After the program is input into the CNC system and verified, can the operator start the CNC lathe to process the workpiece? No, after the parts are verified in order, the tool setting operation 

must be carried out, the cutting parameters must be reasonably adjusted, and the final processing program must be determined.

Tool setting method for external turning tool trial cutting

Machine tool coordinate system

The coordinate system established by the machine tool manufacturer with a fixed point of the machine tool as the coordinate origin is called the machine tool coordinate system.

According to the provisions of JB3051-82, the center line of the lathe spindle is the Z axis, the axis perpendicular to the Z axis is the X axis, and the direction of the turning tool away from the 

workpiece is the positive direction of the two axes.

The machine tool origin (machine tool zero point) is generally set at the intersection of the spindle centerline (i.e., the z axis) and the spindle mounting chuck surface.

The CNC device does not know the machine origin when it is powered on. In order to correctly establish the machine coordinate system when the machine is working, a machine reference 

point (measurement starting point) is usually set within the moving range of each coordinate bearing. When the machine is started, it must first be automatically or manually returned to the 

reference point to establish the machine coordinate system. The machine origin is actually determined by returning (or finding) the machine reference point.

Workpiece coordinate system

The reference point (zero point) determined by the user for compiling the machining program is called the workpiece origin. The workpiece origin of the CNC lathe is generally set as the 

intersection of the right end face of the part finishing and the axis centerline. The coordinate system constructed by the workpiece origin is called the workpiece coordinate system.

The x and z coordinate axes of the workpiece coordinate system are parallel to the x and z coordinate axes of the machine coordinate system and have the same direction.

Tool setting method

The role of tool setting is to find the relationship between the workpiece coordinate system and the machine coordinate system. In CNC turning, the machining origin of the part should be 

determined first to establish an accurate machining coordinate system, while considering the influence of different tool sizes on machining. These need to be solved by tool setting.

The process of trial cutting and tool setting

1. Clamp the workpiece and change the tool to be aligned to the current position of the tool holder.

2. In manual operation mode, start the spindle and use the current tool to test cut the outer circle of the workpiece within the machining allowance range. The length of the turning must be 

easy to measure. Do not move the X axis, withdraw along the positive direction of Z, and stop the spindle.

3. Measure the outer circle size Xa of the turning.

4. Press the "OFS/SET" key and the "Tool Offset" soft key under the CRT screen.

5. Press the soft key "Shape" under the CRT screen.

6. Move the cursor to the position corresponding to the tool number, enter "Xa", press the soft key under the CRT screen to measure, and generate the corresponding tool compensation value 

at the corresponding tool compensation position.

7. In manual mode, use the tool to turn the end face of the workpiece again. After turning the end face flat, withdraw along the positive direction of X, do not move in the Z direction, and stop 

the spindle.

8. Press the "OFS/SET" key to enter the "Shape" compensation setting interface, move the cursor to the position corresponding to the tool position number, enter "ZO", and press the soft key 

"Measure" under the CRT screen to generate accurate tool compensation values at the corresponding tool compensation position.