part and lower slowly; stop when the paper is lightly pinched or the gauge is touched.
Step 4 – account for the gauge thickness: if the tool touched the part directly, Z0; if there is a 10 mm gauge, the tool tip is 10 mm above the surface and the measurement value is entered as Z10.; if 0.10 mm paper is used, Z0.10 can be accounted for. Step 5: go to the Z field on the G54 screen; if you touched the part top directly enter Z0, with a 10 mm gauge enter Z10. and press MEASURE/INPUT C or the panel’s measure key. The control computes the G54 Z shift accounting for the tool length compensation. The programming manual states that when setting the workpiece coordinate system, the tool’s current position includes the tool length and other active offsets.
15. Alternative: setting Z with a reference tool
In some shops all tools are measured against a separate fixed surface, then the part Z zero is set using only one reference tool: all tools are measured against the same measuring surface and their lengths saved to the H fields → the reference tool is called → G43 and the correct H are activated → the reference tool is touched to the part top → G54 Z is measured. After this, the other tools also use the same part Z0 surface correctly thanks to their own H values.
16. Wrong method: changing G54 Z for each tool
The G54 Z value is not changed separately for each tool. Correct system: the part’s Z zero → G54 Z; the tool lengths → H1, H2, H3. Wrong system: change G54 Z when T1 is loaded, change it again for T2… This method breaks the program and compensation scheme. G54 belongs to the part; the H values belong to the tools.
17. When are G55–G59 used?
If more than one part is clamped on the same table, different zeros can be used: G54 → the part in the first vise, G55 → the second vise, G56 → the part in a fixture. If G54 is selected in the program the G54 values are used, if G55 is selected the G55 values are used. On the M70 there are six basic workpiece coordinate systems, G54–G59; optionally, additional coordinate systems can be used with G54.1.
18. Checking the entered zeros and a safe MDI trial
After the tool and part values are entered, do not go straight to cutting. Tool check: does T1 really use H1, are the lengths reasonable, was a value written to the wrong H line? G54 check: is X0 on the correct edge, is Y0 on the correct edge, is Z0 on the part top, does the program use G54, are the edge-finder radius and gauge thickness correct? When checking the part zero, keep the tool at a safe Z height first; e.g. with the correct tool and H, G54 G90 G0 X0 Y0 can be used, but Z must be at a safe position first. For the Z check the tool is not sent straight to Z0 at rapid; first a safe height like G54 G90 G0 Z50. is selected, then the surface is approached in HANDLE/low feed.
19. Simple check program
To try the entered zeros, the moves must be checked at a safe distance. The following is only an example check structure; on a real machine the tool-change command, safe Z, spindle command and program number must be changed to suit the machine. The manual requires checking the program, tool offsets and workpiece offsets with a dry run before starting actual machining.
O9000
G21 G17 G90
G40 G49 G80
G54
T1 M6
S500 M3
G0 X0 Y0
G43 H1 Z50.
M5
G49
M3020. Using the tool wear value
When the tool length needs a small correction, instead of constantly changing the main geometry value, the Wear field can be used. For example if the part came out 0.05 mm thick and 0.05 mm more must be removed in Z, a small wear correction can be made in the right direction; but the sign direction must be checked against the machine’s compensation scheme. The tool screen may show GEOMETRY, WEAR, LENGTH, RADIUS fields — the large tool length is held in Geometry, small corrections in Wear.
21. Common mistakes
- Wrong H number: using H1 while T2 is loaded can cause a Z collision.
- Z move without G43: the tool length may not be accounted for.
- Selecting G55 instead of G54: the program uses a different part zero.
- Forgetting the edge-finder radius: the X/Y zero is off by the radius.
- Not accounting for the gauge thickness: the Z zero is off by the gauge thickness.
- Confusing tool length with G54 Z: the length goes in the H field, the part Z zero in the G54 Z field.
- Writing a value to the wrong axis or setting a zero without a reference return: the machine coordinates may not be reliable.
22. End-to-end application sequence
A. Tool lengths: send the machine to reference → clamp the part → decide the measuring surface → call T1 → touch the surface in HANDLE → open OFFSET/TOOL OFFSET → select H1 → save with MEASURE/INPUT → retract to a safe Z → measure the other tools against the same surface → check the H values. B. X–Y part zero: mount the edge finder → approach the X zero edge → account for the radius → open WORK OFFSET/G54 → measure and save G54 X → approach the Y edge → account for the radius → measure and save G54 Y. C. Z part zero: call the reference tool whose length is measured → activate the correct G43 H → touch the part top/gauge → select G54 Z → Z0 on direct touch, enter the gauge thickness with a gauge → save with MEASURE/INPUT → retract to a safe Z. D. Final check: does the program use G54 → T–H matches → go to X0 Y0 at safe Z → check at a safe height like Z50 → turn on SINGLE BLOCK → lower Feed/Rapid Override → try the program dry/at a safe distance.
23. Summary
In this guide we learned the difference between machine zero / tool zero / part zero; that tool lengths are written in the H field and diameter/radius in the D field; that G43 activates length compensation and G49 cancels it; the G54–G59 workpiece coordinates; setting X–Y with an edge finder and Z from the part top; accounting for the gauge thickness; and safely checking the tool and part zeros.