📷 IMAGE AREA — M70 OFFSET screen: Length/Radius, Geometry and Wear fields and dimensional correction
Recommended size: 1200×630 px (16:9, hero) · WebP/JPG · <150 KB · filename: mitsubishi-m70-tool-offset-screen.webp · alt: Mitsubishi M70 OFFSET screen tool length radius geometry wear
In this guide we cover how tool length and tool radius compensations are used on the Mitsubishi M70 control, the difference between Geometry and Wear, and how to make small corrections based on the measurement result. The topic focuses only on the panel and offset screens.
1. What is tool compensation?
Tool compensation lets the control account for the tool’s real length and diameter. The tools used in the same program can have different lengths, different diameters and different wear as they are used; these differences are saved to the tool offset table. Two compensations are basically used: H tool length compensation, D tool radius/diameter compensation. E.g. T1→H1 and D1, T2→H2 and D2, T3→H3 and D3.
2. Two offset types on the M70 (Type 1 / Type 2)
The Mitsubishi programming manual explains two systems for tool compensation: Type 1 and Type 2. This must not be confused with Program Restart Type 1/Type 2. Offset Type 1: a single common compensation value is used for the same number (H1 = the same value, D1 = the same value); length, radius, shape and wear values may not be kept separately — simpler, but the Geometry/Wear separation is limited. Offset Type 2: the values can be kept in separate fields (tool length Geometry, tool length Wear, radius Geometry, radius Wear). The total used by the control: H = Length Geometry + Length Wear, D = Radius Geometry + Radius Wear. Type 2 is more useful for dimensional correction in mass production.
3. The difference between Geometry and Wear
Geometry is the tool’s main dimension; the tool’s measured length, real radius and the main value tied to its real diameter are entered here (e.g. tool length Geometry −452.630, radius Geometry 5.000). The Geometry value is updated when the tool is first measured or fully changed. Wear is used to record the tool’s wear or a small dimensional correction (e.g. length Wear −0.020, radius Wear +0.010). The Wear field usually holds small values (0.010, −0.020, 0.050); if a very large value of several millimeters is seen, the possibility of a wrong entry must be checked.
4. Tool length compensation: the H value
Tool length compensation is usually activated with G43 and the H address: T2 M6 → G43 H2 Z50.. Here T2 is the second tool, H2 the second tool’s length offset, G43 activates positive tool length compensation, and it moves to Z50 with the compensation applied. To cancel, G49 or in some cases H0 is used. The manual states that when H0 is given, tool length compensation is cancelled and the H number selected with G43/G44 can be kept modal.
5. Tool radius compensation: the D value
Tool radius compensation is used with G41 D... or G42 D... in the program (e.g. G41 D2 X20. Y10.); the control uses the radius value in D2. G41 applies compensation to the left of the programmed travel direction, G42 to the right; G40 cancels radius compensation. The Mitsubishi manual states that in radius compensation only the D number is valid and the H command is not considered.
6. Entering the OFFSET screen
The menu name may vary by machine, but the general path is OFFSET → TOOL OFFSET → LENGTH/RADIUS → GEOMETRY/WEAR. On screen you may see these fields:
| Field | Function |
|---|---|
| Length Geometry | Main tool length |
| Length Wear | Small correction for length |
| Radius Geometry | Main radius value |
| Radius Wear | Small correction for diameter/radius |
On some machines H and D are in a separate table, on others they are shown on the same line.
7. Dimensional correction in tool length (Length Wear)
For example the Z dimension in the program should be 20.00 mm but the part measured 20.05 mm; the part is left 0.05 mm high, so 0.05 mm more material must be removed by the tool. In that case a small correction suited to the machine’s compensation direction is entered in the tool length Wear field (e.g. H2 Length Wear: -0.050). But the sign direction can vary by the machine’s axis/compensation scheme; use a small value on the first correction and re-measure the result. Basic logic: if the part is left high the tool must go a bit lower; if the part came out too thin the tool must stay a bit higher — but which physical direction the plus/minus entry affects on the panel must be verified on the real machine with a small trial.
8. D correction in diameter or slot dimension
For example on an externally machined part the target is 50.00 mm and the measured is 50.04 mm; the part is left 0.04 mm large. If a total of 0.04 mm reduction is needed in diameter, the tool path must be changed radially by ~0.02 mm — because diameter difference / 2 = radial correction (0.04 / 2 = 0.02 mm). A +0.020 or −0.020 correction may be needed in the D Wear field depending on the program direction. Here the G41/G42 direction, the inner/outer contour and the tool-path direction matter; the sign must not be memorized — make a small correction and re-check the dimension.
