Other Parts Discussed in Post: OPA191

Applications engineers tend to overlook printed circuit board (PCB) layout during circuit design. It is often the case that a circuit’s schematic is correct, but does not work, or perhaps works with reduced performance. In this post, I will show you how to properly lay out an operational amplifier (op amp) circuit PCB to ensure functionality, performance, and robustness.

An intern and I were recently working on a design together using the OPA191 op amp in a noninverting configuration with a gain of 2V/V, a 10kΩ load, and a supply voltage of +/-15V. Figure 1 shows the design schematic.

Figure 1: Schematic of the OPA191 in a noninverted configuration

I tasked the intern with laying out the PCB for this design. I gave him some general guidelines for laying out PCBs – keep traces as short as possible and keep components close together to minimize board space – and sent him on his way. How hard could it be? It’s just a few resistors and a couple of capacitors, right? Figure 2 shows the first attempt at the layout. The red lines are traces routed on the top layer and the blue lines are traces routed on the bottom layer.

Figure 2: First layout attempt

That’s when I realized that PCB layout isn’t as intuitive as I thought; I should have been a little bit more detailed with the guidelines. He did everything I recommended, keeping the traces relatively short and the components close together. The layout could be improved, however, to reduce PCB parasitic impedances and optimize performance.

The first improvement we made is moving R1 and R2 next to the inverting pin (pin 2) of the OPA191; this will help reduce stray capacitance on the inverting pin. The inverting pin of an op amp is a high-impedance node and is therefore “sensitive.” Long traces can act as antennas, which allow high-frequency noise to couple into the signal chain. PCB capacitance on the inverting pin can cause stability issues. Therefore, the connections on the inverting pin should be kept as small as possible.

Moving R1 and R2 next to pin 2 allows R3, the load resistor, to rotate 180 degrees, which then allows the decoupling capacitor, C1, to move even closer to the positive supply pin (pin 7) of the OPA191. It is extremely important to place decoupling capacitors as close to the supply pins as possible. Having long traces between the decoupling capacitor and the supply pin adds inductance on the supply pin, which can degrade performance.

Another improvement we made concerns the second decoupling capacitor, C2. The via connecting –VCC and C2 should never be put between the capacitor and the supply pin; it should be in a place where the supply voltage must pass through the capacitor before entering the supply pin of the device.

Figure 3 shows how to move each component and via to improve the layout.

Figure 3: Location of components for improved layout

Even after moving the components to new locations, it’s still possible to make additional improvements. You could make the traces as wide as possible to reduce the inductance of the trace – about the size of the pad to which the trace will connect. Another is to pour a ground plane on the top and bottom layer. This will create a solid, low-impedance path for return currents.

Figure 4 shows our final layout.

Figure 4: Final layout

The next time you are laying out a PCB, make sure to follow all of these layout practices:

  • Make the connections to the inverting pin as short as possible.
  • Place decoupling capacitors as close to the supply pins as possible.
  • If using multiple decoupling capacitors, place the smallest decoupling capacitor closest to the supply pin.
  • Do not place vias between decoupling capacitors and supply pins.
  • Make traces as wide as possible.
  • Do not route traces with 90-degree angles.
  • Pour at least one solid ground plane.
  • Do not sacrifice good layout to label a component with silkscreen.

Additional resources

  • Hello Timothy Claycomb, thank you for your reply

  • Hello Nightwish_flf,

    Thank you for your interest in my blog. I have provided answers to your questions below.

    1. Yes, you can place the via on the pad of the C1, C2, R1 and R3. However, I have been told that in some cases when assembling the PCBs having a via on the pad of a component can cause issues. Therefore, I avoid any via on the pad of a component when possible.

    2. The reason VCC gets routed under Vin is because in a real application the input to the amplifier (Vin) would likely come from a sensor or the output of another amplifier. In that case it would be very difficult or impossible to route VCC around Vin. Therefore, to show what might occur in a realistic application, I routed the power supply under Vin. Also, in an end product there is a good chance that a company would choose to use manufacture a 4 layer (or more) board in which case there would be a solid power plane for VCC and -VCC which would eliminate the trace routing under Vin.

    Again thank you for your interest in my blog,

    Tim Claycomb

  • I  have some questions :

    1. the via maybe need to be placed just under the pads of the components C1,C2,R1,R3, to reduce the loop inductance

    2.is the VCC- routed in the top plane better? In the final layout, the power line is routed under the signal loop, each other coupling, maybe just route it around the VIN

    Hope for your reply. Thank you!

  • Great article Tim. Speaking of ground pins, here's some of the history behind it...


  • Hello Georgy and Farrokh,

    Thank you for your comments.


    These are very good points you have mentioned. There are always things to consider when laying out a PCB.


    Are you referring to the ground connection to the via connecting to component C2? If so, the bottom ground plane connection is simply being covered up by the top ground plane. If I were to delete or hide the top ground plane, you would be able to see the connection to the via on the bottom ground plane.

    Thank you again for the comments,

    - Tim Claycomb