1. MMI172 ExpressSCH & ExpressPCB Quick Tutorial and Design Notes
Sanket Kulkarni Graduate Teaching Assistant Music Engineering Technology
University of Miami
Spring 2018

2. Glossary
Schematic: In electrical engineering, a functional representation of how various devices are connected in the design.
Generally does not look like the physical board
Not to scale, does not include physical dimensions
Created before layout
Layout: In electrical engineering, the layout is the mechanical drawing representing the physical arrangment of the board.
Layout must show everywhere to place copper, silkscreen text, and drill holes:
All component pins, wires (traces) on the board, vias, mounting holes, plane fills, etc.
All dimensions must be accurate so that a manufacturer can build and assemble the board correctly

4. Glossary Mil: 1/1000 inch (0.001”) PCB: Printed circuit board
Standard unit of measure on circuit boards in U.S.
PCB: Printed circuit board
Symbol: Symbolic representation of a part in a schematic
Footprint: Physical representation of a part representing how it looks on the PCB
Trace: A single wire on the circuit board
Net: Signal with all its connections
May be comprised of multiple wires/traces in schematic/PCB
Via: A plated hole in the circuit board that connects traces on different layers
Plane fill: An area of the board (top and/or bottom layer) covered with copper, typically used for power and ground planes

5. ExpressPCB Design Flow
Create schematic ExpressSCH
Check schematic for errors and fix (do this in ExpressSCH)
Place parts in ExpressPCB
Leave adequate clearance between components
Observe component orientations
Place bypass capacitors as close as possible to the power pins of the op-­‐amps (while leaving adequate space)
Choose the correct part/footprint
Manually assign them part ID's that match those used in the schematic (this is super important!)
Link schematic to PCB (do this in ExpressPCB)
Route nets
Use default 10 mi (0.010") traces for low-­‐power analog and digital signals
Use wider traces for higher power traces (see
Use wide (50-­‐100 mil, i.e ­‐0.100") traces or (better) plane fills for power signals
Keep all traces as short as possible
Dont' forget to connect the appropriate signals to the edge connectors!
Check layout for errors. Unfortunately, this is a manual process in ExpressPCB. (You get what you pay for.) The best way is to highlight a net/pin and make sure you have a trace going to every pin that is highlighted.

6. Create Schematic in ExpressSCH

7. NOTE: Dots show connections
No dot, so these nets are not connected
Dot shows these wires are connected

8. Op-­‐amp power supply pins always have decoupling caps connected to POWER GND

9. Op-­‐amps with COMP pins need a compensation cap (check datasheet)

10. Op-­‐amp BAL pins are typically not used in audio – leave them unconnected

11. Bulk bypass caps are needed in every design (one pair per power supply)
Note capacitor polarities
There is no need to provide bypass for unused supplies

12. Check for Errors (& Correct)

13. General Tips – SCH
Pay careful attention to global nets like GND and power rails
Generally, schematics use only 90° angles for nets
– Unlike layout, in which 45° angles are fairly common
When saving parts that have multiple symbols inside them (e.g. NE5532 dual-­‐op-­‐amp) in ExpressSCH:
Group one individual op-­‐amp to make a symbol
Group the other individual op-­‐amp to make a symbol
Select both op-­‐amps together and save as a custom part
This makes it so that you get both op-­‐amp symbols when you place the component, but you can seperately move them around the schematic
Make sure to give both symbols the same Part ID (e.g. U1) or ExpressPCB will think they are two separate chips.
Check pin numbers and make sure they match the datasheet

14. Gotchas — SCH
Be wary of nets that look connected in ExpressSCH but are not
To be connected to the pin of a component, the net must terminate at the little dot at the end of the pin
To be connected to another net (wire) in the schematic, there must be a dot at the intersection
ExpressSCH does not automatically update ExpressPCB
If you add components to the schematic in ExpressSCH a>er you have already linked it to the pcb file in ExpressPCB, you must link it again aler adding the components
Otherwise, ExpressPCB will not know about the components you added in ExpressSCH

15. ExpressPCB Design Flow
Create schematic ExpressSCH
Check schematic for errors and fix (do this in ExpressSCH)
Place parts in ExpressPCB
Leave adequate clearance between components
Observe component orientations
Place bypass capacitors as close as possible to the power pins of the op-­‐amps (while leaving adequate space)
Choose the correct part/footprint
Manually assign them part ID's that match those used in the schematic (this is super important!)
Link schematic to PCB (do this in ExpressPCB)
Route nets
Use default 10 mi (0.010") traces for low-­‐power analog and digital signals
Use wider traces for higher power traces (see
Use wide (50-­‐100 mil, i.e ­‐0.100") traces or (better) plane fills for power signals
Keep all traces as short as possible
Dont' forget to connect the appropriate signals to the edge connectors!
Check layout for errors. Unfortunately, this is a manual process in ExpressPCB. (You get what you pay for.) The best way is to highlight a net/pin and make sure you have a trace going to every pin that is highlighted.

16. Open Template in ExpressPCB

17. Place Components on PCB

18. Assign Part IDs to Match Schematic

19. In Express PCB: Link PCB to Schematic…

20. …by selecting your schematic file

21. Components in the schematic are now linked to components with the corresponding Part ID in the layout.
E.g.:
The so>ware now knows that R1 in the schematic is the same part as R1 in the layout.

22. Now You Can Highlight a Net to Show Its Connections
Then click on a pin. Notice all pins connected by the net are now also highlighted in blue.
Click here

23. Route the Net Click here to route a trace
This sets width of trace that will be routed
These buttons control which layer the trace will be added to: Red = Top Green = Bottom
(Note that you can also add text. We’ll cover that and the Silkscreen layer later.)

