It is easy to add your own parts to the Copper Connection Parts Library. Parts files are identical to standard PCB files, except that they are stored in a special location.
Before proceeding, make sure you know how to use the program, such as by completing the Getting Started tutorial.
For the first example, we are going to walk through the minimum steps, without any fancy options.
That's it. To see or use the part, choose "More Parts in Library" from the Part Tool menu in the Tools ribbon on the left side of the editor window.
Choose More to View the Parts Library
You'll find the part listed as Simple Example. If you're having trouble locating that part, type "Simple" in the Find field and press enter. Or, sort by Name.
Parts created in ExpressPCB are easy to use in Copper Connection. Learn how to use your ExpressPCB parts in Copper Connection.
Better parts have an id letter (standard designator), pin numbers, and a brief description. And, rather than one part per file, it is better for multiple similar parts to be included in the same file with a meaningful file name for organizational purposes.
To edit a part, right-click on the part in the Parts Library and choose Open Part File.
As an example, choose Open Part File on the DIP 8-pin part. The part file opens in the editor.
Multiple parts in a single part file
Look at that! It's just a regular PCB file with groups of elements in it. The file is named "DIPs.rrpcb" and there are multiple DIP parts in the file.
Select IC DIP 8-pin by clicking on it.
Click on a part to see and edit the part description
The entire part is selected, because it is a group. Elements that are not grouped are not considered parts.
In this example, in the Description section of the ribbon, the ID is "IC" and the part number (#) is "DIP 8-pin". ID can be blank, but it is helpful to provide a standard designator so that the part shows up on the Bill of Materials by default.
In the part number (#) field, some non-blank text is required for the group to be included in the Parts Library. The part number must be unique within that particular part file. That is, you cannot have a part with no name and you cannot have multiple parts with the exact same name in the same part file.
Optionally, you can add information in the note/purpose field that will then appear in the Parts Library when medium or large tiles are displayed.
Entering other descriptive information will appear in the Part Library window
In the File menu, under Board Properties, you can make any category you want for all of the parts in this file. The category is included in the list atop the Part Library window, to provide quick filtering.
User-definable categories in the part file's Board Properties appear in the Parts Library
In summary, here are the requirements for a part to be included in the Parts Library:
Recommended, but not required:
At startup, the software reads all of the PCB files in the User-Defined Parts folder, Built-In Parts folder, and their subfolders. The actual location of the parts folders depend on the operating system. To access the folders, go to the Parts Library window, right click on a part or empty area and choose the desired folder to open in Windows Explorer.
The part file's filename is not important, other than ensuring it has a readable filename extension (such as ".rrb" or ".rrpcb"). For example, you can store capacitor parts in a part file called "Diodes.rrb" if you really want to. The filename has no affect on the part or the part category. Furthermore, you can use the same filename in multiple folders, without conflict.
Although you can make changes to the files in Built-In Parts folder, they will be overwritten when the software is updated. Instead, place your customized parts in the User-Defined Parts folder.
Making changes to a part in a parts file will NOT alter any other files containing those parts. That is, when a part is placed on a board, copies of each element are made. It doesn't matter if the original is changed in the future -- there is no link back to the original. This prevents finished boards from breaking due to updated part libraries.
After making changes to a part in a part file, you need to save the file. Then, click the Refresh button in the Parts Library window to make the software re-read the part files -- otherwise changes will not appear until you exit and rerun the software.
A feature of the software is the ability to label the pins on the parts.
If it isn't enabled already, check ID Annotations in the View menu. This will let you see the pin numbers as you edit them.
Before grouping the part, select a hole or pad by clicking on it. Type the pin number (1,2,3 or +,-) in the ID field of the Description section of the ribbon. Type the pin function (Input A, +5V, Vcc, GND, etc) in the part number (#) field [which is a bit of a misnomer in this case -- sorry about that]. If applicable, type anything else helpful ("rail-to-rail") into the note field.
When all of the pads/holes have their description fields filled in, group the elements. Then provide the ID and part number of the entire group to name the part.
For this extra effort, your well-defined part will assist you in making and verifying the right connections. When ID Annotations is checked in the View menu, the pin numbers and part ID/name are shown on the board. When Info at Cursor is checked in the View menu, lots of valuable information is shown in a tool tip. Consider how useful this will be when placed on a board.
Pin information in a part
Tip: The pad or hole with the ID of '1' or '+' (if any) will be placed directly under the cursor when the user clicks with the part tool. In order words, a part is initially placed based on pin 1, if it exists.
What happens when you want to make a change to a single element on a part? When you Ungroup a part, the description information (ID, part name, and part notes) of the group is lost.
However, after you make your changes, you can select the elements and choose Group As→(part name) in the Arrange menu. The software remembered the description information during Ungroup, and can now associate it with the selected elements.
Restoring group description information
Alternatively, if you only need to modify one of the elements, there is a way that you select the element without ungrouping. The first click selects the group. The second click selects the element in the group. Make your changes as you would usually do (change the shape or size of the pad, change the element layer, delete it, etc). No need to re-group, as the part was never ungrouped.
First click selects entire part. Second click selects any individual element when still grouped with the part
Power users will appreciate the ability to generate parts using dimensions from a manufacturer's datasheet. Choose "New Land Pattern" from the Part menu in the Tools ribbon.
Choose New Land Pattern
A window appears with a variety of templates to choose from (see below). For example, to create an LM393 comparator, you would choose DIP from the upper-left pulldown menu. Then, enter the # of pads.
New Land Pattern
After that, only three dimensions (labeled in bold) are required: Y (Pad Length), E (Pad Pitch), and C (Row Pitch). If your datasheet doesn't include C, you can enter G or Z instead to auto calculate C.
Additionally, you can enter the Part ID (schematic designator) and Part Number, if desired. Also, you can enter the Pin Names to have the pads automatically assigned their pin name.
Click OK to close the window. Then, click on the board to place your part.
If you want to save your part for use on future boards, follow the steps at the beginning of this article to save the part to your parts folder.