nlited

I have collected all the pieces of the puzzle, now it is time to begin connecting them together: Control, Power, USB, Expansion, and Motor. Schematic capture is the process where I create the sketches that describe how all the components are wired together. The schematic describes the components only terms of their logical function, there is little or no concern about physical size or space. Wires can cross over any number of other wires and reach any component.

As I placed each component into the schematic, I add it to the Parts list in the AutoBOM. I don't need to specify the exact part yet, I can leave the component name, value, and part number blank; I just need to enter the RefDes to create a new row in the Parts list that will be filled in later. The schematic at this point is a sketch of the final design, I don't want to be bogged down in the minutia of looking up datasheets, the goal is to chunk in the functional blocks quickly, to discover any major design obstacles as early as possible.

Sheets should be 8.5x11" standard letter size.

When creating multi-page schematics, it is very helpful to include the sheet number in the component ID. For example, "R104" is a resistor on sheet 4.

Using "wireless" connections between pins removes the rats' nest from the schematics and makes off-page connections without requiring an extra port component.

The component symbol should match its physical pin layout as much as possible.

Sheets should be letter size. The biggest reason is that when debugging a circuit, I want to have a hardcopy for notes and easy reference. Since I don't have a 17x22" printer, a C-sized sheet will be reduced down to fit onto a 8.5x11" sheet anyway, with an end result of an unreadable sheet. The second reason is that it forces each individual sheet to remain simple, with only a single IC. This is a good thing.

It may be tempting to rearrange the pins on the schematic symbol for a component to tidy up the schematic. DON'T DO IT. The closer the symbol matches that actual part, the easier it will be to arrange the components on the board during the first layout, and makes tracing the from schematic from the layout much easier.

The first pass at the layout exposed some significant problems with the schematic. This was not a good thing, but it was also not surprising. I try not to spend much time trying to make a perfect layout during the first pass, there is a good chance I will find problems with the schematic that will trash the layout.

I need to be extremely vigilant and careful when renaming nets! DipTrace gives very little feedback when renaming nets and I have freqently renamed, merged, and lost entire nets unexpectedly. While trying to clean up the VCC_3V and VCC_5V nets I somehow merged the 5V net into the 3V, resulting in a real mess.

Do not rename a wire by changing the net name from the context menu. Instead, delete the wire first, verify that the pin has been disconnected from the net, then recreate the connection to the pin. The connection can be a wire or a "wireless" connection to a net.

For example, when I select the VCC_3V net in the design manager, I should not see any instances of a VCC_5V pin. This is where creating my own VCC_5V net port and setting the pin name has paid off, otherwise all of the components would be named "PORT1" and the pins would be named "1". Because this pin now belongs to the VCC_3V net, any time I try to connect a VCC_5V port it instantly joins the VCC_3V net. This confused the hell out of my for about 30 minutes. The only solution I could find was to first delete all the VCC_5V net ports, then rebuild the VCC_5V net.

After purging all the instances of VCC_5V from the VCC_3V net, I tried connecting the VCC_5V net port again. This time it finally worked.

Now I need to go back and reconstruct the VCC_5V connections I just deleted. This time, checking which net is actually used each time. This problem occurs when I notice that a net is wrong and I just rename it to the correct net. Big trouble if I forget to check "related wires only" OR if the wire is connectect to an off-sheet component OR if the wire is connected to a net port. It is safer to fully deconstruct the wire and rebuild it. In this example, the net between pin65 and C227 is erroneously set to VCC_3V when it should be VCC_5V. I can just right-click the wire and rename it to "VCC_3V" with "related wires only". This usually works as expected, but I need to be vigilantly watching the net in the design manager. I am finally able to wire up the power selectors correctly.

I have spent all day fixing schematic problems that were exposed during the first pass at the layout. It is time for a break, then I will review the schematic again before attempting another layout. Hopefully I will be able to reuse the existing board. Most of the work was around the A3967's, and not much changed around those devices.

Schematic Design