I am starting from scratch, so I will be creating all the components as well as the schematic. The first data entry step is to create the component library for the project, starting with the two components I know: MSP430F1121A and the JTAG connector. I am sure there will be others, but the first components I want to drop into the schematic are these, so there is no point to opening the schematic editor until I have them.
Every project needs its own component and pattern libraries. The internal name (not file name) of the component library should be "Project Components" and the internal name of the pattern library should be "Project Patterns". The "component" and "pattern" suffixes are important when I add both the component and pattern libraries to the layout project and DipTrace lists both names.
Creating new components is a two-step process, first create the component in the Component editor. Every component lives in a library, there is no option (other than exporting as an ascii file) to save an individual component. It is easy to have many libraries scattered around in many projects. However, all components in the project should be in the project-specific library. Even the basic resistors, caps, etc should be copied from the standard library into the project library. This protects the project from changes to the reference library that may happen later. Once the project is complete the new and updated components and patterns should be copied (back) into the master library.
In the component editor, create a pin for every connection point on the component. The location and orientation do not matter, as this is just for the schematic. Add shapes to make the component recognizable on the schematic, but it does not need to have any relation to its physical appearance. Name the pins, but make sure the pin names match the pin number on the physical part. This is critical, as it is how the schematic pins will be mapped to the board layout pads later.
Each pin can be assigned "Type" and "Electric" properties. It would be nice if these properties were used to assign the net classes in the layout, but that doesn't seem to be possible. It seems these properties are only used for Spice analysis.
Create an additional field for the component named "Library" and set it to the component library name. Create a field named "PnP" and set it to "SMT", "Hand", or "None". Add as many additional fields as needed, more information is always better than less (provided it is correct!).
It is my experience that creating a new component is a very short and quick task. So short that except for very large IC's with many pins, it is quicker to create a new component from scratch than to hunt for a component created by someone else. In addition, it is critical to use a naming scheme that is consistent with the PnP parts library. See . Creating the component for the MSP430F1121A with 24 pins takes about 10 minutes.
If there is an existing component in another library, I can copy the component by first creating a new blank component in my current library and then importing from the other library using "Component > Get from library...". Make sure to set the Library field to the name of this (destination) library.
Using the default settings, the size of the passive components (resistors, caps, etc) is out of scale (too large) compared to the multi-pin IC components. The scale is better if the spacing between the pins is increased from 2.54mm (1/10") to 5mm (1/5").