Post Processor with Vector 10, JTS

The following functions and/or variables can be used in connection with "jobs" and the JTS option. Post processing functionality from prior Vector versions still remains and can still be used.

Generating the numerical control programs for a job can come only from the job table. The NC button "numerical control" in the job table generates the numerical control program. The NC program is generated in the order that process steps are listed in the job table. Changing tools is fully automatic. For the first tool the Macro is "toolchange0", for all further tool changes the macro "toolchange" is used.

Templates (CCT – Data)

To avoid re-entering the machine specific data for each session of Vector, a main cct file can be created for each machine. This file can have global variables, tool data, and macros stored in the Job List. In this way the data that is used repeatedly are available immediately after opening or importing. To create a template, save the drawing as a template type with File-Save As

Variable names are identified by the @-symbol before the name.

Global Variable (Symbol)

Global variables are defined in the Job list with the function "symbol". They can be used once or several times, in the creation of the functions on the Contour, Cycle and Macro menus.

NAME Defines the name of the variable. "@" is required before the name symbol.

VALUE defines, dependent on the type of variable, a default value.

Symbol type "Integer" defines a whole number value

"Real" defines a decimal number

"String" defines a text entry

The type "Integer" and "Real" can also be formatted numerically by clicking the Format button.

The variable "@programnumber" is pre-defined according to the syntax required for a particular CNC machine controller. The values are entered in the program number filed in the job table:

With Heidenhain - controls for example the program number is needed at the beginning and at the end of the numerical control program. Thus when the variable "@programnumber" is placed in the macro "start" and "end", Vector automatically writes the contents of the variable in the defined position.

NC-Macro Start NC-Macro End

Formatting

NC-Insert Machine to open the NC editor for a specific machine. Click Options-Format to view the formatting dialog:

Click the buttons under Format to view the formatting dialog for the specific word addresses.

Some NC word addresses require formatting. These can be customized with settings in the machine specific NC editor.

NC-Insert Machine to open the NC editor for a specific machine. Click Options-Format to view the formatting dialog. Click the buttons under Format to view the formatting dialog for the specific word addresses.

The following variables can be formatted:

@cdt Time * scale factor is used for the dwell time. The scaling factor converts the entered value. For example if the dwell time one enters is in seconds, and milliseconds is required in the numerical control program, then the scale factor is 1000.

@feed, @regfeed, @feedR The scaling factor converts the entered value Feed * scale factor equals the feed motion placed in teh NC program as required for the CNC controller.

@spindle, @regspindle The scaling factor serves to convert the entered spindle speed value. Spindle * scale factor equals spindle revolutions per minute

@toolnumber, @regtoolnumber The tool number

@toolcorrd the tool offset diameter or tool radius offset number

@toolcorrl The tool length offset number

Macro menu

Standard - macros

Macros can be called as part of the "job" in the job table directly. The macros "start", "stop" and "end" are available by default, in the list of those available from the pulldown menu of the function "macro" in the job table. Other macros can be addressed, by entering the name into the input line. The exact way of spelling and case must be identical to the listing in the NC-Macro menu of the NC editor.

Standard - macros from the job list:

start numerical control program start

stop numerical control program stop

end to numerical control program end

box stock this macro call is automatically added into the job list when a Job stock is added.

toolchange0 the first tool change

toolchange second and all following tool changes Vector recognizes automatically whether a tool for an operation must be changed.

Date and time variable: (global symbols)

@date enters the current system date in the following form in the numerical control program:

Day, Month, Current date, current time, Year

Example: Do November 16 15:41:00 2004

@year the year of the current system date

@month the month of the current system date

@day the day of the month of the current system date

@hour the hour number of the current system time

@minute the minutes of the current system time

@second the seconds of the current system time

@msecond the millisecond number of the current system time

Box Stock (macro box stock)

The volume extents for the defined blank in the job list under "job <

box stick >" are specified:

@xbmin indicates the smallest x-value of the blank.

@ybmin indicates the smallest y-value of the blank.

@zbmin indicates the smallest z-value of the blank.

@xbmax indicates the largest x-value of the blank.

@ybmax indicates the largest y-value of the blank.

@ybmax indicates the largest z-value of the blank.

Over the macro "box stick" can be written the mass of the blank into

the numerical control program. Example macro definition "box stick" for ISO and Heidenhain - controls:

Tool change (macro toolchange[0 ])

@jobname sends the name of the job entered with the job definition.

@regfeed Register designation "F" out. Example: Feed motion 120 results in, dependent on formatting, "F120"

@feed "F" sends the feed motion without register designation. Example: Feed motion 120 results in, dependent on formatting, "120"

@regspindle gives the number of revolutions per minute to include. Register designation "S" out. Example: Number of revolutions 1200 results in, dependent on formatting, "S1200"

@spindle sends the number of revolutions without register designation "S". Example: Number of revolutions 1200 results in, dependent on formatting, "1200"

@regtoolnumber the tool number with register designation "T" out. Example: Tool no.. "3" results in, dependent on formatting, "T03"

@toolnumber the tool number without register designation "T" out. Example: Tool no. "3" results in, dependent on formatting, "03"

@toolcorrd this generates – tool offset diameter or tool radius number.

