A recently published AppNote on converting a PADS ASCII file to Allegro PCB Editor has eased the life of many users by providing a step-by-step methodology and appropriate debugging techniques. It also covers various scenarios where Allegro PCB Editor generates errors or warnings during the translation, and explains how to debug errors and obtain a neat board file (.BRD) to be used in Allegro PCB Editor.
The PADS translator can be launched from File > Import > CAD Translators > PADS, from within Allegro PCB Editor. This translator converts the PADS database files (.asc) into Allegro PCB Editor board database files (.brd). It is assumed that the PADS database being translated is completely placed and routed.
Prerequisites for running the translator
PADS Layout creates an ASCII database version file (.asc), which contains all information about decal, part type, part, signal (logical connectivity), route (physical connectivity), and graphics.The component mapping from PADS ASCII file to Allegro prototypes is as per the table given below:
This is the PADS to Allegro PCB Editor Layer mapping file. The accuracy of the translated Allegro PCB Editor .brd file depends on the accuracy of the Copper layer mapping in the layer mapping file (Options File). The default pads_in.ini file is located at <Cadence_Install_Folder>/tools/pcb/bin location. It is advised to have a copy of the default pads_in.ini file in the work area and modify it accordingly.
Steps involved in the translation
1. Create a PADS ASCII file from the PADS job file (.pcb).
2. Create an options file and map the PADS and Allegro PCB Editor layers.
3. Execute the translator.
4. If there are any errors, the translation fails. Open the pads_in.log file to view the errors.
5. Correct the errors either in the .asc or .ini files. At times you may need to recreate the .asc file.
6. Re-run the translator.
7. Open the translated .brd file and review all aspects (pad geometries, symbol geometries, stackup, shapes, and so on) of the design for completeness and correctness.
Note that the translator does not guarantee 100% translation of everything. You need to edit the design that can be maintained completely within Allegro PCB Editor.
The pads_in application reads the input file and determines the number of etch/conductor layers it uses. If all required program arguments are not specified, the translation Options dialog box appears as follows:
The window above allows the users to modify the pads_in.ini file before translation begins.
Avoid editing the default pads_in.ini file located at <Cadence_Install_Folder>/tools/pcb/bin, instead, make a copy of the pads_in.ini file in the working folder and modify the same.
The PADS to Allegro Layer Mapping fields defines the element-layer mapping. The list box contains all the PADS objects (Lines, Copper, Text, Decals, Pads and Vias) and the name of the class and subclass to be mapped with in Allegro PCB Editor. Although the default mapping is done according to the pads (.asc) file, users can map the class / subclass name if needed. Each element appears once for each PADS layer, for a total of 31 entries per element.
All 2D lines on PADS layer 0 are mapped to the BOARD/SUBSTRATE GEOMETRY class and the subclass ALL, which is not pre-defined. Lines on PADS layer 1 map to the ETCH/CONDUCTOR class and the subclass TOP/SURFACE and so on. The translator presets all-necessary ETCH/CONDUCTOR class mappings by default, even if a previous translation created the options file. This is also true during batch translations.
Files Generated during translation
The following files are generated in the output directory after translation is complete:
Most of these are temporary files generated for use by the translator. They remain in the output directory only for reference. The key file is the Allegro PCB Editor board (.brd) file, which is the output from the translation.
Refer to the complete AppNote for a detailed procedure about each of the steps involved in the translation and about the known problems and solutions.
Note: The above link can only be accessed by Cadence customers who have valid login credentials for Cadence Online Support (http://support.cadence.com).