In this lesson we learn, step by step, how to perform tool zeroing with the reference-tool method on a vertical machining center equipped with a Mitsubishi M70/M700 control, and how to set multiple tools through the T-OFS page. In previous lessons we covered program management, running a program safely and restarting an interrupted program. This lesson focuses on one of the most critical stages of pre-machining setup: correctly teaching the control the Z-axis length relationship of your tools.
Tool zeroing errors are among the most common causes of crashes and scrapped parts, so it is important to follow the steps in this lesson in order and with care.
1. What is tool zeroing and why is it done?
On a CNC machining center, every tool has a different length. To move the Z values written in the program to the correct depth, the control must know either the length of each tool or the length difference between the tools.
Tool zeroing is the process of teaching the control the position of the tool along the Z axis relative to the workpiece surface. When this is done incorrectly, two typical results occur: the tool plunges deeper than expected and crashes, or the tool cuts in the air without ever touching the part.
2. The method used in this lesson: reference tool and the RELATIVE screen
Tool and workpiece zeroing on the M70/M700 can be done in several ways. In this lesson we explain the reference-tool method, which is widely used on the shop floor. The logic of the method is as follows:
- One of the tools is chosen as the reference tool.
- The reference tool is touched on the workpiece surface, and that point is taken as Z zero on the RELATIVE (relative position) screen.
- The workpiece Z zero is written with EASYSETTING, based on the reference tool.
- The length difference of every other tool relative to the reference tool is read from the RELATIVE screen and entered on the T-OFS page.
In this method the measured value is not the absolute length of the tool but the length difference relative to the reference tool. Knowing this distinction is important for interpreting the values on the T-OFS page correctly.
3. Preparation and safety before starting
Check the following before starting the zeroing procedure:
- The workpiece must be firmly clamped in its workholding (vise, clamps, fixture).
- The surface to be touched must be clean, free of chips, burrs and pooled coolant.
- Axis movements should be made in handle mode with a low multiplier (x10 or x1).
- When approaching the surface, always use the lowest multiplier for the final distance.
Never use rapid traverse while touching the tool on the surface.
4. Choosing the reference tool
The reference tool is the tool against which the length difference of every other tool will be measured. In practice, a tool that stays permanently in the magazine and whose length does not change is usually chosen as the reference. Keep the following in mind:
- Do not use a tool that wears quickly or is changed frequently as the reference.
- If the reference tool is replaced, the length differences of all tools must be measured again.
5. Touching the reference tool on the workpiece surface
Call the reference tool into the spindle and, using the handwheel, slowly touch it on the top surface of the workpiece that is considered the finished surface.
To improve touch sensitivity you can use the paper method: place a thin sheet of paper on the surface and lower the tool until the paper moves with slight friction. For higher-precision work, prefer a Z-axis setter (dial-type presetter) or a tool length measuring probe.
6. SETUP → CNT SET: opening the RELATIVE POSN screen
Press the SETUP key on the panel and select CNT SET from the menu at the bottom of the screen. The RELATIVE POSN. (relative position) screen appears. This screen shows the relative position of the axes with respect to a chosen point and can be zeroed separately for each axis.
7. Zeroing the RELATIVE Z value
On the RELATIVE POSN. screen, move the cursor to the Z axis, type 0 and press INPUT. From this moment on, the point where the reference tool touched the workpiece surface is taken as Z=0 on the RELATIVE screen. All subsequent length-difference readings will be made from this point.
8. SETUP → COORD: writing the Z zero with EASYSETTING
Press SETUP, select COORD from the bottom of the screen and zero the Z axis with the EASYSETTING function.
EASYSETTING is a practical function that writes the current position into the selected workpiece coordinate system (for example G54) in a single operation. With this step, the surface touched by the reference tool is defined as Z0 in the workpiece coordinate system.
The screen layout and the details of the EASYSETTING steps may differ slightly depending on the control version and the machine builder’s panel configuration. When in doubt, refer to the instruction manual of your own machine.
9. If you are working with a single tool: check and test
If your program uses only one tool, zeroing is complete at this point. Even so, before machining:
- Check on the COORD screen that the Z value was written as you expect.
