5 Axis Cnc System

The CNC machine tool with five-axis function can realize the relative movement between the workpiece and the tool in a variety of postures. On the one hand, it can maintain a better machining posture of the tool, avoid the extremely low cutting speed of the tool center, and also avoid the tool, workpiece, and fixture. Interference between the two to achieve a larger machining range within a limited stroke. The five-axis function is also an important indicator to measure the capabilities of the CNC system.

Workpiece Coordinate Rotation

For a five-axis machine tool with a turntable structure, the workpiece is consolidated with the rotary table, that is, the workpiece coordinate system (WCS) is consolidated with the rotary table. When the worktable is rotated, the workpiece coordinate system (WCS) must be rotated accordingly. After that, the X, Y, Z directions of the workpiece coordinate system are no longer consistent with the original machine tool coordinate system (MCS) XYZ directions. The five-axis interpolation algorithm needs to automatically complete the rotation of the workpiece coordinate system at any time to ensure the correct tool running path.

Since the workpiece coordinate system rotates with the turntable, the CNC system provides the user with the opportunity to choose the machine tool coordinate system MCS or the workpiece coordinate system WCS in the manual operation mode. If the user selects the manual operation under WCS and the WCS has been rotated, the manual operation will move in the direction of the rotated coordinate axis. Take the C-axis turntable as an example: if the C-axis has been rotated from the initial 0 degree, after the CCW has rotated 45 degrees , The user selects the manual X axis under WCS, the CNC machine tool will link the XY axis, and follow the 45-degree diagonal line on the XY plane, as shown in Figure 2. The above behavior is very convenient for the workpiece edge seeking and manual positioning machining. It does not need to consider how many degrees the turntable has turned, as long as the operation is based on the direction shown in the workpiece coordinate system on the drawing. In the automatic machining mode, all G92, G54-G59, and G52 are set under WCS, and they will rotate with the rotation of WCS.

It is worth noting in automatic machining: If the user is programming in the workpiece coordinate system, before pushing the tool, it is recommended that the user use G53 to return to the MCS, and then execute the tool retract action according to the MCS coordinate system; otherwise, it is necessary to clarify the current angle relationship between WCS and MCS. For example: when the C axis is 0 degrees and the WCS coordinate system is 180 degrees, the direction of the WCS coordinate system is exactly the opposite. The starting position C of the feed is 0 degrees, and the XY is the positive value of the WCS, the position C is 180 degrees when the tool is retracted, and then back At the starting point, it will return to the negative value of the WCS absolute value.

For machine tools with a pendulum head structure, the five-axis CNC system only focuses on the coordinates of the control point (the center of rotation of the pendulum head) in the machine coordinate system MCS, while the five-axis CNC system controls the tool tip point coordinates in the workpiece coordinate system WCS. as the picture shows. Combined with the rotation of the WCS with the turntable, the CNC system controls the behavior so that the relative positional relationship between the tool and the workpiece is always correctly reflected under the WCS. The user can safely compare the workpiece drawing and consider the workpiece programming under the WCS without considering the machine tool structure.

RTCP

In five-axis machining, whether it is tool rotation or turntable rotation, the tool tip point generates additional XYZ movement. The five-axis numerical control system can automatically compensate for the displacement between the workpiece and the tool nose point caused by these rotations and swings, which is called RTCP (rotation around the tool nose point) control function. For example, Dalian Koyo’s GNC61 uses G203 to activate this function; in Siemens 840D, TRAORI is used to turn on RTCP; in Heidenhain TNC530, M128 is used to turn on RTCP. In this way, the user can program on a five-axis machine tool like a 3-coordinate, and can add rotation instructions for adjusting the posture adjustment between the tool and the workpiece at the right time, without considering the additional movement caused by these rotation instructions.

Tool Vector

In five-axis programming, it is recommended to use the attitude vector of the tool relative to the workpiece coordinate system (WCS) to express the attitude relationship between the workpiece and the tool. The result of this machining is that the user does not have to consider the specific type and structure of the five-axis machine tool. The same workpiece program can be processed on different types of five-axis machine tools. All coordinate machining related to the machine tool structure is completely automatically completed by the five-axis CNC system.

For example, 840D uses (A3, B3, C3) to express the tool vector; Dalian Guangyang’s GNC61 uses (VX, VY, VZ) to indicate the attitude of the tool tip to the control point under WCS, right (VX, VY, VZ) There is no special requirement for vector length.

5-Axis Bevel Machining

According to statistics, in the world, five-axis machine tools are actually used for five-axis simultaneous machining only 5%, such as impellers, blades, aviation structural parts and other special parts; 73% are used for five-axis directional machining, such as V-engine cylinder blocks, Mold manufacturing, etc.; pentahedron machining accounts for 22%, such as box structure parts on machine tools.

