Archive of the former Yahoo!Groups mailing list: Homebrew PCBs

Norm,
First the individual Components (schematic symbols) and Patterns (PCB foot prints) are not stored as separate files but are combined into Libraries. A library may contain zero or more elements (components or patterns) and is saved as a file. Component and pattern libraries differ in their file extension, .eli for Component libraries and .lib for pattern libraries. There are two different editors for this and they both work about the same. There doesn't seem to be a "save to" or paste function available so it's a little different moving a component (or pattern) from one library to another.

In general I would not edit the DipTrace libraries as you risk loosing any changes if you should install and update, just edit on the ones you make.

Here are the steps to make a component library (pattern will be similar):
Launch the comp editor, use Library>New to make a new library giving it a name.
Once the Library exists you can add elements to the library.
Use Component>Add New to Library to add an "untitled" component. Then use the Component Properties Panel "Name" field to change untitled to your component name.
Now use the rest of the tools to make the component.
If you want another component do the same again.
Then use Library Save or Save as to save the library.
It's really fairly easy.

Now if you see a part in one of the DipTrace libraries you would like to modify and use you would normally copy it to your own library first. But there is no copy and paste. So the trick is first open up the target library (ie. My-component-lib) then use Component>Get from Library to go fetch a copy from the source library. This puts a copy in your current working library that you can now rename and modify. Don't forget to save your library before exit. The Get from Library can target your current library as well as others.

I find the best way to use DipTrace is to always go from schematic to PCB. If something needs to be fixed go back to the schematic fix it there adjusting the libs as necessary then refresh the board. In the PCB editor use renew from schematic by "component". Normally you don't use "By ref des"—don't know when you would use that, just stick with "by component". It uses a hidden index assigned to all the components that doesn't change as ref des can.

Other than that works very similar to Orcad. I use a lot of "connect by name" wiring on my schematics. I just add a stub to a pin and give it a net name with "connect by name property set" Any other stubs with the same name are connected just make sure to set the connect by name property.

Craig