How to Make a Printed Circuit Board (PCB)

From APL
Revision as of 15:11, 12 May 2017 by Aplstudent (talk | contribs)

Jump to: navigation, search

Open the program gEDA Schematic Editor. (gschem)

Choose Components and Build the Circuit

Using the Add component menu (looks like a 2 pronged power cable) select the various electronic components that will be on your board.

The filter option in this menu allows you to quickly type the part in order to find it rather than searching through the menus. (ie. ground or resistor)

Move the parts around similar to how they will be constructed on the board. This wont be the final layout, but make sure all necessary connections can be made. Then connect components by clicking the blue add nets mode button next to the add components button.

To de-select a component or a wire right click the mouse.

If you need to rotate or flip components for any reason, click on the component and then press er to rotate or ei to flip.

You can change the name and what is visible about the component by double clicking on it and changing the visibility settings about its attributes.

After the circuit is constructed and all connections are made correctly its time to add footprints to the components.

Assign Footprints

Footprints provide the information about the physical specifications of each part in the circuit such as size, number of pins, pin size... ect.

Most common circuit parts (resistors, caps,...) have pre-made footprints available, speciality parts need to have their footprints designed and saved. Once a footprint is made and saved it can be used in the future.

To assign a footprint to a commonly used part, double click on the component. Towards the bottom of the menu, below add attribute, select the name drop down menu. When the menu drops down, select footprint. In the value box, this is where you'll enter the code for the specific footprint needed. Common codes and naming conventions can be found at this website, [1]

After the value is entered, click add. Again keep in mind you can choose to make this footprint name not visible on the diagram. To assign the same footprint to multiple components, click on another component before closing the edit attributes menu, and again click add. This will add the previously chosen footprint to the newly selected component.

Custom Footprints

To build a custom footprint open the program pcb designer. The Via button in the lower left portion of the side bar menu corresponds to pins. Click and drag these vias where physical pins will. This requires measuring and planning on the physical component. There is mm measurements in the top right corner to tell where the cursor is so that you can be precise about where the vias are placed.

When all components have a footprint and when all needed connections are made you are ready to send this blueprint to the pcb designer program. Save your file at this time. Now in the command line use the command gsch2pcb. Make sure you are in the directory where the .sch file is. For example this is what your command line should resemble with different file names and in a directory where your file is saved. (gsch2pcb -d ~/pcb-mylib/ BridedTeePCB_preamp.sch).

When done successfully, the command line will give directions to continue. I have listed them below. 1. Run pcb on your file BridedTeePCB_preamp.pcb 2. From within PCB, select File -> Load layout data to paste buffer and select (this will be you files name) to load the new footprints into your existing layout. 3. From within PCB, select File -> Load netlist file and select to load the updated netlist. 4. From within PCB, enter :ExecuteFile(BridedTeePCB_preamp.cmd) to update the pin names of all footprints.