Working Style

Parameter Name

Description

PRP Name

Pos to Machine

This parameter enables writing posts in the new style. SolidCAM provides GCode output for a number of coordinate systems.

pos_to_machine

DPP File Name

Name of the *.dpp file used to customize the Documentation output.

doc_processor_name

Machine's Tool Table Name

Defines the tool table name of the machine to be the part tool table.

tool_table_name

Delta for Tool H

The delta address of the offset table in the machine controller. Used for the Documentation option only.

Delta_for_TOOL_H

Home Data At Start

Defines the location where the @home_data will be printed: either at the beginning of the program after @def_tool, or in the end of the program after @end_of_program.

home_data_at_start

At Start All Axes Set To Home Ref

Determines if all axes are shown in Home Reference position for START PROGRAM item in the Move List Pane of Machine Simulation, when simulating the entire part.

At End All Axes Set to Home Ref

Determines if all axes are shown in Home Reference position for END PROGRAM item in the Move List Pane of Machine Simulation, when simulating the entire part.

Safety Distance

Defines a default value for the ‘safety_dist’ parameter used in the dialog boxes throughout various operations.

safety_dist

Hole Wizard (metric)

Name of the Hole Wizard process for metric units (location is defined in SolidCAM Settings).

Hole Wizard (inch)

Name of the Hole Wizard process for inch units (location is defined in SolidCAM Settings).

Compensation By Zero(Milling only)

Indicates whether the tool-radius compensation is zero (Yes) or tool radius (No).

comp_by_zero_tool

Compensation Rough Passes (Milling only)

Default value for Compensation Exists parameter on Rough Passes.

-

Compensation Finish Passes (Milling only)

Default value for Compensation Exists parameter on Finish Passes. passes.

-

Compensation Clear Offset Passes (Milling only)

Default value for Compensation Exists parameter on Clear Offset.

-

Compensation for Chamfer exists (Milling only)

Arc Exist as Default (Milling only)

Default value for Support Arcs parameter.

arc_exist

Software Transform

Enables enhancements of the transformation feature.

software_transform

Finish Retreat (Turning only)

Indicates whether the finish process of the machine cycle retreats to the start point (Yes) or remains at the last point (No).

finish_retreat

Semi-Finish Retreat (Turning only)

Indicates whether the semi-finish process of the machine cycle retreats to the start point (Yes) or remains at the last point (No).

semi_finish_retreat

Compensation On Rough With Cycle (Turning only)

Allows whether or not cutter wear compensation can be used in the rough process of the machine cycle.

Use Turning Cycle as Default

Default value for Turning Cycle parameter.

turning_cycle_dflt

Use Groove Cycle as Default

Default value for Groove Cycle parameter.

groove_cycle_dflt

Tool Path Info for XY

Tool path information for XY approach is shown in trace.

--

Tool Path Info for Z

Tool path information for Z approach is shown in trace.

--

Output GCode Channels

Controls generation of GCode files for several turrets.

Mixed on Single File – Generates separate GCode files for each turret and combines all files into the first GCode file. The first GCode file is the file generated for the first turret defined in Devices section of VMID.

Separated Files – Generates separate GCode files for each turret.

Order on Single File – Generates one GCode file that includes GCode of all operations in the order that operations are defined in CAM Manager.

turret_channel

GCode File Extension

Specifies the extension of the generated GCode file.

gpp_file_ext

GCode File Name Format

Specifies the naming format of the generated GCode file. The GCode file can be named using the Part Name & Channel Name or using the Program Number & Channel Name.

GCode File Name Max Length

Specifies the maximum number of characters allowed in the GCode file name.

max_g_name_length

GCode Folder

Specifies the name of the GCode folder.

dir_gcode

Allow Spaces in GCode File

Allows whether or not spaces can be used in the GCode file name.

Separate Folder For Each GCode File

Creates a separate folder for each GCode file to which the GCode segment files are saved.

split_gcode_folders

Separate Folder For Each CAM-Part

Creates a separate folder for each CAM-Part to which the GCode files are saved.

gcode_part_subfolder

Split Files Counter Separator

Specifies the symbol to be used for separating the parts of the file name.

split_gcode

Skip Machine Limits Checking

Specify whether or not to check machine limits in GCode generation.

Default Program Number

Default program number.

prog_num_dflt

Default Procedure Number

Default number for first procedure.

proc_num_dflt

Indicates whether procedures can be generated in the GCode.

gen_procs

If several drilling operations have the same drill points, then the drill points are stored in a single separate procedure.

drill_proc

Indicates whether internal procedures of the operation will be generated.

gen_internal_proc

Numerate Procedures Separately for Every Split

Defines that all GCode programs created in a part with splits have subroutines that start with the same number of the first block.

same_sub_numbers

Initialize GPP Variables Every Split

All GPP variables will be initialized in every GCode program in part with splits.

init_var_after_split

Optimize Operations Loops

Saves tool paths among continuous operations that have the same Edit operations. Used only for Milling.

optimize_jobs_loop

Loop Exist

If “YES”, generates pcode @loop.

Otherwise, instead of @loop, generates @change_ref_point for transformation and @rotate for rotation.

loop_exist

Procedures in Turning

Defines whether to generate a separate procedure for geometruc points of a turning process, or the points will be generated immediately after the cycle.

turn_proc

Procedures in Combine Turning

Generates a procedure of common geometric points for several cycles.

turn_common_procs

Procedures in Turning With Single line

Specifies the GCode format if the cycle geometry is a single line.

gen_single_line_proc

The postprocessor determines automatically which pair of angles to use.

The second angle pair, other than the first automatically determined, is used.

Type of start angle.

Solution Type for

Start Angle

Type of solution for start angle.

solution_for_start_

angle

Preferred Start Angle

Preferred start angle.

start_angle

Angle Tolerance for Using Machine Limits

Angle tolerance for using machine limits.

angle_tol_for_limits

Interpolation for Distance

Sets the interpolator for distance on and off.

interplat_for_dist

Enable Mx Edit

Enable to change inside the 5-axis operation the value of the following two parameters: Auto Angle Pair and Other Angle Pair.

enable_mx_edit

Use Machine Limits

Defines whether to use the machine limits in both translational and rotational axis.

use_machine_limits

Retract Distance

Determines the retract distance of the tool from the part if a large angle change is detected based on the limit defined by angle change limit.

retract_distance

Interpolation Distance

Sets the interpolation distance step in MLC. The postprocessor will interpolate between two tool tip positions (part coord.) using this threshold value.

interplat_distance

Angle Change Limit

Angle change limit in degrees from one posted tool path position to the next one.

angle_change_limit

Interpolation Angle Step

Interpolation angle step in degrees; the postprocessor will interpolate between posted tool path positions using this angle.

interplat_angle_step

Pole Angle Tolerance

Defines the pole areas where the rotary axis and spindle direction are parallel.

pole_angle_tolerance

The tool path time calculated in the simulation process is multiplied by this factor. It is used to improve the accuracy of the work time calculations.

This parameter determines the extra time (in seconds) of every movement block. It is added to every block in order to improve the accuracy of the work time calculation.