The structure of the DMU80P five-axis machining center is shown in Figure 1, with 3 linear motion axes (X, Y, Z) and 2 rotation axes (B, C). The swing head is the B axis, the swing range is 0 180 °, and the rotary axis is in the plane of the machine tool coordinate system G19, and the angle between the machine tool and the Y axis is 45 °;The C-axis rotation center is the Z-axis, the rotation range is 0 360° (unlimited), and the control system is SINUMERIK 840D SL. 
Fig.1 DMU80P machine tool structure DMU80P five-axis machining center has a 45° angle between the B axis and the Y axis, which belongs to the swing head non-orthogonal "variable shaft" machine tool, due to NX 110 There is no variable axis license, it does not support the programming of the variable axis machining toolpath, nor does it support the post-processing of the variable axis toolpath, and the post-processor developed based on the machine tool type and parameters cannot be used. At present, the programming methods of fixed shaft machining mainly include manual three-axis programming, manual "3+2" directional programming, CAM three-axis programming, and CAM "3+2" directional programming. For the five-axis machining center, the tool axis is oriented by 2 rotation axes, and no movement is done during the machining process, and the remaining 3 linear axes do feed movement. These 4 programming methods are actually in the category of three-axis programming, but in the three-axis CNC milling machine, the cutter axis attitude is constant, and in the five-axis machining center, 2 rotary axes are introduced, and the cutter axis attitude is variable. Therefore, the three-axis CNC milling machine, whether it is manual programming or CAM programming, belongs to the special "3+2" directional programming, as shown in Figure 2. 
Fig.2 Programming commonality 13.1. The orientation of the tool axis vector and the Z-axis of the workpiece coordinate system is consistent with the direction of the general three-axis machine tool workpiece coordinate system (the frame can be set) is obtained by the offset of the machine tool coordinate system, and the workpiece coordinates are x0 y0 z0;The establishment of the workpiece coordinate system of the five-axis machine tool can be obtained by the rotation transformation of the machine tool coordinate system through the rotation of two rotation axes, and the linear axis can be non-parallel to the linear axis of the corresponding mechanical coordinate system, and the z-axis of the workpiece coordinate system is perpendicular to the datum plane if the linear axis is used as the datum plane after the calibration plane. At this time, the tool axis vector is consistent with the Z-axis of the workpiece coordinate system, which can be regarded as the workpiece feature in the G17 plane of the workpiece coordinate system when there is no swing, and the three-axis programming mode can be directly adopted. 1.3.2 The orientation method of the forward inconsistency between the cutter axis vector and the Z-axis of the workpiece coordinate system needs to be realized by the transformation of the workpiece coordinate system, that is, the workpiece coordinate system is first made in the position of the z-axis forward space inclination plane in a mutually perpendicular position by the mode of "translation, rotation and translation", and then the three-axis machining of space is carried out. In the SINUMERIK 840D SL CNC system, the transformation of the coordinate system can be achieved by means of the programmable frame Trans (Absolute Zero Translation) Atrans (Incremental Zero Translation) and ROT (Absolute Coordinate Rotation) Arot (Incremental Coordinate Rotation) commands, or by means of a Cycle800 oscillating cycle. The advantage of the CYCLE800 cycle over the trans atrans and rot arot commands is that if the system is reset or powered off, the rotary frame can be maintained, which is convenient for retracting the tool along the tool axis, so the cycle 800 cycle command is better than the trans atrans and rot arot commands for the tool axis orientation in the inclined plane. To sum up, regardless of whether the tool axis vector is consistent with the Z-axis of the initial workpiece coordinate system, the tool axis in 3+2 directional machining is transformed based on the initial workpiece coordinate system (WCS), and has nothing to do with the machine tool coordinate system (MCS), that is, the transformation of the tool axis is completed by the machine tool numerical control system through the rotary data set, and has nothing to do with the machine tool structure, and the non-orthogonal swing head can be defined as an orthogonal structure in the post-processor creation, so as to adapt to the restriction of the CAM software without variable axis license. Using POST Builder, a post-processing construction tool from Siemens NX11, a new post-processor is created according to the actual parameters and constraints of the machine tool, and relevant kinematics, programs, tool paths and other parameters are set. The DMU80P five-axis machining center is a non-orthogonal swing head + turntable structure, and the technical parameters are shown in Table 1. Table 1 Main technical parameters of DMU80P machine tool.
