Option File Generator HelpMill Turn
With the Turning mode, you can set the GPost in this mode instead of the milling mode at the start of the program. The new MODE/TURN command can also be given in your input program to switch between the MILL and TURN modes.
Optionally, you can specify the input coordinates to be in the Machine or APT like part system. The default is to similar to the Mill mode as in (X, 0, Z), where X is the lathe radius and Z is along the center line.
The GPost now supports the MODE/MILL command to be used with the SPINDL/PARLEL,ZAXIS or SPINDL/PARLEL, XAXIS. To make this work, you must specify the input coordinates to be in the Machine coordinates as (X, Y, Z) for both spindle configurations. If your input file is in any other format, you can convert via the transformation panel or use TRANS/matrix, OPTION, 11 command in your input file.
There are two options. These are:
SPINDL/PARLEL, ZAXIS - when this option is selected, you would be doing "end work" with XC and Z-axis output to profile or drill at the end of your part
SPINDL/PARLEL, XAXIS - when this option is selected, you would be doing "side work" with XC and Z-axis output to profile or drill at the side of the part
In either of the above conditions, some machines support a Y-axis stroke instead of the combined ZC or XC output. In this case, the command MODE/YAXIS,ON-OFF-AUTO is supplied to be used in the input program. There are three options for this setting:
No
Yes
Auto - when Auto is selected, make sure you set the Y-axis limits. The GPost will automatically select Y machine or XC and ZC when programmed Y-axis is within the set limits
When the Auto mode is set, make sure you set the Y-stroke limits on your machine. The GPost will automatically output either the Y machine or XC and ZC when programmed Y-axis is within the set limits.
For turning mode, the tool changes are done using the TURRET command (the milling mode uses the LOADTL command). This section allows you to specify options like X in diameters and the G92 type of tooltip programming conditions.
Motion records in the CL file are adjusted by the specified gauge lengths and are output as tool tip coordinates. The postprocessor command TURRET/CENTER cancels gauge length compensation to output turret reference coordinates until another turret command is processed. This option selects the default condition prior to the initial TURRET statement in the CL file.
The preset blocks can be output by the postprocessor automatically for each turret change to adjust for the specified gauge lengths. Check this box if you wish for this to be the case.
This is where the the CSFM programming options can be specified and the "R-Output When not in SPINDL cmd" settings can be specified. Note: if the G-Codes are initialized to zero (0), they will be changed to their respective default (e.g. G92 would be set to 92). This might be the case since these values are based on new Commons which are set to 0.
Single point G33 type threading is supported and the options for Lead register and modality are set in this section. The input program will supply THREAD/ON or THREAD/AUTO commands followed by the GOTO to enable threading motion as before.
CAM systems can generate a complete threading cycle with THREAD/AUTO or THRDSQ commands. You can let the GPost convert this into multiple G33 blocks. If you prefer to handle this in FIL, then select the option "Do not expand" and write your FIL code to parse THREAD/AUTO command and output the desired G76 etc. block.
Note: this option must be set in the option file and can not be set / reset using FIL. Also, if the G-Code and Register Address are initialized to 0, they will be set to their normal defaults (e.g., G33 = 33, and the Register Address would be "K").
--------------------------------------------------------------------------------------------------------------------------
Option File Generator Help
Copyright (c) 2005, All Rights Reserved,
Austin N.C., 505 East Huntland Drive, Suite 480
Austin, TX 78752
www.austinnc.com