@toolcorrl gives the tool lengths offset number

@toollength the tool length is sent.

@tooldiam sends the tool diameter.

@toolradius sends the tool radius.

@toolname sends the tool name.

@tcomment1 sends a tool comment.

@tcomment2 sends a second tool comment.

@jobname sends the name of the job entered with the job definition.

Contour Menu

The following variables are available to the Contour menu:

@l creation of the procedure movement

ISO: G XYZ IJK R

Heidenhain: L CC XYZ IJK RND

@comp the radius correction register designation "G" out.

Example: Radius correction "G41" results in "G41".

@regcomp the radius correction register designation "G" out.

Example: Radius correction "G41" results in "G41". This variable works modal, that is the correction does not change with empty contents of the variables.

@regfeed Register designation "F" is output.

Example: Feed motion 120 results in, dependent on formatting, "F120"

@feed "F" sends the feed motion without register designation.

Example: Feed motion 120 results in, dependent on formatting, "120"

@regspindle gives the number of revolutions per minute, with Register designation "S"is output. Example: Number of revolutions 1200 results in, dependent on formatting, "S1200"

@spindle sends the number of revolutions without register designation "S". Example: Number of revolutions 1200 results in, dependent on formatting, "1200"

@regtoolnumber the tool number with word address "T" is output. Example: Tool no.. "3" results in, dependent on formatting, "T03"

@toolnumber the tool number without register designation "T" is output. Example: Tool no.. "3" results in, dependent on formatting, "03"

@toolcorrd outputs Tool diameter/radius number.

@toolcorrl gives the tool length offset.

@toollength the tool length is sent.

@tooldiam sends the tool diameter.

@toolradius sends the tool radius.

@toolname sends the tool name.

@tcomment1 sends a tool comment.

@tcomment2 sends a second tool comment.

Rear spar Driver specially:

@textend this is for Heidenhain - controls only and gives contents of the Field "extra", Function options - drivers, in the numerical control program

Cycle Menu

@jobname sends the name of the job entered with the job definition.

@regfeed generates feed with register designation "F" out. Example: Feed motion 120 results in, dependent on formatting, "F120"

@feed "F" sends the feed motion without register designation. Example: Feed motion 120 results in, dependent on formatting, "120"

@regspindle gives the number of revolutions per minute with register designation "S" out. Example: Number of revolutions 1200 results in, dependent on formatting, "S1200"

@spindle sends the number of revolutions without register designation "S". Example: Number of revolutions 1200 results in, dependent on formatting, "1200"

@regtoolnumber the tool no. is generated with register designation "T". Example: Tool no.. "3" results in, dependent on formatting, "T03"

@toolnumber the tool no. is generated without register designation "T". Example: Tool no.. "3" results in, dependent on formatting, "03"

@toolcorrd generates tool diameter or radius offset number.

@toolcorrl gives the tool lengths offset number.

@toollength the tool length is sent.

@tooldiam sends the tool diameter.

@toolradius sends the tool radius.

@toolname sends the tool name.

@tcomment1 sends a tool comment.

@tcomment2 sends a second tool comment.

Drilling parameters

@czdepth the absolute drilling depth is sent.

@czretract retract level absolutely, Z-value after the drilling is completed.

@czrapid absolute z-position in rapid traverse to be started at.

@czsafe sends the absolute safety margin.

@feedR feed value for the retraction of the tool from the drilled hole

@cdt dwell time

@cdx lateral feed in X (incremental) when turning offBore

@cdy lateral feed in Y (incremental) when turning offBore

@cstepdz Drilling depth with deep hole boring (absolute)

@creddz reduction value of the feed (incremental)

@cmindz minimum feed

Parameter for drilling cycle coordinates

@c gives all drilling coordinates (X, Y and Z), inclusive. Register designation out.

@cx only the x-coordinate is generated with register designation "X" of the drilling position is output. With modal set the value only appears if it changes.

@cy only the Y-coordinate is generated with register designation "Y" of the drilling position is output. With modal set the value only appears if it changes.

@cz only the Z-coordinate is generated with register designation "Z" of the drilling position is output. With modal set the value only appears if it changes.

@ccx gives only the value to the x-coordinate, without register designation "X" out. This variable is always sent, even if modal is set.

@ccy gives only the value to the Y-coordinate, without register designation "Y" out.This variable is always sent, even if modal is set.

@ccz gives only the value to the Z-coordinate, without register designation "Z" out. This variable is always sent, even if modal is set.