Gildemeister machines are now supported in Code Wizard by the adaptive-gildemeister.cgx and adaptive-gildemeister-inch.cgx files.
New Code Generator operator for concatenating two strings - STRCAT("abcd", "efgh") produces "abcdefgh".
The Code Generator directive %INCLUDE can now have a path to the included source code text file. This can be a path relative to the location of the main 'including' source code file, or an absolute path. Examples:
%INCLUDE=include.mac (included file in same folder as including file)
%INCLUDE=codeFragments\include.mac (included file in sub-folder of including file's folder)
%INCLUDE=C:\codeFragments\include.mac (absolute path)
New for safe turret parking:
In Code Wizard, new settings for the Turret Park command. In Machine Parameters ► Turret 1/2, these are Main Park Position and Sub Park Position (X, Y and Z, in absolute machine coordinates). For ATCs, there are additional B angle settings, Angle at Main Park and Angle at Sub Park. These values are written to the Code Generator MT lines (see below).
Note that the 'Sub Park' settings are for the opposite end of the machine to the 'Main' positions - they are still valid even if the machine has no sub-spindle.
In Code Wizard, new Turret Park and Turret UnPark code constructors for upper and lower turret.
In Code Generator, new PARK macro using the following variables:
|
XMOVE YMOVE ZMOVE |
Park position in Initial CPL coordinates |
|
POSITION |
Turret index position. Null if not specified |
|
BMOVE |
B axis park angle. Null if no B turret present |
|
SUBFUNCT |
Applicable position 1 = Main, 2 = Sub |
|
XPARK YPARK ZPARK |
Park position in machine coordinates |
In Code Generator, new position numbers for safe turret parking in the MT line. These are 37 to 40 = Main Turret Park Position X, Y, Z, B (angle), and 41 to 44 = Sub Turret Park Position X, Y, Z, B (angle).
New Code Wizard option Force Move After Toolchange. This is useful when a toolchange will be made, but no tool move will be involved (the new tool starts at the same position as the old tool finished). Previously there would be no move code output, and hence no TLO. Now you can check the option, which forces a move code output (by the Rapid After Toolchange code constructor), with the associated TLO. The new option is in NC, Style G-Codes and Modality ► Tool Change tab, for all adaptive templates. The default setting is unchecked, to maintain compatibility with older parts. If you check this, you should check the effect on your machining.
In the Code Wizard, TNC template, new tokens CYCL-CODE (cycle number) and CYCL-DESC (cycle description). Used to correct the functionality in the latest version of the Modify Hole Cycle code constructor.
New for holder-compatible tool selection (see also related changes in Strategy Manager and ToolStore):
In Code Generator, new HOLDERTYPE system variable. This is set to the new Holder Type value of toolchanges. The system variable can be used in generating setup sheets, for example. (Note that the Holder Type setting for tools also has an associated new Strategy Manager instruction modifier.)
In the Code Wizard, Machine Parameters dialog, Turret 1 and Turret 2 tabs, new tool Holder Type setting (select from the list of typical types, or type in your own value). In the code generator source code this appears at position 45 of the MT line. Made available to strategies as a Machine attribute.
In the Code Wizard, Machine Parameters dialog, Turret 1 and Turret 2 tabs, new Filename Suffix settings. These allow you to specify the suffix to be used to identify the turrets' NC code files. The settings are only available with Tape Output set to 'Two' (Machine Parameters tab), producing separate NC code files for each turret. The default settings are '-1' and '-2', which were the previous (fixed) values. In the code generator source code, the suffix values appear at position 46 of the MT line.
In Code Wizard turn templates, the duplication of the Maximum High Feedrate setting has been removed. The setting in NC Style, G-Codes and Modality ► Rapid Traverse has been deleted, leaving only the version in Machine Parameters dialog ► Machine Parameters tab.
Although you would probably have made both the settings the same, on creating your code generator, you are recommended to check this before updating. To do this open the CGD into Code Wizard, making sure you decline the automatic prompt to update. Now check the settings, making sure the Machine Parameters version is correct. Now update using File menu ► Update (at this point you will lose the setting in Rapid Traverse).
To make the tool (tip) Angle available to code generators, the toolchange macros (15 and 165) now set the new system variable INCLUDEDANGLE. Associated with this is the new Code Wizard token TOOL-ANGLE, available in core toolchange and Set Tooling Data List code constructors.
New Code Generator system variable NUMBEROFTEETH storing the number of teeth of the current tool. This is set by the toolchange macros (15 and 165). Use for setup sheets, for example.