9. Dimensional correction in an inner pocket
Example: the target pocket is 40.00 mm and the measured is 39.96 mm; the pocket is left 0.04 mm small. For the pocket width to grow by 0.04 mm, the tool center must shift ~0.02 mm outward on each side (radial correction 0.04 / 2 = 0.02 mm). But on an inner contour the effect of the D Wear sign can appear opposite to an outer contour; this is because of the G41/G42 direction and which side of the contour the tool moves on.
10. Should Geometry or Wear be changed?
Use Wear when: there is a small dimensional difference on the part, the tool has worn over time, a correction of a few microns/percent is needed, or the dimension must be corrected gradually in mass production. Use Geometry when: a new tool is fitted, the tool length is re-measured, a tool of a completely different length is fitted, or a wrong main tool value is being corrected. Constantly changing the Geometry value for small dimensional corrections is not a good tracking method.
11. The Wear value when a new tool is fitted
When a worn tool is removed and a new tool fitted, the old Wear value must be checked. For example the old tool may have Length Wear −0.080; if this value is left when the new tool is fitted, the control applies the old wear correction to the new tool too. General procedure: measure the new tool’s Geometry, check the old Wear value, zero the Wear if needed, and make a small correction again based on the first measurement.
12. How is a compensation value entered?
General sequence: (1) Open the OFFSET screen. (2) Find the correct tool number. (3) Select the Length or Radius section. (4) Select the Geometry or Wear column. (5) Type the correct value. (6) Save with INPUT. (7) Re-check the entered value. On some screens: INPUT writes the new value over the old one; +INPUT adds to the existing value; CALC changes the current value by calculation; MEASURE computes a new value from the current machine position. The behavior of the keys must be checked against the machine builder.
13. Changing compensation during automatic operation
The Mitsubishi programming manual states that if the tool compensation amount is changed during automatic operation (including a Single Block stop), the new value may take effect from the next or a later block. So when compensation is changed while the program is active: do not assume the current move will change immediately, check from which block it takes effect, remember the same block may need to be restarted, and do not make large corrections. The safest method is to make the compensation change at a suitable stop point and watch the next move carefully.
14. Checking the H and D numbers
The tool and the offset number in the program do not have to be the same; for example T2 M6 → G43 H12 Z50. → G41 D22 X... is technically possible (tool T2, length offset H12, radius offset D22). But to reduce confusion for the operator, the T2 → H2 → D2 match is usually preferred. The machine’s programming scheme must be checked.
15. Common mistakes
- Changing the wrong tool line: T2’s Wear value may be changed instead of T3.
- Changing Radius instead of Length: the D value may be changed when the Z dimension was to be corrected.
- Changing Wear instead of Geometry (or vice versa): the main tool dimension can be spoiled for a small correction.
- Decimal error: correct 0.020, wrong 0.200 or 2.000.
- Writing the whole diameter difference into D: if there is a 0.04 mm difference in diameter, the radial correction is usually 0.02 mm.
- Not checking the plus/minus direction: the dimensional error can grow further.
- Leaving the old Wear value on a new tool: the new tool may run with the wrong compensation.
16. Short application example and summary
Suppose the surface machined with tool T4 is left 0.03 mm high. General sequence: (1) Check which H number T4 uses in the program. (2) Open the OFFSET screen. (3) Find the relevant H line. (4) Go to the Length Wear column. (5) Note the current Wear value. (6) Make a small 0.03 mm correction in the needed direction. (7) Save with INPUT. (8) Re-check the value. (9) Measure the next part. (10) Make a small extra correction per the result. Advancing gradually is safer than making a large correction on the first try. In summary, in this guide we learned the difference between the H and D compensations, the Offset Type 1/Type 2 system, the Geometry and Wear fields, the use of G43/G49/G40/G41/G42, Length Wear correction for Z, the radial-correction calculation for diameter, checking the old Wear on a new tool, and that a change made during automatic operation can take effect in later blocks.
📷 IMAGE AREA — Diameter difference / 2 = radial correction diagram, and a Length Wear Z-dimension correction example
Recommended size: 1200×675 px (16:9) · WebP/JPG · <150 KB · filename: mitsubishi-m70-radial-correction-wear.webp · alt: Mitsubishi M70 diameter difference radial correction and length wear dimensional correction