Recommended project directories structure

Question

I am new to Cadence software. Before starting working on a large project, I would like to know if there is a recommended or most common structure for the directories and files. 
 One option is to a single directory and all the files in there, but it does not look very convenient for large project. Another option is to have global directories for footprints, symbols, etc. This works fine for a single project, but with multiple projects then everything gets mixed. 
 In other EDA software tools I usually set up things like this: 
 ``` . ├── libs │ ├── lib_1 │ │ ├── 3D │ │ │ └── a.step │ │ ├── a.footprint │ │ ├── a.symbol │ │ ├── b.footprint │ │ └── b.symbol │ └── lib_2 │ ├── 3D │ │ └── a.step │ ├── a.footprint │ ├── a.symbol │ ├── b.footprint │ └── b.symbol └── main.project ``` 
 which is very convenient because 
 
 It remain local to the project, 
 if I reuse say `lib_1` in another project, I can simply symlink to it and use it without duplicating information or having to update any path, and 
 the working directories stay clean. 
 
 I tried to setup something similar for Allegro X but ended up having a lot of issues with the paths. Right now I have everything in a single directory, but I see an inconvenience when the project starts to grow.

bdc66a938f164d · Accepted Answer

For future reference, this is how I achieved what I wanted: 
 1. Within Allegro, go to "Setup/User preferences/Paths/Library" and add `$PROJECT_LIBS` to `padpath`, `psmpath` and `steppath`. 2. Create a folder next to your project called `libs`. 3. Create local project libraries with folders inside `libs`, e.g. `libs/connectors`, `libs/vias`, etc. 4. Create `open_project.bat` and paste the contents below into it, save it and close it. 4. Run `open_project.bat` (double click it) to open your project from now on. It will automatically and temporarily add all your libraries paths and start Allegro. 
 Important: The changes made by the script are temporary, meaning that it will not interfere with any other existing configuration and also next time you open your project, you have to do it through the script. 
 Script `open_project.bat`: 
 ``` REM Manual configuration below: set PATH_TO_ALLEGRO_EXE=C:\Cadence\SPB_24.1	ools\bin\allegro.exe set NAME_OF_PROJECT_FILE=main.mcm :::::::::::::::::::::::::::::::::::::: REM Get the directory of this batch file, we assume the `NAME_OF_PROJECT_FILE` sits right next to this script: set PROJECT_DIR=%~dp0 REM Initialize PROJECT_LIBS variable: set PROJECT_LIBS= REM Enable delayed variable expansion so the `for` loop does not fail: setlocal enabledelayedexpansion REM Recursively loop through all subdirectories in ./libs: for /R "%PROJECT_DIR%libs" %%L in (.) do ( if exist "%%L\" ( set PROJECT_LIBS=!PROJECT_LIBS! %%L; ) ) ::echo %PROJECT_LIBS% ::pause REM Launch Allegro with the project file: set PATH_TO_PROJECT_FILE=%PROJECT_DIR%%NAME_OF_PROJECT_FILE% start "" "%PATH_TO_ALLEGRO_EXE%" "%PATH_TO_PROJECT_FILE%" ``` 
 Note that the script works recursively, so you can have an arbitrary directory structure within `libs`, e.g.: 
 . ├── libs │ ├── lib_1 │ │ ├── component_a │ │ │ ├── 3D_model.step │ │ │ ├── a.dra │ │ │ ├── a.psm │ │ │ ├── pad_1.pad │ │ │ └── pad_2.pad │ │ └── component_b │ │ ├── 1.pad │ │ ├── 2.pad │ │ ├── 3D_model.step │ │ ├── 3.pad │ │ ├── 4.pad │ │ ├── b.dra │ │ └── b.psm │ └── lib_2 │ └── component_c │ ├── 3D_model.step │ ├── c.dra │ └── c.psm ├── main.mcm └── open_project.bat

excellon1 · Answer

Hi 
 In Allegro you can basically create any structure that you like, no real limitations. I have found a Global structure for the libs to work best. If your doing a number of projects just keep them in their own folder, You don't need to include the libs etc in that folder only things like the Schematic .Dsn, .brd pcb, Netlist . By way of an example, I kind of like the plain English approach, for example. Allegro Padstacks TH Allegro Padstacks SMD Allegro Vias Allegro Step Models Allegro Libs Allegro Modules Allegro Clip Files Allegro Templates Allegro Stackup 
 Under Allegro Libs one could have additional folders that describe the contents such as. IC Capacitors Resistors Diodes These are basically the foofprint containers that reside on disk. Its an easy read if browsing the disk or if you need to schedule backups etc in a corporate situation. When you create PCB footprints or ,dra's be aware that the footprint will be made up of a number of items. Typically these are. .pad = Padstack, .psm = Package symbol, .dra = Footprint. Depending on how you name your footprint and padstack etc over time it can be difficult to find the complete footprint on disk. One way around this is to take the approach of having the same name for each item. For example assume you are creating a soic8 footprint then the naming would be like this. SOIC8.DRA SOIC8.PSM SOIC8.PAD On disk it would be fairly easy to identify a complete footprint done that way. The 3 parts would get put in the folder IC on disk. Usually I create the folders first using windows explorer then point to them when configuring Allegro paths from within Allegro. Best Regards

excellon1 · Answer

Hi 
 For clarity & in relation to your specific question of "Recommended project directories structure" there are a number of parts to this and certainly the Allegro Configuration & Libraries are a part of this but it is not the whole part by a long shot. The Orcad/Allegro tool set is basically a "Siloed" type of system. That is each part Schematic Capture, Board editor, Pcb footprint & padstack creation all operate independently of each other. This is unlike similar products like say Alt that are based around a database where by everything gets combined into a database file type of project. If you are used to this type of thing, Its not going to help you in the Allegro world. You have to kind of think about the system as a whole & not just the PCB end of things. In the Orcad/Allegro flow what drives the PCB editor is Orcad Capture, Or the Cadence schematic tool. Orcad is fairly popular as a schematic tool goes so my assumption is this is what you are using. If you load up Orcad Capture and draw your schematic the physical output on disk will basically be a 2 folder system The root folder say c:\Orcad_Design will contain your project & the .dsn schematic file. When you create a netlist and then run the packager to create a board there will typically be a sub folder under the root folder and by default it is named Allegro. That folder is where the board would be. So since Capture is basically driving everything then the actual "Recommended project directories structure" is one Root folder and one sub folder for the board. That's it. Just two folders on disk !. In this flow the libraries are totally seperate from both Capture & Allegro. If your just learning the tool & if I'm not mistaken Cadence does offer some pre canned designs so as to kind of kick the tires and learn the system. Best Regards.

Stats

Recommended project directories structure

Community Guidelines