1. Feed function
1.1. Rapid feed
Eeoemm7p3001 In rapid feed mode, each axis moves at the set rapid feed speed without being affected by other axes moving at the same time. Note that the rapid feed speed varies depending on the machine tool instructions, and finally different axes reach the destination at different times and overload may occur.
In the big operation, G00 G01 G02 G03 is the same as the FANUC system command and will not be explained here.
1.2. Cutting feed
1.2.1. Feed per minute (G94)
[Function]
This function uses a numerical value following the address code F to set the feed rate per minute of the cutting tool.
[Programming format]
G94
[Setting unit]
By setting the NC optional parameter (command unit system), you can choose from 1 mm/min, 0.1 mm/min, 1 inch/min, 0.1 inch/min, 0.01 inch/min, and the setting range is 0.1-24000.0 mm/min, 0.01-2400.00 inch/min.
[Detailed explanation]
• The maximum feed rate allowed is called the limit feed rate, which is set by the NC optional parameter (long byte) No. 10. If the axis moves outside this range, its feed rate will be set to the limit feed rate and the following alarm signal will appear on the alarm display line of the screen: 4204 Alarm-D Feed rate exceeded (change). The programmed feed rate can be used for the actual feed rate or the over-limit feed rate.
1.2.2. Feed per revolution (G95)
[Function]
This function uses a numerical value following the address code F to set the feed rate per revolution of the cutting tool
[Programming format]
G95
[Setting unit]
By setting the NC optional parameter (command unit system), you can select from 1 mm/rev, 0.01 mm/rev, 0.001 mm/rev, 1 inch/rev, 0.001 inch/rev or 0.0001 inch/rev, and the setting range is 0.001-500.000 mm/rev
[Detailed explanation]
Since the limit feed rate is set in mm/min, it can be converted to mm/rev by using the following formula: fm = fr N, where N = axis speed (rev/min), fm = feed rate (mm/min), fr = feed rate (mm/rev).
2. Basic operation functions
2.1. Plane selection (G17 G18 G19)
[Programming format]
G17 Xp Yp
G18 Zp XP
G19 Yp Zp
2.2. Dwell command (G04)
[Programming format]
Both of the following programming formats can be used to specify the dwell waiting function: G04 F__
F sets the dwell time length
The dwell time unit can be selected from 1 0.1 0.01 and 0.001 seconds using NC optional parameters (command unit system)
The maximum programmable dwell time is 99999.999 seconds
G04 P__
P sets the dwell time length. The dwell time unit is selected in the same mode as when specifying with F.
2.3. Workpiece coordinate system selection (G15 G16)
[Programming format]
Mode G code G15 Hn (0 n 200)
Once a new workpiece coordinate system n is set using the mode G code, the coordinate values ​​set in the same and following blocks are interpreted as the coordinate values ​​in the selected workpiece coordinate system n.
 
One-line G code G16 Hn (0 n 200)
If a new workpiece coordinate system n is set using the single-click G mode, only the coordinate values ​​set in the same data block are regarded as the coordinate values ​​in the selected workpiece coordinate system n.
 
• After turning on the power and resetting the NC, the system automatically selects the workpiece coordinate system previously selected by the command G15. G15 and G16 cannot be expressed in the following modes.
2.4. Change of workpiece coordinate system (G92)
[Programming format]
G92 X Y Z W
2.5. Additional head rotation command (M73-M76)
[Format]
M73 Rotate the spindle head front end
M74 Rotate the spindle head left end
M75 Rotate the spindle head right end
M76 Rotate the spindle head front end
2.6. Additional head 5 degree rotation command (M94, M95)
[Format]
M94 RH=θ forward rotation
M95 RH=θ reverse rotation
θ is a multiple of 5
2.7. Translation and rotation of coordinate system (G11, G10)
[Function]
Translation/rotation function translates or rotates a workpiece coordinate system. The new coordinate system defined by compensating or rotating a workpiece coordinate system is called a local coordinate system. Deleting a local coordinate system is possible. Format, parallel shift/rotation of coordinate system G11 IP__P__, cancel the local coordinate system G10. When the G10 instruction is specified, the translation and rotation angle are canceled.
[Explanation]
Once G11 is executed, NC enters the state of defining the local coordinate system. If G11 is executed again in this state, G11 will change the previously defined local coordinate system. In the second G11 mark, if the address mark is omitted, it will continue to be used in the first G11.
2.8. Tool length compensation function
[Function]
The tool length compensation function can compensate the position of the cutting tool so that the tip of the cutting tool should be located at the programmed position. Available G codes:
G53 Cancel tool length compensation
G54 Tool length compensation X-axis
G55 Tool length compensation Y-axis
G56 Tool length compensation Z-axis
[Format]
{G54 - G56} IP__ H__
IP Current position of the tool after compensation
H Tool offset amount, standard tool compensation number is H00 to H50 and this can be extended to H00 to H100 H200 or H300, the compensation amount of H00 is always 0.
2.9. Cutter Radius Compensation (G40 G41 G42)
[Function]
The tool compensation function automatically organizes compensation for the tool radius. Programming according to the geometric dimensions of a workpiece cannot obtain the correct dimensions because the tool size (diameter) is not taken into account. However, if the tool diameter is taken into account, it will be very difficult to program. This problem can be compensated by a function called tool radius compensation. This technology automatically compensates the tool diameter. If the tool radius compensation function is used during programming, the program will automatically generate the correct tool center path according to the geometry of the part.
[Format]
G17 G41 (G42) Xp__ Yp__ D__
G18 G41 (G42) Zp__Xp__ D__
G19 G41 (G42) Yp__Zp__ D__
G40 Cancels the cutting radius compensation (the mode is automatically selected when the power is turned on). For details, refer to the tool movement when the cutting radius compensation is canceled.
G41 Cuts on the left (offset - cutting downward from the left side when viewed from the direction of tool movement). For details, refer to Changing the compensation direction in the cutting radius compensation mode.
G42 right cutting (from the tool movement direction, the right side compensation is upward cutting). The tool radius compensation mode is set by G41 or G42 and canceled by G40. For a more detailed list, refer to the tool compensation mode to set the compensation direction:
G17 Xp-Yp plane selection The plane selection mode is the same as G02 or G03 mode
G18 Zp-Xp plane selection The plane selection mode is the same as G02 or G03 mode
G19 Yp-Zp plane selection The plane selection mode is the same as G02 or G03 mode
2.10. Tool change command
[Format]
Tn M06
2.11. Additional head change command
MCR-B2 has four sets of rotary heads T301 T302 T303 T304
[Format]
Tn M170
Example
T303 M170