24. Vias Connect Traces on Different
Layers
2. Choose via type here
1. Click here to activate via tool
3. Click to place via in desired spot. The green trace (bottom layer) and the red trace (top layer) are now connected by this via.

25. Controlling layer visibility
Remember: Red = Top layer
Green = Bottom layer Yellow = Silkscreen
These buttons control which layers are displayed (click to toggle)

26. General Design Rules Leave adequate clearance between components
Observe component orientations
Place large or critical components first
Place bypass capacitors as close as possible to the power pins of op-­‐amps (while leaving adequate space)
Use one layer (top or bottom) for horizontal traces, and the other layer for vertical traces
Keep all traces as short as possible
Route critical traces first
Try to minimize the number of vias on critical signals and power traces
Use wide (50-­‐100 mil, i.e ­‐0.100") traces for power signals and signals that will carry a lot of current
More good tips at (read them!):

27. Power Supplies Use the correct power rail
– +48V phantom power is generally only connected to input signals via a resistor
Never used for op-­‐amps
This high voltage will destory them
Block from op-­‐amp inputs using a blocking cap
Pay attention to op-­‐amp power rails
Be careful when rotating or flipping op-­‐amp symbols to note which is +Vcc pin and –Vcc pin
Reversing the power supplies will destroy the op-­‐ amp

28. Grounds Use the correct ground: Earth or power GND: Analog GND:
Use for bypass caps and connections to power pins
Analog GND:
Use for any connections that touch the signal path (pull-­‐up/-­‐down resistors, filter caps, etc)
Chassis GND:
Connect to mounting screws only

29. General Tips – PCB Be careful with clearances:
Remember that unlike in schematics, if two signals cross each other on the same layer in ExpressPCB layout, they are connected
Unlike SCH, if two things on the same layer look like they are touching in the PCB, then they almost certainly are and are therefore connected.
Use the correct pad to connect to plane fills:
Use thermal pads to connect components to plane fills
Use normal pads to connet vias to plane fills
Try to place most of the components (esp. large ones) in the layout before
you route any traces
Make placement of bypass capacitors a priority
Remember that you must use vias to connect traces on the top layer to traces on the bottom layer
Remember that through-­‐hole component pads extend all the way through the board and that components have pads on the bottom of the board

30. Gotchas — PCB ExpressSCH does not automatically update ExpressPCB
If you add components to the schematic in ExpressSCH a>er you have already linked it to the pcb file in ExpressPCB, you must link it again aler adding the components
Otherwise, ExpressPCB will not know about the components you added in ExpressSCH
Be careful when moving components in the layout: ExpressPCB will keep things connected that are, but it does not make sure things that should not be connected stay unconnected
It will short routed traces together without warning
If moving components, it’s olen better to delete attached traces, move the component, then re-­‐route the traces to it.
Remember that ExpressPCB puts the referenc designators inside the component body by default
Unfortunately, the component bodies will obscure the reference designators for the parts when the components are soldered to the board
So you need to move them to where they will still be visible aler the part is soldered down.

31. Route in 1 Direction on Each Layer
Note how the top layer has mostly horizontal traces, bottom layer mostly vertical traces
It does not usually matter which layer is used for a particular direction.
Horizontal traces could have been routed on the bottom layer
Routing horizontal on the top layer is a little easier because the edge fingers are on the top layer
Diagonal traces can go on either layer

32. Route Using 90° and 45° Angles
This is more a matter of aesthetics
Other angles work fine but look “unprofessional” to some (thus frowned upon)

33. Minimize the Number of Vias
It’s true that as a rule horizontal traces generally go on one layer and vertical on the other, but you should also try to minimize vias.
The following page shows several cases where I broke the “rule” and because it saved vias.
It is common practice to route following the rule, then later remove vias where you find opportunities to do so.
There is olen a trade-­‐off between minimizing vias and minimizing traces lengths. Just try to strike a reasonable balance.

34. Minimize the Number of Vias
Note these signals are routed on the bottom layer even though they are horizontal because it saved using vias
Note these signals are routed on the top layer even though they are vertical because it saved using a via

35. Minimizing Vias
Notice how this large via was eliminated by moving the vertical trace from the bottom to the top layer
Double-­‐click on a trace to edit its properties

36. Routing Power and GND Traces
Remember that these pins need to carry more current than a typical signal trace – therefore need wider traces: –
Whenever routing wide traces, uses correspondingly larger vias
When routing power and GND traces, use wider traces all the way to pin of the op-­‐amp IC
Better: use plane fills for ground and/or power rails
Treat connections to anything that is connected to a chip’s power and GND pins (e.g. bypass caps) just like power pins
Connections to pull-­‐down resistors and filter caps can be narrow

37. Routing Power and GND Traces
Note wide traces need large vias if going to other wide traces
Note very wide traces on main trunks of power and GND signals
Note wide traces to power pins and bypass caps

38. Routing Balanced Signal Pairs
Try to route the two signals in a balanced signal pair together as much as possible (best effort)
Improves noise immunity
Noise imparted on one signal is likely to also be equally imparted on the other and will be canceled through common mode rejection
Example: See routing for Input +4dB Cold/Hot signals from edge pins to resistors R2 and R1 in layout below

39. Other Layout Tips Avoiding crosstalk and noise:
Avoid routing critical audio signals parallel to traces which carry a lot of current
E.g.: In amplifiers, avoid routing input signals in parallel with high amplitude output signals
If digital signals are present on the board, keep them away from analog signals
Digital signals generate a lot of noise and crosstalk
In all of the above cases, it is okay to cross over/under the other signal on another layer at a 90° angle
Just avoid routing them in parallel (on either layer)

40. End