Industry Information

How to avoid the safety problem of machining center in use

How to avoid the safety problem of machining center in useHow to avoid the safety problem of machining center in use

As China becomes a large CNC machining country, the technical requirements for machining centers are becoming higher and higher, and the machining centers are not as unfamiliar as in the early stages of imported processing. There are more and more users using machining centers, even many operators There is not much operating experience. The feed rate of the CNC machining center has increased from 16m / min in the 1980s to the current 24 ~ 40m / min. The spindle speed has also increased from 2500r / min to the current 6000 ~ 40,000r / min. . Under such circumstances of high speed and structure, once due to programming and operation errors, the operator has no time to press the emergency stop button, the tool has collided with the workpiece. In order to avoid machine tools and personal accidents, the following measures can be taken during programming and operation / (take FANUC system as an example).

1. The origin of the workpiece coordinate system set by the programmer during programming should be outside the workpiece blank, at least on the workpiece surface.

Under normal circumstances, the origin of the workpiece coordinate system can be set anywhere, as long as this origin has a certain relationship with the origin of the machine coordinate system. But in actual operation, if the command value is zero or close to zero, the tool will point directly to the position of zero or close to zero. During milling, the tool will run towards the table or fixture base: during turning, it will run toward the chuck base. In this way, the tool will penetrate the workpiece and point directly at the reference plane. At this time, if it moves fast, an accident must occur.

FANUC system general setting: when the decimal point is omitted, it is the minimum input unit, usually µm. When the decimal point is omitted, the input value will be reduced by one thousandth, and at this time, the input value will be close to zero. Or, for other reasons, the tool should have left the workpiece but actually did not leave the workpiece and entered the workpiece. When this happens, the zero point of the workpiece coordinate system should be set outside the workpiece or on the base surface of the table / (or fixture /), and the result will be different.

2. Programmers and operators must be careful about decimal points when writing programs.

The FANUC system is the smallest setting unit when the decimal point is omitted, while most domestic systems and some systems in Europe and America, when the decimal point is omitted, is mm, which is the calculator input method. If you are used to the calculator input method, there will be problems on the FANUC system. Many programmers and operators may use both systems. To prevent the size from being reduced due to the decimal point, the decimal point should also be added to the program in the calculator input method. Doing so is superfluous for certain types of systems, but after you get into the habit, there will be no problems with the decimal point.

In order to make the decimal point eye-catching, the isolated decimal point is often written in the form of “.0” when programming. Of course, when the system is executed, the zero after the decimal point of the value is ignored.

3. When adjusting the workpiece coordinate system, the operator should set the reference point outside the physical / (geometric /) length of all tools, at least on the tool point of the longest tool.

For the workpiece coordinate system on the workpiece installation drawing, the operator obtains it by setting the offset of the machine coordinate system on the machine tool. That is, the operator sets a reference point on the machine tool, finds the size between this reference point and the zero point of the workpiece coordinate system set by the programmer, and sets this size as the workpiece coordinate system offset.

On a lathe, the reference point can be set at the center of rotation of the tool post, the tip of the reference tool, or another position. If no additional motion is added, the zero commanded by the programmer is the reference point of the tool holder / (machine tool /) moved to the offset zero position. At this time, if the reference point is set at the rotation center of the tool post, the tool post must collide with the workpiece. In order to ensure no collision, the reference point on the machine tool should be set not only outside the tool holder, but also outside all the tools. In this way, even when the tool holder is equipped with a tool, the reference point will not collide with the workpiece.

On a milling machine, the reference points of the X and Y axes are on the spindle axis. However, the reference point of the Z axis can be set at the spindle end or at a point outside the spindle end. If it is at the spindle end, when the command is zero, the spindle end will reach the zero position specified by the coordinate system. At this time, the key on the end of the spindle will collide with the workpiece: if a tool is installed on the spindle, it will collide with the workpiece. To ensure that there is no collision, the reference point on the Z axis should be set beyond all tool lengths. Even if no other movement is added, the reference point will not hit the workpiece.

4. When adjusting the tool length offset, the operator should ensure that the offset value is a negative value.

When the programmer instructs the tool length compensation, the T code command is used for turning, and the G43 command is used for milling, that is, the tool length offset value is added to the command value. In the direction of the machine tool coordinate axis, the direction of the tool moving away from the workpiece is specified as positive, and the direction of the tool moving closer to the workpiece is negative. The operator adjusts the tool offset value to a negative value to instruct the tool to move to the workpiece. When the commanded tool approaches the workpiece in the program, in addition to the commanded value, the offset value of the tool is added. This additional value is moved toward the workpiece. At this time, in case this value is missed, the tool will not reach the target point.

To make the tool offset value a negative value, when specifying the reference point on the machine tool, it must be set beyond all tool lengths, at least at the tool position / (point /) point of the reference tool.

5. When canceling the tool length offset / (compensation /), the tool should be outside the workpiece.

Sometimes, the tool length offset should be canceled during machining. For example, in the machining center, if G28, G30 and G27 commands are issued, the machine tool returns to the tool change point for automatic tool change. In order to ensure that the tool change position is accurately reached, the tool length offset should be canceled in the command, such as G30Z-G49: where, Z- is the intermediate point of the tool movement. When the tool reaches the intermediate point, the tool length compensation must be canceled. If this intermediate point is not selected properly, the tool tip may not leave the workpiece, or it may move toward the workpiece instead, and an accident may occur at this time. During programming, the tool length is generally not determined. If the value of the command is not enough to move the tool tip away from the workpiece, danger will occur. In this case, incremental value programming should be used so that the incremental value is greater than all tool length compensation values. If the tool length compensation value is 200mm, command G30 G49 G91 Z200.0. If you set the reference point on the machine tool and adjust the tool length offset / (compensation /) according to the method suggested above, the tool tip must be far from the workpiece as long as the command point is outside the workpiece.

6. Tool number and tool compensation number should be easy to check.

The tool number is commanded by T code, and the compensation number is set by the operator in the system offset data area. The turning system uses a T code plus 2 or 4 digits. Among them, the high digit specifies the tool number and the low digit specifies the tool compensation number. In the milling system, the tool number is commanded by the T code, the tool length compensation is commanded by the H code, and the radius is commanded by the D code, and the H and D codes use the same set of data, and the tool number and the compensation number are independent of each other. , The programmer can designate independently.

In order to facilitate verification and setting, except for special purposes, the tool number and compensation number of the turning system are preferably the same, for example: T11 or T101. That is, the No. 1 tool uses the No. 1 compensation value. The milling system uses T1 to call the tool, H1 to call the tool length compensation value, and D21 to call the tool radius compensation value / (if there are less than 20 tools /). That is, the No. 1 tool uses the No. 1 length compensation value and the No. 21 radius compensation value, which is convenient for programming and setting operations, and also easy to remember to reduce the probability of errors.

7. When contour milling, lift the tool after the tool leaves the contour surface of the workpiece.

When contour milling, make the tool leave the contour surface of the workpiece and then lift the tool. In addition to not leaving a mark on the contour, you can also develop good habits to avoid accidents in other situations.

At present, the CNC system provides many functions of the inspection program. Under normal circumstances, programming and setting errors can be checked out. With the measures suggested here, even if the inspection fails, it will not cause an accident.

Leave a Reply