1.4.1 The post-processing basic information setting defines the post-processor name as DMG 45XBC, and the post-processing output unit is mm;The machine tool is a five-axis milling machine with rotor and turntable;The controller selects SINUMERIK 840D Basic from the library and takes the default values for the rest. 1.4.2. The machine tool parameter setting configuration linear axis stroke x=800 mm, y=1 050 mm, z=850 mm;Return to zero position: x=450 mm, y=-1 mm, z=-1 mm;The fourth axis is defined as the B-axis (head), the rotation plane is the Zox plane, and the axis limit is 0 180°;The fifth axis is the C-axis ** stage), and the rotation plane is the XOY plane;The axis is limited to 0 360 °. 1.4.3. According to the general requirements of the NC program, combined with the actual machine tool structure, the program structure should be automatically returned to the safe position before the first movement of the processing program, before the automatic tool change, and after the machiningThe zero coordinate system of the workpiece should be activated before the tool axis is oriented, so as to prevent the default use of 2 or more coordinate systems in a program based on the previous coordinate system, and the orientation and the first movement of the tool to execute the D command, so as to avoid the collision caused by the cancellation of the tool compensation after returning to the safe position. Add blocks named "Tool Change Return Home Z" and "Tool Change Return Home" before and at the end of the other blocks in the "First Tool" in the "Program and Operation Start Sequence" of [Program and Tool Paths], after the other blocks in the "Automatic Tool Change", and before the other blocks in the "First Move". Add the text command "supa, g0-rapid move, z=-1, d0" to the block "tool change return home z", add the text command "supa, g0-rapid move, x=450 y=-1, $mom sys leader(fourth axis)=0, $mom sys leader( fifth axis)=0", complete the automatic return to safe position command customization. Add a block named "fixture offset" before the G17 plane selection block in "Initial Move", click to add the text command "g-offset - user expression" in the block, edit the text command, the expression is $mom siemens fixture offset value, the minimum value is 54, the maximum value is 599. Add the text command "D1-Tool Length Compensation" after the G1 G0 command line in "Linear Motion" and "Fast Movement" in "Tool Diameter" to complete the tool compensation command setting. 1.4.4 3+2 directional machining output cycle800 cycle NX post-processor can automatically judge whether the tool axis vector in directional machining is consistent with the Z-axis of the workpiece coordinate system, and if it is consistent, it is judged to be a three-axis toolpath, and the output rotation axis is oriented B0 C0;If it is inconsistent, it is judged to be a 3+2 toolpath, and the trans atrans and rot arot instructions are output by default, and through the above discussion of the advantages and disadvantages of the cycle800 instructions, the processor adopts the cycle800 swing cycle mode for the directional output of the 3+2 toolpath. In the "Custom Command" of [Program and Tool Path] - "PB cmd check block cycle800", edit as follows**:
#please set your swivel data record#---set cycle800_tc "\"r_data \"" ;
Change R Data to TC1 (machine data group name), and turn on the default setting "PB cmd set Sinumerik Default Setting" in "Program" "Operation Start Sequence" "Program Start" in [Program and Tool Path] and edit it as follows**:
#to set default coordinate rotation output mode for 3+2 operationsglobal dpp_coord_rotation_output_typeset dpp_coord_rotation_output_type " traori " ;if
Change Traori to Swiveling, and complete the setting of 800 cycles for 3+2 toolpath output. 1.4.5 Output settingsIn the "Other Options" under [Output Settings], change the output file extension to "MPF" for the SINUMERIK 840DSL numerical control system, save and exit post-processing. The verification of post-processing is based on the correctness and rationality of the output NC program, and the verification of the trial processing workpiece is shown in Figure 3 through the structural rationality of the NC program, the correctness of the toolpath, the directional instruction output, and the correctness of the Cycle800 parameters under limited conditions. 
Figure 3 Verify the structure of the workpiece.
Set the origin of the clamping offset coordinate system G54 in the center of 20 mm on the upper surface of the workpiece, +ZM is perpendicular to the upper surface, and +XM is the length direction to the right, as shown in Figure 4. The rotary coordinate system G54-ROT is set at the center of the orifice in the +xm direction, and the +zm axis is perpendicular to the inclined plane, as shown in Figure 5. 
Fig.4. G54 coordinate system settings
Fig.5 The G54-Rot coordinate system sets G54 as the parent of G54-Rot and G54-Rot as the rotation of the coordinate system, which is generated by G54 through the following transformation: X-axis offset 225 mm z-axis offset -25 mm rotated 45° about the y-axis. When post-processing, G54-Rot should not output programmable coordinate system G instructions, and should be statically converted to the system "frame" through CYCLE800 instructions, so that the 3+2-axis machine tool system can transfer the workpiece coordinates to the inclined surface that needs to be processed at present by "translation, rotation and translation" in the mode of "translation, rotation and translation", so as to realize the rotation of the spatial workpiece coordinate system. The typical toolpaths are prepared as shown in Figure 6, and the process is shown in Table 2. 
Fig.6. Typical toolpath verification Table 2 Toolpath verification process.
The programmed toolpaths output the NC program through the constructed post-processing. 2.2.1. The logical structure of the program is verified by comparing the output program with the post-processing structure, as shown in Figure 7. 
Fig.7 Comparison between the logical structure of the program and the actual NC output result22.2. The toolpath correctness verification was carried out by using the G** simulation software CIMcoedit to check the toolpaths respectively, as shown in Figure 8, the toolpaths simulated by the NC program were consistent with the toolpaths prepared by NX software. 
Fig.8. Toolpath inspection.
2.2.3 cycle800 cycle output parameters check the feature processing on the inclined surface, output cycle800 cycle and analysis as follows: ......n550 g54①n560 cycle800(1②,"tc1"③,0④,57⑤,22.5,0.,-2.5⑥,-0.,45.,-0.⑦,0.,0.,0.⑧,1⑨,1.1) G54-based transformation (parent). (2) Fallback method (fixed value). (3) The name of the data group (consistent with the device). (4) Coordinate plane (fixed value, new). (5) Rotation mode (fixed value, rotation around axis). (6) Translate first (x-axis translation 22.)5 mm, Y-axis translation 0, Z-axis translation -25 mm）。(7) Re-rotation (0 rotation about the X axis, 45° rotation about the Y axis, 0 rotation about the Z axis). (8) Re-translation (x-axis translation 0, y-axis translation 0, z-axis translation 0). (9) Priority direction (fixed 1 or -1, 1 is positive). (10) Incremental fallback (not used). According to the comparison between the output cycle800 cycle and the set G54-ROT, the logic of the two cycles is the same, and the output data group name and parameters are correct. 2.2.4. Trial processing verification verifies all the characteristics of the digital model preparation of the machining tool path and post-processing into NC program, the machine tool is tested for processing, the processing result is shown in Figure 9, the processing result is consistent with the programming digital model, and the post-processor verification is successful.
Figure 9 Trial processing verification results Original author: Chen Mingkun, Huang Haifeng, Yang Sheng Author's Affiliation: SAIC-GM-Wuling Automobile Co., Ltd