Service Home G01 Linear Interpolation Motion (Group 01)

G01 Linear Interpolation Motion (Group 01)

G01 Linear Interpolation Motion (Group 01)

F - Feed rate
* B - B-axis motion command
* C - C-Axis motion command
* U - X-axis incremental motion command
* W - Z-axis incremental motion command
* X - X-axis absolute motion command
* Y - Y-axis absolute motion command
* Z - Z-axis absolute motion command
* A - Optional angle of movement (used with only one of X, Z, U, W)
* I - X-axis chamfering from Z to X (the sign does not matter, only for 90 degree turns)
* K - Z-axis chamfering from X to Z (the sign does not matter, only for 90 degree turns)

* ,C - Distance from center of intersection where the chamfer begins (the sign does not matter, can chamfer non-90 degree lines)
* ,R / R - Radius of the fillet or arc (the sign does not matter)
This G code provides for straight line (linear) motion from point to point. Motion can occur in 1 or more axes. You can command a G01 with 3 or more axes All axes will start and finish motion at the same time. The speed of all axes is controlled so that the feed rate specified is achieved along the actual path. The C-Axis may also be commanded and this will provide a helical (spiral) motion. A C-Axis feed rate is dependent on the C-Axis diameter setting (Setting 102) to create a helical motion. The F address (feedrate) command is modal and may be specified in a previous block. Only the axes specified are moved.Corner Rounding and Chamfering ExampleA chamfer block or a corner rounding block can be automatically inserted between two linear interpolation blocks by specifying ,C (chamfering) or ,R (corner rounding).

NOTE: Both of these variables use a comma symbol (,) before the variable.
There must be a terminating linear interpolation block after the beginning block (a G04 pause may intervene). These two linear interpolation blocks specify a theoretical corner of intersection. If the beginning block specifies a ,C (comma C) the value after the C is the distance from the corner of intersection where the chamfer begins and also the distance from that same corner where the chamfer ends. If the beginning block specifies a ,R (comma R) the value after the R is the radius of a circle tangent to the corner at two points: the beginning of the corner rounding arc block that is inserted and the endpoint of that arc. There can be consecutive blocks with chamfer or corner rounding specified. There must be movement on the two axes specified by the selected plane (the active plane X-Y (G17), X-Z (G18) or Y-Z (G19). For chamfering a 90 angle only, an I or K value can be substituted where ,C is used.Chamfering


%
o60011 (G01 CHAMFERING) ;
(G54 X0 is at the center of rotation) ;
(Z0 is on the face of the part) ;
(T1 is an OD cutting tool) ;
(BEGIN PREPARATION BLOCKS) ;
T101 (Select tool and offset 1) ;
G00 G18 G20 G40 G80 G99 (Safe startup) ;
G50 S1000 (Limit spindle to 1000 RPM) ;
G97 S500 M03 (CSS off, Spindle on CW) ;
G00 G54 X0 Z0.25 (Rapid to 1st position) ;
M08 (Coolant on) ;
(BEGIN CUTTING BLOCKS) ;
G01 Z0 F0.005 (Feed to Z0) ;
N5 G01 X0.50 K-0.050 (Chamfer 1) ;
G01 Z-0.5 (Linear feed to Z-0.5) ;
N7 G01 X0.75 K-0.050 (Chamfer 2) ;
N8 G01 Z-1.0 I0.050 (Chamfer 3) ;
N9 G01 X1.25 K-0.050 (Chamfer 4) ;
G01 Z-1.5 (Feed to Z-1.5) ;
(BEGIN COMPLETION BLOCKS) ;
G00 X1.5 M09 (Rapid Retract, Coolant off) ;
G53 X0 (X home) ;
G53 Z0 M05 (Z home, spindle off) ;
M30 (End program) ;
%
This G-code syntax automatically includes a 45 chamfer or corner radius between two blocks of linear interpolation which intersect a right (90 degree) angle.Chamfering Syntax
G01 X(U) x Kk ;
G01 Z(W) z Ii ;
Corner Rounding Syntax
G01 X(U) x Rr ;
G01 Z(W) z Rr ;
Addresses:I = chamfering, Z to XK = chamfering, X to ZR = corner rounding (X or Z axis direction)Notes:1. Incremental programming is possible if U or W is specified in place of X or Z, respectively. So its actions are as follows:X(current position + i) = UiZ(current position + k) = WkX(current position + r) = UrZ(current position + r) = Wr
2. Current position of X or Z Axis is added to the increment.
3. I, K and R always specify a radius value (radius programming value).
Chamfering Code Z to X: [A] Chamfering, [B] Code/Example, [C] Movement.


