(G90.1/G91.1) of the center of the circle (Y and Z directions,
respectively).
It's an error if:
l Y and Z are both omitted
The axis words are all optional except that at least one
of Y and Z must be used.
l J and K are both omitted
J and K are optional except that at least one of the two
must be used.
E X A M P L E
G17 G02 X1.0 Y1.6 I0.3 J0.4 Z0.9 is a center
format command to mill an arc in incremental arc
distance mode (G91.1) that makes a clockwise (as
viewed from the positive Z-axis), circular, or helical arc
whose axis is parallel to the Z-axis, ending where X =
1.0, Y = 1.6, and Z = 0.9, with its center offset in the X
direction by 0.3 units from the current X location and
offset in the Y direction by 0.4 units from the current Y
location. If the current location has X = 0.7, Y = 0.7 at the
outset, the center is at X = 1.0, Y = 1.1. If the starting
value of Z is 0.9, this is a circular arc; otherwise, it's a
helical arc. The radius of this arc would be 0.5.
In the center format, the radius of the arc is not specified, but
it may be found easily as the distance from the center of the
circle to either the current point or the end point of the arc.
(Sample Program G02EX3:)
(Workpiece Size: X4, Y3, Z1)
(Tool: Tool #2, 1/4” Slot Drill)
(Tool Start Position: X0, Y0, Z1)
N2 G90 G80 G40 G54 G20 G17 G94 G64 (SAFETY BLOCK)
N5 G90 G20
N10 M06 T2 G43 H2
N15 M03 S1200
N20 G00 X1 Y1
N25 Z0.1
N30 G01 Z-0.1 F5
N35 G02 X2 Y2 I1 J0 F20 (ARC FEED CW, RADIUS I1,J0
AT 20 IPM)
N40 G01 X3.5
N45 G02 X3 Y0.5 R2 (ARC FEED CW, RADIUS 2)
N50 X1 Y1 R2 (ARC FEED CW, RADIUS 2)
N55 G00 Z0.1
N60 X2 Y1.5
N65 G01 Z-0.25
N70 G02 X2 Y1.5 I0.25 J-0.25 (FULL CIRCLE ARC FEED
MOVE CW)
N75 G00 Z1
N80 X0 Y0
N85 M05
N90 M30
9.2.5 Dwell (G04)
For a dwell, program: G04 P~
l P~ is the dwell time (measured in seconds)
Dwell keeps the axes unmoving for the period of time in
seconds specified by the P number.
E X A M P L E
G04 P4.2 (to wait 4.2 seconds)
Troubleshooting
It's an error if:
l The P number is negative
9.2.6 Set Offsets (G10)
Use the controls on the Offsets tab to set offsets. You can
program offsets with the G10 G-code command.
Read the following sections for reference:
Set Tool Table (G10 L1) 180
Set Coordinate System (G10 L2) 181
Set Tool Table (G10 L10) 181
Set Tool Table (G10 L11) 181
Set Coordinate System (G10 L20) 181
Set Tool Table (G10 L1)
To define an entry in the tool table, program: G10 L1 P~ R~
l P~ is the tool number
l R~ is the radius of tool
G10 L1 sets the tool table for the P tool number to the values
of the words. A valid G10 L1 rewrites and reloads the tool
table.
Troubleshooting
It's an error if:
l Cutter Compensation is on
l The P number is unspecified
l The P number is not a valid tool number from the tool
©Tormach® 2024
Specifications subject to change without notice.
Page 180 UM10811: 1500MX Operator's Manual (Version 0424A)
For the most recent version, see tormach.com/support
9: PROGRAMMING
To Next Page
Loading...