- Retract the tool to a safe height.
- Test the program first with graphic check (CHECK), then in single block at a low feed rate.
10. The logic of multi-tool zeroing
Real jobs use more than one tool in a single program: a roughing mill, an end mill, a drill, a tap and so on. Since every tool has a different length, the length differences relative to the reference tool must be taught to the control.
The logic is this: when the reference tool touched the surface, RELATIVE Z was set to 0. When another tool is touched on the same surface, the Z value read on the RELATIVE screen is that tool’s length difference relative to the reference tool. This value is entered on the T-OFS page next to the corresponding tool number.
11. Calling the next tool (tool change via MDI)
Switch to MDI mode, type the tool change command on the MDI screen (example: M06 T2), confirm the line with INPUT and execute it with START.
Note: On some machines the tool change line is written in the order T2 M06. The processing order of T and M06 on the same line depends on the machine builder’s PLC. Check your own machine’s instruction manual to see which format applies.
12. Touching the tool on the surface and noting the RELATIVE Z value
Slowly touch the new tool with the handwheel on the same surface where the reference tool was touched, and note the Z value shown in the RELATIVE section of the CNT SET screen.
This value can be positive or negative. If the tool is longer than the reference tool the difference reads in one direction; if shorter, in the other. Note the value exactly as displayed, including its sign — do not change the sign.
13. Entering the length difference on the T-OFS page
Press SETUP, open the T-OFS (tool offset) page from the bottom of the screen and enter the noted Z value next to the corresponding tool number.
Repeat the same procedure for every other tool used in the program: call the tool, touch it on the surface, read the RELATIVE Z value and enter it on the T-OFS page.
The column layout of the T-OFS page (length, wear, radius) can vary depending on the tool compensation memory type of the machine. Make sure the length difference is entered in the length (geometry) column.
14. Critical rule: the reference tool must read 0 on the T-OFS page
The length value of the reference tool on the T-OFS page must be 0. The workpiece Z zero has already been written based on the reference tool. If a length value is also entered for the reference tool, the compensation is applied twice and the tool moves to a position that is wrong by exactly that amount. This is the most dangerous mistake made with this method.
15. Verifying the entered values and a safe first run
After all tools are set, perform these checks before starting the job:
- Compare the value of every tool on the T-OFS page against the list you noted.
- Double-check that the reference tool’s value is 0.
- For each tool, call it via MDI and command a Z move at a safe height while watching the remaining distance on the screen.
- Run the program first in graphic check (CHECK), then in single block mode with a low feed override.
- On the first part, verify the critical depths with a caliper or micrometer.
16. Common mistakes
- Not leaving the reference tool’s T-OFS value at 0.
- Touching the other tools before RELATIVE Z has been zeroed.
- Entering the length difference with the wrong sign (+/−).
- Touching different tools on different surfaces; all tools must be touched on the same reference surface.
- Chips or burrs on the touching surface.
- Entering the value against the wrong tool number on the T-OFS page.
- Touching with a worn or chipped tool.
- Replacing the reference tool without updating the length differences of the other tools.
17. Quick procedure summary
- Touch the reference tool on the workpiece surface.
- SETUP → CNT SET → on the RELATIVE POSN. screen move to the Z axis, 0 INPUT.
- SETUP → COORD → zero the Z axis with EASYSETTING.
- Call the next tool via MDI (e.g. M06 T2 → INPUT → START).
- Touch the tool on the same surface and note the RELATIVE Z value.
- SETUP → enter this value against the corresponding tool number on the T-OFS page.
- Repeat steps 4–6 for the remaining tools.
- Check that the reference tool’s T-OFS value is 0.
- Do a safe trial with graphic check, single block and low feed.
18. Lesson summary
In this lesson we learned tool zeroing with the reference-tool method on the Mitsubishi M70/M700 control. The reference tool was touched on the workpiece surface, RELATIVE Z was zeroed on the CNT SET screen, the workpiece Z zero was written with EASYSETTING, and the length differences of the other tools relative to the reference tool were read from the RELATIVE screen and entered on the T-OFS page. The most critical rule of the method is that the reference tool must remain at 0 on the T-OFS page. See you in the next lesson.