Chamfering Code X to Z: [A] Chamfering, [B] Code/Example, [C] Movement.


Corner Rounding Code Z to X: [A] Corner rounding, [B] Code/Example, [C] Movement.


Corner Rounding Code X to Z: [A] Corner rounding, [B] Code/Example, [C] Movement.


Rules:1. Use K address only with X(U)address. Use I address only with Z(W) address.
2. Use R address with either X(U) or Z(W), but not both in the same block.
3. Do not use I and K together on the same block. When using R address, do not use I or K.
4. The next block must be another single linear move that is perpendicular to the previous one.
5. Automatic chamfering or corner rounding cannot be used in a threading cycle or in a Canned cycle.
6. Chamfer or corner radius must be small enough to fit between the intersecting lines.
7. Use only a single X or Z-axis move in linear mode (G01) for chamfering or corner rounding.
G01 Chamfering with AWhen specifying an angle (A), command motion in only one of the other axes (X or Z), the other axis is calculated based on the angle.G01 Chamfering with A: [1] Feed, [2] Rapid, [3] Start Point, [4] Finish Point.


%
o60012 (G01 CHAMFERING WITH 'A') ;
(G54 X0 is at the center of rotation) ;
(Z0 is on the face of the part) ;
(T1 is an OD cutting tool) ;
(BEGIN PREPARATION BLOCKS) ;
T101 (Select tool and offset 1) ;
G00 G18 G20 G40 G80 G99 (Safe startup) ;
G50 S1000 (Limit spindle to 1000 RPM) ;
G97 S500 M03 (CSS off, Spindle on CW) ;
G00 G54 X4. Z0.1 (Rapid to clear position) ;
M08 (Coolant on) ;
X0 (Rapid to center of diameter) ;
(BEGIN CUTTING BLOCKS) ;
G01 Z0 F0.01 (Feed towards face) ;
G01 X4. (position 3) ;
X5. A150. (position 4) ;
Z-2. (Feed to back of part) ;
(BEGIN COMPLETION BLOCKS) ;
G00 X6. M09 (Rapid Retract, Coolant off) ;
G53 X0 (X home) ;
G53 Z0 M05 (Z home, spindle off) ;
M30 (End program) ;
%

NOTE: A -30 = A150; A -45 = A135
When specifying an angle (A), command motion in only one of the other axes (X or Z), the other axis is calculated based on the angle.G01 Chamfering with A: [1] Feed, [2] Rapid, [3] Start Point, [4] Finish Point.


%
o60012 (G01 CHAMFERING WITH 'A') ;
(G54 X0 is at the center of rotation) ;
(Z0 is on the face of the part) ;
(T1 is an OD cutting tool) ;
(BEGIN PREPARATION BLOCKS) ;
T101 (Select tool and offset 1) ;
G00 G18 G20 G40 G80 G99 (Safe startup) ;
G50 S1000 (Limit spindle to 1000 RPM) ;
G97 S500 M03 (CSS off, Spindle on CW) ;
G00 G54 X4. Z0.1 (Rapid to clear position) ;
M08 (Coolant on) ;
X0 (Rapid to center of diameter) ;
(BEGIN CUTTING BLOCKS) ;
G01 Z0 F0.01 (Feed towards face) ;
G01 X4. (position 3) ;
X5. A150. (position 4) ;
Z-2. (Feed to back of part) ;
(BEGIN COMPLETION BLOCKS) ;
G00 X6. M09 (Rapid Retract, Coolant off) ;
G53 X0 (X home) ;
G53 Z0 M05 (Z home, spindle off) ;
M30 (End program) ;
%

NOTE: A -30 = A150; A -45 = A135