The current 16.6 HotFix now provides support for the Altium to Allegro PCB Editor Translator. The translator will convert both PCB and schematic files into Allegro PCB Editor and Allegro Design Entry HDL (DEHDL) files. Look to a future HotFix for the availability of the Altium to OrCAD Capture schematic translator.
Running the Altium to Allegro PCB Translator
In Allegro PCB Editor under the File menu select Import, Cad Translators, Altium PCB:
Note: A non-legacy PCB designer license must be used for the menu to appear:
Browse to the ASCII PcbDoc Altium design file to be translated (see the note below on exporting the ASCII version of the Altium design):
When the “Create Individual Symbol Definitions” box is checked, the translator will generate a separate symbol definition for each instance of a component by adding a suffix. For example 0805_1, 0805_2, 0805_3 and so on. This allows you to account for instance-specific footprint modifications within in the Altium design. By default this option is unchecked, which means that the translator will create one symbol definition only for a given Altium footprint. Use this option only if instance-specific changes have been made in the Altium design.
Running the Altium to DEHDL Schematic Translator
In Allegro PCB Editor under the File menu, select Import, Cad Translators, Altium Schematic to DEHDL:
Browse to the ASCII PrjPCB Altium design file to be translated (see the note below on exporting the ASCII version of the Altium design). Then select the output project directory. By default, the translator tries to match the look of the original schematic. There are two options to control the graphics:
- Simple Symbol Graphic: Enabling this option will ignore any custom symbol colors defined in Altium
- Simple Symbol Pin: Enabling this option will ignore any custom pin shapes defined in Altium
Translating a Schematic and PCB Design Project
The process to translate an entire Altium project (schematic and PCB) is to first translate the schematic into DEHDL. Next, from the translated schematic, export an Allegro netlist into a new empty Allegro database. Then run the Altium to Allegro PCB translator from that Allegro database. Using this method ensures that the Altium2PCB translator will consider the netlist and device logic already imported and start to translate only the remaining data in order to complete the board.
Exporting the Altium Project to ASCII
To translate an Altium project, the Altium schematic and PCB database (.SchDoc & .PcbDoc) need to be in ASCII format, which is accessible under the file save data type in Altium:
Feel free to share your experiences using this new translator!
Jerry “GenPart” Grzenia