Floor facing

Macro for milling the end surface of a part on a milling machine. Often used to perform preliminary operations.

You can make it as a custom G-code on your machine, see other macros.

[!NOTE] Specify the G-coda number for the simplified form of the cycle call. For example G201.

Call Format

G65 P_ [B_] [C_] D_ F_ [K_] [R_] T_ U_ [W_] X_ Y_ Z_
G201 [B_] [C_] D_ F_ [K_] [R_] T_ U_ [W_] X_ Y_ Z_

Attributes

P – name of the subroutine. O9013. Defaults to the position before the loop starts
*B – initial coordinate along the Z axis
*C – starting angle. The contour tilts counterclockwise
D – cutter diameter. Can be omitted if the T attribute is specified and the tool geometry is entered in the OffSet table
F – feed speed
*K – allowance along the Z axis
*R – length of approach and retraction of the tool from the edge of the part
T – corrector number. For Fanuc, this may not be specified if the D attribute is specified.
U – percentage of cutter overlap
*W – removal in one pass along the Z axis. By default, processing occurs in one pass
X – part length
Y – part width
Z – final coordinate along the Z axis
* – optional attributes

Examples

Example 1: trimming 220x150mm in one pass along the Z axis with a cutter diameter of 50mm. 60% cutter overlap. End Z coordinate = -2.

%
<FLOOR-FACING>
G54 (working coordinate system)
G90G80G40G21G17G0
G61
G91G28Z0
G90
T5M6 (tool change)
G64
M8
M3S5000 (spindle start)
G43Z10.H5 (lowering the tool)
G0X0Y0 (moving to the center of the part)
G201 D50. F800 U60. X220. Y150. Z-2. (call macro)
M5
M9
G91G28Z0
G90
M30
%

Example 2: trimming 140x100mm with a cutting depth of 1.5mm along the Z axis and tool offset number 5. 65% cutter overlap. The first pass will be made on Z-1.5, the second on Z-3., the third and fourth on Z-4.5 and Z-5. respectively...

G43Z10.H5
G0X0Y0
G201 B0. F500 T5 W1.5 U65. X140. Y100. Z-5.

Example 3: transverse trim 200x100mm (along the Y axis). 40% cutter overlap.

G43Z10.H5
G0X0Y0
G201 F500 C90. D50. U40. X100. Y200. Z-2.

Example 4: the dimensions of the workpiece are 200x100mm,the center of the coordinate system along the X axis is the left face, and along the Y axis is a fixed jaw.

G43Z10.H5
G0X[200./2]Y[100./2]
G201 F300 D50. U65. X200. Y100. Z-2.

Example 5: the dimensions of the workpiece are 200x100mm, the center of the coordinate system along the X axis is the right edge, and along the Y axis is a fixed jaw. End coordinate along the Z axis = 20.

G43Z24.H5
G0X[-200./2]Y[100./2]
G201 F300 C90. D50. U40. X100. Y200. Z20.

Exceptions

3001 - Invalid startup type. Macro cannot be started as main program
3002 - -D- Invalid tool diameter
3003 - Tool diameter -D- and its number -T- are missing. One of these parameters must be specified
3005 - -T- Invalid tool number
3006 - -X- Part length must be positive
3007 - -Y- Part width must be positive
3008 - -Z- End plane of machining
3009 - -U- Invalid cutter overlap percentage
3010 - -W- Invalid depth of cut
3011 - -K- Invalid stock height
3012 - -C- Invalid inclination angle of machining plane
3013 - -F- Missing feed rate
3014 - -F- Feed rate out of range
3015 - -R- Tool retraction length must be positive
3016 - -B- End machining plane is higher than start machining plane

Defined Variables

#161 - current position along the X-axis
#162 - current position along the Y-axis
#163 - current position along the Z-axis
#164 - maximum corrector number
#165 - maximum feed speed
#166 - maximum allowance along the Z axis
#169 - percentage of flat diameter on last pass

System Variables Used

#3000 - Macro alarm
#5001 - End point position of the previous block (workpiece coordinate system). X-axis
#5002 - End point position of the previous block (workpiece coordinate system) . Y-axis
#5003 - End point position of the previous block (workpiece coordinate system) . Z-axis
#4000 - Subroutine number

Compatibility

Milling - FANUC Series Oi-MODEL F
Milling - HAAS

[!WARNING] Before starting the makras, do not forget to check all the system variables used, they may differ on some machines.