Creating Custom Libraries using PCAD Library Manager
Creating a custom library for your design may be one of the most important steps in the design process. You will be extracting component information from many libraries for your design. Unfortunately, Accel does not store the information regarding which libraries your components come from. This is why it is important to create a custom library so there is no doubt as to where the components live for that particular design. Whether you create it at the very beginning of the design process or you create it after you complete your schematic, the bottom line is create it. Now, let's take a look at both methods for creating a custom library.
Creating a custom library up front
The first thing is to create a new library to copy all your component information into. Open Library Manager or Library Executive and select New from the Library pull down. Select a directory to save it to, then give it a unique name, such as the base number of your drawing number series (C0600) or the board name (RF Conv). Numbers tend to work best, but it's a personal preference type of thing. Click Save. Now you can begin copying components into your new library or you can begin creating new components in your library.
To copy components from existing libraries, select Copy from the Library pull down menu. Begin by clicking on Destination Library and select the library file you just created. Now, click on a source library and select a component. Click on it and click copy. Now click on the button Browse to Add and notice how your screen looks.
You can use this if you are wanting to verify a component pattern or if your just not sure what a particular component looks like.
You can click on the name of the component you are interested in and switch between the symbol & pattern views of it. Once you have decided that is the component you want, click on OK and notice that in your copy window, that component is now highlighted. Click on copy to copy it into your custom library.
Let's look at what we have in our custom library. Select the Component menu pull down and click on Open. Find the library you created with the Library New command, in this instance custom.lib., and click open. You should now see the names of all the components you just copied using the library copy command.
These are the components you have determined you will be using in your new design. Continue to copy components into your custom library or create new ones until you have all the components you will need to do your design. This is now your custom library for this design.
Archiving a custom library once your schematic is complete
Once you see the procedures for this method, I know your going to say, "This is the easiest way to go. I think I will do all my designs like this." I agree that this is certainly the easiest method. However, if you are working on multiple designs (or you share a machine with someone else that is doing Accel designs) and you use different libraries per design, you could find yourself in trouble fast. Here's why...to create a custom library through Archive Library, you MUST have all the libraries you used while drawing your schematic added in through Library Setup for Accel to find all the components to archive into your library. If you don't, it won't be able to find the information and your components won't get added to your new library. If you are going to use this method, I might suggest that you keep a list of the libraries you are using so you can make sure you have them all when you do get ready to archive.
Open your schematic and make sure all the libraries you used are open, by using the Library Setup command. Now, from the Library menu pull down, select Archive Library.
You will be prompted to give it a name, usually it is a good idea to name it the same as your design or your schematic, type in the name and click save. When it is done archiving, it may display a list of errors, something like this:
|Archive Library Log
Component CD4001AD was placed from library RCACMOS1B.LIB. Library RCACMOS1B.LIB is not one of the open libraries. Open libraries will be searched for component CD4001AD.
Component MC14490 was placed from library DAVES.LIB. Library DAVES.LIB is not one of the open libraries. Open libraries will be searched for component MC14490.
Component MC14490 was not found in any of the open libraries.
As you can see, this archive was not successfully created. If you were to look at what it did create, you would see that it did not create the MC14490. If I look at my error report, I see that I need to add the library DAVES.LIB. Once I add this through Library Setup, Archive will create this component.