1. Z-direction tool setting of machining center
There are generally three methods for the Z-direction tool setting of the machining center:
1) On-machine tool setting method 1
This tool setting method is to sequentially determine the mutual positional relationship between each tool and the workpiece in the machine tool coordinate system through tool setting. The specific operation steps are as follows.
(1) Compare the tool lengths, find the longest tool as the reference tool, perform Z-direction tool setting, and take the tool setting value (C) at this time as the Z value of the workpiece coordinate system, at this time H03=0.
(2) Install the T01 and T02 tools on the spindle in turn, and determine the value of A and B as the length compensation value through tool setting. (This method does not directly measure the tool compensation, but it is different from method 3 through sequential tool setting.)
(3) Fill in the determined length compensation value (the longest tool length minus the remaining tool lengths) into the setting page. The positive and negative signs are determined by G43 and G44 in the program. At this time, it is generally expressed by G44H—. When G43 is used, the length compensation is a negative value.
This tool setting method has higher tool setting efficiency and precision, and less investment, but it is inconvenient to write process files, which has a certain impact on the production organization.
2) On-machine tool setting method 2
The specific operation steps of this tool setting method are as follows:
(1) ? The XY direction alignment is set as before, input the offset value for the XY item in G54, and set the Z item to zero.
(2) Replace the T1 used for processing with the spindle, use the block gauge to find the positive Z direction, read the Z item value Z1 of the machine tool coordinate system after the tightening is appropriate, deduct the height of the block gauge, and fill in the length compensation value H1.
(3) Install T2 on the spindle, use the block gauge to align it, read Z2, deduct the height of the block gauge and fill in H2.
(4) By analogy, align all the tools Ti with the block gauge, deduct the height of the block gauge from Zi and fill it in Hi
(5) When programming, use the following methods to compensate:
T1;
G91 G30 Z0;
M06;
G43 H1;
G90 G54 G00 X0 Y0;
Z100;
...(The following is the machining of the No. 1 tool until the end)
T2;
G91 G30 Z0;
M06;
G43 H2;
G90 G54 G00 X0 Y0;
Z100;
…(all processing contents of No. 2 knife)
...M5;
M30;
3) Off-machine tool preset + on-machine tool setting
This method of tool setting is to use a tool presetter outside the machine tool to accurately measure the axial and radial dimensions of each tool, determine the length compensation value of each tool, and then use the longest tool on the machine tool to perform Z To set the tool, determine the workpiece coordinate system.
This tool setting method has high tool setting accuracy and efficiency, which is convenient for the preparation of process documents and production organization, but the investment is large.
2. Input of tool setting data
(1) The tool setting data obtained according to the above operations, that is, the X, Y, Z values of the origin of the programming coordinate system in the machine tool coordinate system, must be manually input into G54~G59 for storage. The operation steps are as follows:
①Press【MENU OFFSET】key.
②Press the cursor key to move to the workpiece coordinate system G54～G59.
③Press【X】key to input X coordinate value.
④Press【INPUT】key.
⑤Press【Y】key to input Y coordinate value.
⑥Press【INPUT】key.
⑦Press【Z】key to input Z coordinate value.
⑧Press【INPUT】key.
(2) The tool compensation value is generally input into the machine tool by MDI (manual data input) method before program debugging. The general operation steps are as follows:
①Press【MENU OFFSET】key.
②Press the cursor key to the compensation number.
③Enter the compensation value.
④Press【INPUT】key.
3. Trial cutting method
The trial cutting method is a simple tool setting method, but it will leave traces on the workpiece and the tool setting accuracy is low. It is suitable for tool setting during rough machining of parts. The tool setting method is the same as that of the mechanical edge finder.
4. Leverage dial indicator for knife setting
The tool setting accuracy of the lever dial indicator is high, but this method of operation is more troublesome and less efficient.
The tool setting method is as follows: use the magnetic watch seat to attract the lever dial indicator on the main shaft of the machining center, so that the watch head is close to the hole wall (or cylindrical surface), when the watch head rotates for one week, the beating amount of its pointer is within the allowable tool setting. Within the error, such as 0.02, at this time, it can be considered that the rotation center of the spindle coincides with the center of the hole to be measured, and input the X and Y coordinate values in the machine coordinate system at this time into G54.
5. Tool setting in Z direction
Considering the manufacturability of tool setting, the upper surface of the workpiece is usually used as the origin of the Z direction of the workpiece coordinate system. When the upper surface of the part is relatively rough and cannot be used as the precision reference for tool setting, there is also a vise or worktable as the reference as the origin of the Z direction of the workpiece coordinate system, and then the workpiece height is corrected upward in G54 or the extended coordinate system. There are several methods for in-machine tool setting in Z direction, such as Z-direction measuring instrument setting, tool setting block setting and trial cutting method setting.
7. Z-direction measuring instrument for tool setting
The Z-direction measuring instrument has high tool setting accuracy, especially when many tools are set on the machine in the milling machining center, the tool setting efficiency is high, the investment is low, and it is suitable for single-piece parts processing.
1) Z-direction tool setting during single-tool machining in the machining center
The single-tool machining of the machining center is similar to that of the CNC milling machine without the problem of length compensation. The steps are as follows:
(1) Replace the tool that will be used for machining;
(2) Move the tool to just above the workpiece, measure the distance between the workpiece and the tool with a Z-direction measuring instrument, and record the Z-axis reading Z of the current machine tool (mechanical) coordinate system;
(3) The Z value is deducted from the height of the measuring instrument in the Z direction at this time (such as 50.03mm), and then the measured value is filled in the Z item of OFFSETSETTING-->Coordinate System-->G54;
(4) Run G90 G54G0 X0 Y0 Z100; check whether the alignment is correct