Moving to Altium Designer from Cadence Allegro PCB Editor
- Using the Import Wizard to Convert Allegro PCB files
- Importing Allegro Designs
- Analyzing Files
- Reporting Options
- Default PCB Specific Options
- Current PCB Layer Mappings
- Current PCB Options - Reviewing the Output Project Structure
- Output PCB Projects
- Using ASCII Conversion to Import Without Allegro
- See Also
The translation of Cadence® Allegro® Design files can be handled by Altium Designer's Import Wizard. Complete flexibility is found in all pages of the wizard, giving you as little or as much control as you would like over the translation settings before committing to the actual translation process.
Allegro ASCII Extract files (*.alg) can be created by running a batch process on an Allegro machine. See Using ASCII Conversion to Import Without Allegro. The ASCII files can then be translated, on machines without Cadence Allegro PCB Editor installed, to Altium Designer PCB files (*.PcbDoc). The benefit of this, is that you only need one licensed copy of Cadence Allegro PCB Editor to convert all of your designs into Allegro ASCII Extract files (*.alg), which can then be distributed to other team members for translation.
Using the Import Wizard to Convert Allegro PCB files
The Import Wizard can be launched from the Altium Designer's File menu. Choose Allegro Design Files from the list of File Types.
Files in the Import Wizard translate as follows:
- Allegro Binary PCB Design files (*.brd) translate to Altium Designer PCB files (*.PcbDoc).
- Allegro ASCII Extract Files (*.alg) translate to Altium Designer PCB files (*.PcbDoc).
Alternatively, drag your Allegro Design Files into the Projects Panel which will automatically launch the wizard in Allegro Import mode.
Follow the pages of the Import Wizard to customize and complete the conversion of your Allegro Design Files.
Importing Allegro Designs
Use the Add button on the Importing Allegro Designs page to load the Allegro Design files (*.brd) or (*.alg) for processing. Click on the Next button to continue through the wizard.
Note: If you to attempt to add Allegro Design Files (*.brd) to the Import Wizard and you do not have Cadence Allegro installed, the following warning will be displayed:
The Analyzing Files page is where each Allegro file is analyzed by the Import Wizard to check if the data is valid and if it can be translated.
The Buttons will become active when the analysis of the files is complete.
Use the Reporting Options page to enable or disable the settings for logging all errors, all warnings and all events respectively.
A Log Report in ASCII file format (*.LOG) is generated for each translated Allegro PCB file. This log is saved in the \Imported sub folder of your original Allegro files. Open the Log Report after translation in a text editor to examine the details.
Default PCB Specific Options
Specify Polygon Connect and Plane Connect Options for the PCB import process. Enable the Import Auto-Generated Copper Pour Cutouts option to import the voids that are auto generated in Allegro PCB Editor as cutouts when the file is translated. The default options are displayed below.
Current PCB Layer Mappings
All used Allegro PCB layers must be mapped to an Altium Designer layer prior to import when using the Import Wizard. Layer Mapping is a mapping between the names of the Allegro PCB layers and Altium Designer PCB layers.
Default mapping is provided by the Import Wizard to build the layer mapping for each PCB. Layer mapping can be customized for each of your designs to be imported. You may wish to import multiple Allegro PCB designs and map the same Allegro layer to the same Altium Designer layer. You can set your layer mapping once and use this layer mapping for all of your files to be imported.
The advantage of importing in this manner is that batch layer management can save time when importing multiple designs. The disadvantage to using this is that Default Layer Mapping is not always intelligent with differing structures in designs, and so some manual changes may be required.
Use the Menu button on the Import Wizard or right click on the Allegro and Altium Designer Layer Mapping List to manipulate the layer mapping of Allegro PCBs to Altium Designer PCBs. The Invert Selection menu item inverts the items that were selected to not selected and those that were not selected to selected in the Layers list of the Wizard. This is a handy way to quickly choose layers to map to Altium Designer layers.
You can use the Load and Save Layer Mapping Configuration files using the Load Layer Mapping and Save Layer Mapping menu items respectively to quickly apply layer mapping for Allegro and Altium Designer layers.
Current PCB Options - Reviewing the Output Project Structure
Each of the imported Allegro Design Files are located in a separate sub directory in a specified Project Output Directory. You can further customize the PCB projects by dragging Allegro Design filenames to other Projects in the PCB Projects list.
Output PCB Projects
The Output PCB Projects page is where each Allegro PCB is converted to an Altium Designer PCB document (*.PcbDoc) in a design project. This process can be time consuming due to intensive tasks such as loading geometry data, translating nets and components and generating vias and copper pour polygons. You can monitor the status bar on the bottom of Altium Designer workspace to see which operation is taking place. Please wait until the Cancel, Back, Next and Finish buttons are enabled to indicate the processing is complete.
If the translation process is successful, the Wizard is completed. You can click to close the wizard and start working on your translated PCB design in Altium Designer. Cleanup will be performed on this translated PCB document first before you can perform edits on it.
Read on to find out more about Altium Designer and your PCB designs.
Using ASCII Conversion to Import Without Allegro
An Altium Designer workstation that does not have a licensed Allegro installation is able to import Allegro ASCII Extract files (*.alg). The following procedure enables a Licensed Allegro user to convert Allegro binary *.brd files to Altium compatible *.alg files. The conversion must be run on the Allegro licensed machine.
- Locate the following two files in the \System folder of your Altium Designer installation (Summer 08 or later):
- Copy the two files to the folder containing the *.brd binary Allegro version 15.2 or 16 file.
- Open a command prompt, navigate to the folder containing these files and type the following:
- Surround your filename with double quotes if the filename contains spaces, i.e.:
Allegro2Altium "your file.brd"
- The ASCII file is now created in the folder. Copy the *.alg file to the Altium Designer workstation, Summer 08 (Version 7) or higher, and import using the Import Wizard.
Below are references to other articles and tutorials in the Altium Designer Documentation Library that talk more about the conceptual information as well as walking you through specific tasks. Remember, you can also browse through the Help contents, and use F1 and What's This at any time in a dialog for more details.
For more PCB project options, refer to the tutorial, Tutorial - Getting Started with PCB Design
For more FPGA project options, refer to the tutorial, Tutorial - Getting Started with FPGA Design
For a tutorial that steps you through all the basics of creating components, read Creating Library Components Tutorial
For a tutorial that steps you through all the basics of editing multiple objects, read Editing Multiple Objects
For an overview of Altium Designer's FPGA design, development and debugging capabilities, read Soft Design