5-AXIS CNC5-axis NC functions

⊙With and without tool center point control

• Tool center point controlA function that treats the programmed X, Y, Z as the position of the tool tip (tool center point), and has the NC automatically calculate the linear-axis compensating motion so the tool tip follows the programmed position and path even when the rotary axes turn. The feed rate can also be treated as the tool tip speed.^{[1][2][3][4][5][6]}
• Without tool center point controlIf you move only a rotary axis, the NC simply rotates the axis, so the tool tip does not stay put (it drifts off along an arc). When the tool length changes, you need a program recalculated in CAM.^[1][5][6]
• Two command formats of tool center point control (FANUC classification)Type I: command the rotary axis angles directly. Type II: command the tool orientation as a vector (I, J, K). With Type II, the same program works even on different machine configurations (head rotation, table rotation, mixed).One source / reference^[3]

◇Other 5-axis functions

• Tilted working plane command (Tilted Working Plane)A function that defines a coordinate system along a tilted face (tilted coordinate system) so you can write the program on that face as if it were an ordinary XY plane. The most commonly used function in 3+2 machining.^{[3][7][8][1][5][9][10]}
• How to define a tilted planeSix methods: Euler angles, roll-pitch-yaw angles, three points on the plane, two vectors, projection angles, and tool axis direction.^[3][8][2]
• Tool axis direction controlA function that automatically indexes the rotary axes so the tool is perpendicular to the plane defined by the tilted working plane command. Because the tilted coordinate system follows when indexing turns the rotary axes, you don't need to reset the coordinate system after indexing.^[7][8]
• There are normally two rotary axis solutionsFor the same tilted plane, there are generally two sets of rotary axis angles that point the tool perpendicular to it (e.g., A+45°/C+90° and A−45°/C−90°). You can specify which to use; if you don't, the NC chooses the nearer one within the travel range. If it is out of range, an error occurs.One source / reference^[5]
• 3D tool radius compensationSo that you can use a tool with a different diameter from the one CAM calculated for, the tool radius is compensated in the direction of the surface normal (face milling) or in the direction perpendicular to both the travel direction and the tool axis (side milling). CAM must output the surface normal vector for each block.^[1][2][5]
• Tool cutting point command (cutting edge point control)The program commands the point where the tool touches the workpiece (cutting point), and the NC compensates tool length, tool radius and corner radius. You don't have to fix the program when you change tools.^[2][3][4]
• Tool orientation control (orientation interpolation for side milling)Interpolates between the tool orientations at the start and end points so that the side of the tool sweeps a flat plane. Prevents overcutting by the tool side when machining a slanted surface with the side of the tool.^[2][3][5][1]
• Workpiece setup error compensationEven if the workpiece is placed offset from what the program assumes (translated or rotated), the measured error is used to correct the path so the part can be machined without changing the program. It also applies to the rotary axis motion of tool center point control and tilted working plane commands.^{[2][3][11][12]}
• 3D manual feed (retracting along the tool axis direction)A function to manually pull a tilted tool out along its tool axis, or move it parallel to the tilted plane, for example when a tool breaks. On a 3-axis machine you just raise Z, but on a 5-axis machine several axes must move in coordination.^[2][4][1]
• 3D collision checkThe NC holds the table, fixtures, spindle, tools and so on as combinations of boxes, cylinders and planes, judges collisions before moving, and stops the axes. It works in both manual and automatic operation.One source / reference^[2][3]
• Smoothing of tiny line segmentsA series of short lines (G1) output by CAM gives stepped speed at the block joints, leaving stripes and vibration marks on the surface. NCs have functions that merge them into splines or round corners within tolerance (Siemens COMPCAD and CYCLE832; FANUC Nano Smoothing 2 and Smooth TCP).^[1][2][3]

≡Commands by NC maker

The same function is commanded differently depending on the NC. The G-codes and M-codes below are only those confirmed in each maker's public documents. G-code numbers for FANUC's tilted working plane command and others are not listed because they could not be confirmed in public documents.

FG93 (cancel and return to normal with G94)

• Inverse time feed. The F value is interpreted as ‘the block finishes in 1/F minutes’ (F = 1/time [min]). When a rotary axis moves, the relationship between tool tip speed and each axis speed changes block by block, so CAM often uses it for 4- and 5-axis programs.^[17][18][19]
• While G93 is active, F is required in every G1, G2, G3 block (it is not carried over as modal). Rapid traverse (G0) is not affected^[17][18]
• On Haas, a reset returns to G94One source / reference^[17]
• After switching among G93, G94 and G95, command the feed againOne source / reference^[19]
• Group number: Haas uses group 05One source / reference^[17]

To calculate the F value, use5-axis calculations.

If you move a rotary axis in G94 (feed per minute)

• The meaning of the feed when you move a rotary axis in G94 (feed per minute) differs by NC. In NIST RS274NGC, a block where linear axes move uses feed per minute along the length of the XYZ path as if the rotary axes were not moving, and a block with only rotary axes uses deg/min.One source / reference^[18]
• In Heidenhain's standard, the rotary axis feed is in deg/min, so the farther the tool is from the center of rotation, the faster the actual contouring feed. M116 treats a rotary table axis as mm/min.One source / reference^[5]
• With tool center point control, TRAORI, and FUNCTION TCPM (F TCP), the feed is the relative speed between the tool tip and the workpiece.^[1][3][5]

↧Tool length and center of rotation

• When the tool orientation changes, the longer the tool, the larger the linear-axis compensating motion. With tool center point control, the program can be used as is even if the tool length changes (the control calculates with the actual tool length).^[1][2][3]
• When using tool center point control, always apply tool length compensation (H number, tool length data). If you don't, the tip position calculation goes wrong and you risk damaging the ballbar or the machine.^[13][6]
• If the center of rotation position used by the control (Haas MRZP, each maker's machine configuration parameters and kinematics) differs from the real machine, the machined part will show errors when the rotary axes move. That is why measuring and correcting the center of rotation (kinematics calibration) is needed.^{[20][6][7][1]}
• Mitsubishi Electric has a function (tool length compensation along the tool axis direction) that can apply tool length compensation along the tool axis even when a rotary axis has moved the tool axis away from the Z direction.One source / reference^[4]

GRelated pages in the G-code dictionary

• G43: tool length compensation. Tool center point control extends this idea to tool orientation and rotary axes
• G49: canceling tool length compensation. Some NCs also use it to cancel tool center point control
• G53: positioning in the machine coordinate system. Used to retract the tool before rotating
• G68: 2D coordinate rotation. Not the same as 3D tilted-plane machining
• G94: feed per minute. The counterpart of inverse time feed G93