New Code Generator system variables: TOOLMODE (driven=1, fixed=0), HANDOFTOOL (right=1, left=2, neutral=3), TOOLREVERSE (non-reverse=0, reverse=1). These are set by the toolchange macros (15 and 165). Use these for setup sheets, for example.
New facility for outputting PROGID to NC code. Previously this would have to be specified each time NC code was generated. Now this information can be stored in a job, for retrieval and outputting to the code. Related to this are:
New job fields Program ID and Program ID 2.
For outputting these new fields to code, new Code Generator system variables JOBPROGID1 and JOBPROGID2.
Changes to the template logic mean that the information is retrieved from these new variables if set, or from the existing PROGID variable otherwise.
For controlling whether there is a prompt for the information on NC code generation, there is a new Code Wizard setting NC Style, G-Codes and Modality ► Interactive Startup.
The settings are Always Ask, Ask if Not Set and Never Ask. If 'asking' is enabled and the user inputs information, this overrides the job information, otherwise the job information is used, if present.
New Code Generator system variable RAPID3D. This has been introduced so that the Hole cycle is aware of the Machine Parameters ► Rapid 3d setting, and outputs moves appropriately. The has been introduced to all milling templates.
New code constructor PDI Attribute Extension. This is for use in PDI customisation, and produces the macro ATTRIBUTE_EXTENSION. These changes are to allow the use of the system variable SUBFUNCT without clashes with other uses of the variable. The new ATTRIBUTE_EXTENSION macro is called when SUBFUNCT is less than 200. As standard the code constructor produces a 'dummy' macro - you should modify this to suit your customisation. You still need to 'trap out' SUBFUNCT values such as 2 (=secondary feed rate).
More macros now set #MACRO. These macros are: 103, 104, 105, 106, 108, 109, 113, 117. You should check your customisation, as #MACRO is used extensively.
Changes to helical arcs in the TNC adaptive template:
Circle centre points are no longer modal. The point will always be fully specified.
The linear block has been removed from between the centre definition and the arc move.
XY circle end positions have been removed from the arc block, as they are not needed for the polar coordinate mode that is used.
Where a series of helical moves is followed by a 2D "clean up" pass, this last pass is also output in polar (IPA360) form. This avoids problems with some TNC controls. Issues can arise when rounding requires the 360 move to be slightly more or less than the nominal full circle.
New Code Wizard options NC Style, G-Codes and Modality ► Reverse Y Main Spindle Driven Tools and equivalent for the sub-spindle. Use these to invert the sign of the Y coordinate output as appropriate. These are in the adaptive turning templates.
New Code Wizard options for the New Rough Turning cycle, in NC Style, G-Codes and Modality ► Turning Cycles G-Codes:
The new Return to Start option can be set to Ignore, Within Cycle and After Cycle, and comes into effect when the cycle has 'Finish At' set to 'Cycle Start' (previously this setting was ignored).
Support for CRC code output. This needs to be enabled in the cycle, and Cycle Clearance Move at End needs to be checked.
(Also note that the CRC code can be output on the first rapid move in a Rough Turn cycle - the COMPGCODE token may need to be added to the Rapid Move code constructor.)
In Code Wizard, changes to the default settings for thread turn canned cycles in the Okuma template:
G code changed to G71 and various other field addresses changed.
New token THREADTOTDEPTHDIAM, for diametral depth. This is now the default but if a radial depth value is needed the old token is still available.
The other depth tokens have been modified to use # variables. Also DIAM variants have been added using the same variables, modified according to template radial/diametral settings:
|
Token |
Variable |
|
START_DEPTHDIAM |
#DEPTH2 |
|
FINAL_DEPTHDIAM |
#DEPTH3 |
|
SPRING_DEPTHDIAM |
#DEPTH4 |
New code constructors in General
Motion that support 3D (XYZ) approach moves (as produced with Rapid
3D set (checked) for the machine in Edgecam). These are First
Z After Toolchange (Feed) and First
Z After Toolchange (Rapid).
The original 'Rapid-After-Toolchange' and 'Feed-After-Toolchange' code
constructors remain. To control whether the original or new code constructors
are used, there is a new option NC, Style
G-Codes and Modality ► Tool
Change ► Apply TLO.
Set this to First Move (original
orthogonal code constructors) or First
Z Move (new code constructors, with TLO being applied to first
move with a Z component after the tool change).
For head-head machines the 'First Z Move' setting will give best results,
avoiding moves out of limits when approaching in an angled CPL (tool axis
skewed relative to machine linear axes). For table-table machines either
will be suitable depending on the machine capability and user preferences.
New 'override Edgecam setting' options in NC, Style G-Codes and Modality ► Feed Moves options. For a range of tool types you can force a 'per Rev' or 'per Minute' output (or accept the Edgecam setting and not override).