The concept of Frames is used in 840D to describe the spatial slope and coordinate system.

The PLANE function is used in TNC530 to define the slope of the machining operation. For example: Use the space angle to define the inclined plane:

N50 plane spatial spa+27 spb+0 spc+45 … Spatial angle A: rotation angle SPA is rotating around the machine’s fixed X axis; space angle B: rotation angle SPB is rotating around the machine’s fixed Y axis; spatial angle C: rotation The angle SPC rotates around the fixed Z axis of the machine tool. In addition to the spatial angle definition, the TNC530 also supports a variety of spatial slope definitions such as projection angle, Euler angle, and three-point.

GNC61 has a G92 coordinate system under the workpiece coordinate system WCS, which is responsible for the overall offset of the user-defined coordinate system on it, and can be used to express the reference of the fixture. In the G92 coordinate system, the user can define the G54, G55, G56, G57, G58, G59 coordinate system, which can be used to express the respective coordinate systems of multiple workpieces under the same fixture reference. GNC61 has designed the program local coordinate system G52, which is located under G54-G59 and can be rotated and tilted arbitrarily. It is valid in the set machining program. Once a new program is loaded, G52 will be automatically cleared to 0. GNC61 supports the user to directly define G52 (spatial angle) in the program to specify an inclined coordinate system. In addition, GNC61 also provides built-in functions defined by other inclined coordinate systems, including:

SG52_EULER, specifies the G52 rotating coordinate system through Euler angles; SG52_2VEC, uses two vectors to define the machining plane; SG52_3PT, specifies the G52 rotating coordinate system through three points.

In addition, on the basis of defining the inclined plane, the five-axis CNC system also needs to support the automatic orientation of the tool to a posture perpendicular to the inclined plane. Heidenhain’s TNC530 has three machining methods: MOVE, TRUN, and STAY. In MOVE mode, when RTCP is turned on, the tool can be oriented automatically, that is, the tip of the tool will not move; in TRUN mode, the tool will be oriented automatically, but RTCP is not turned on, that is, the tool only swings without RTCP compensation movement; STAY means no Any movement is generated, but the corresponding required amount of movement is saved by system variables. In the automatic machining mode of Dalian Koyo GNC61, GNC61 supports two automatic tool orientation commands: G200 tool automatic vertical slope non-RTCP; G201 tool automatic vertical slope with RTCP.

Five-Axis Interpolation

Usually, the so-called five-axis CNC system adopts five-axis linear interpolation in the default state, that is, the ABC increment is equal to the linear increment for interpolation. Regardless of whether the RTCP five-axis linear interpolation is turned on or not, the side edge of the tool is not directly restricted, which may cause the size and shape of the part formed by the side edge to not meet the requirements. For this reason, CNC manufacturers often support special five-axis interpolation for other constrained side edges.

1. Plane knife vector interpolation

In the blanking die, there are a large number of requirements for the sidewall to maintain a flat surface; there are also a large number of cavity milling machining requirements for the slope of the side wall in aerospace thin-walled structural parts; the welding groove of the welded parts also has the requirement of milling the sloped surface. 840D provides ORIVECT and G213 of GNC61 are all the above functions. Usually this function automatically starts RTCP.

2. Double spline constraint interpolation

Namely, specify the spline curve of the tool tip point, and then another spline curve that constrains the tool, the CNC system will complete the interpolation of the ruled surface constrained by the two splines. 840D provides ORICURVE, as well as G6.3X provided by GNC61 to achieve the above functions.

3. Conical interpolation

Specify the tool vector to run along a specific cone surface. This interpolation function is suitable for machining the conical transition surface between the cone and the space slope. ORICONCW\ORICONCCW\ORICONIO\ORICONTO provided by 840D completes the above functions.

Spatial Tool Radius Compensation

For five-axis machining, RTCP plays the role of tool length compensation. The five-axis tool radius compensation can adjust various types of tools without modifying the coordinates of the workpiece surface in the five-axis machining program to ensure the correct surface shape of the workpiece. Both FANUC’s most advanced 30i series CNC system and Siemens’ high-end 840D system support the above functions.

In five-axis machining, due to the opening of RTCP and various special five-axis algorithms, such as plane vector interpolation, double spline constraint interpolation, etc., it may cause fluctuations in the speed of each linear feed axis. These fluctuations sometimes cause The vibration of the machine tool affects the surface machining quality of the parts, which exceeds the allowable range of the machine tool. For this reason, the five-axis CNC system needs to smoothly adjust the speed of each axis. At present, FANUC’s most advanced 30i series CNC system and Siemens’ high-end 840D system support the above functions.