I'm trying to design a 4-layer PCB board and would like to check if the following layout will perform well. By well, I mean if it will perform optimally. Factors such as Low EMI and noise coupling etc.

I have the ATMEGA32U4 (U3) on the top layer. On the bottom layer I have the BNO055 Iertial Measurement Unit (U1) sensor and the 2 crystals (X1 is a 32.768kHz crystal for the BNO055 and X2 is a 16Mhz crystal oscillator) for the ATMEGA32U4.

strong text

I will be using the following 4 layer stack up.

enter image description here

I've tried searching online for similar scenarios however I am unable to find any documentation.

Any feedback or alternate layouts would be much appreciated too! (Hopefully in the same footprint 22.75mm by 12.75mm)

  • 2
    \$\begingroup\$ You say that you "would like to check if the following layout will be okay". What exactly are you unsure about? Please edit your question and clarify. \$\endgroup\$ Jun 30 at 11:46
  • 1
    \$\begingroup\$ What is an IMU? \$\endgroup\$
    – jonathanjo
    Jun 30 at 11:50
  • 1
    \$\begingroup\$ You are asking about a "layout", but there is no layout, yet. Just some placed components and a stack-up. It's not clear what you are actually asking about. \$\endgroup\$
    – feynman
    Jun 30 at 12:21
  • 2
    \$\begingroup\$ For it to be "optimal" you'd need to describe your criteria. In any case, you're missing a) decoupling caps, b) caps for the CPU oscillator (see datasheet fig 6.2), and the passives for the Bosch device (figs 5.4 and 5.5 of datasheet) \$\endgroup\$
    – jonathanjo
    Jun 30 at 12:25
  • 2
    \$\begingroup\$ The PCB layout could be relevant or irrelevant, as what components and connections you use are also important. For example the IMU needs 3.3V supply, and you have no regulator, how are you going to power the system? You need to design the system first, then implement it in the form of schematics and finally as PCB. I bet 4-layer board is not required at all for hobby purposes. For USB the 4 layers will almost be mandatory, but this is just for a couple of millimeters. \$\endgroup\$
    – Justme
    Jun 30 at 12:39

1 Answer 1


choosing a PCB stackup and determining an appropriate approach to component placement can be a challenging decision. I would like to offer you some advice based on my experience.


You need to select a stack-up for your PCB. There are various options available, each with its own unique advantages. However, it's important to note that these advantages may come at a cost. Here are some options listed in ascending order of cost:

  • Only Through-Vias from 1-4
  • Blind-Vias from 1-2, 3-4 and Through-Vias from 1-4
  • Blind-Vias from 1-2, 3-4 and Buried-Vias from 2-3

Different via types. See https://www.analogictips.com/printed-circuit-boards-part-3-vias-and-multilayer-boards/

Depending on the complexity of your layout, I would recommend designing for Option (1) as it is the most cost-effective and easily producible.

If this project is for a hobbyist endeavor, cost considerations become significant, and opting for cheaper PCB manufacturing services can be advantageous.

I also suggest selecting a manufacturer before commencing the design process. This allows you to consult their specifications regarding track size, spacing, drill diameter, restring, and other relevant parameters.


Best practice dictates, that the crystals should be placed on the same side as the component they are intended for. By doing so, the CLK signals can avoid the need for vias. This approach helps prevent issues related to signal integrity, EMI emissions, and other potential problems.


When utilizing a through-vias only 4-layer PCB, I often employ the following stack-up:

  • Signal
  • GND
  • 3V3
  • Signal

This arrangement provides capacitance between the GND and 3V3 layers, which helps mitigate EMI issues. Additionally, since only through-vias are used, there are no significant drawbacks in achieving a compact layout.

Recommended Layout

Please see: Circuit Board 4-Layer PCB Stackup Planning, Cadence or Advantages of 4 Layer PCB Fabrication, Hillman-Circuits or PCB Stackup Design Guidelines, MOKO Technology


The key to designing a successful and compact layout lies in prioritizing component placement and investing sufficient thought into it. By doing so, the routing process becomes significantly easier, ensuring shorter tracks and minimizing the need for excessive vias.

I commonly use this process:

  • Design the board outline based on mechanical specifications.
  • Place all connectors on the board anf lock them.
  • Position all large components, such as decoupling capacitors or inductors.
  • Group components into logical blocks (e.g., place decoupling capacitors near their respective pins, position the crystal next to the MCU, inductors close to the DC/DC IC ...).
  • Arrange these logical blocks according to the flow diagram (e.g., USB transceiver near the USB jack, MCU adjacent to RAM, DC/DC close to PWR-In).
  • For blocks that do not require a specific placement, prioritize the layout that minimizes vias and track lengths.
  • Spend ample time shuffling these blocks around until you achieve a satisfactory arrangement.
  • Don't hesitate to continue shuffling to optimize the layout further.

Important: If you can ease up your design by moving digital signals on the MCU, do it! The LED-GPIO can be any GPIO... So make your work a little easier!

Nice memory bus layout

Do you notice how well the memory bus is routed? All the tracks are perfectly parallel, and by making a slight adjustment to move the memory IC upwards, the fan-out process has become significantly easier.

This serves as an excellent example of how investing an additional 30 seconds of thoughtful consideration can save you up to an hour of routing time!

Please see: Guide on Component placement by PROTO-ELECTRONICS.com or 5 Basic Rules you need to know by Altium.com or PCB Component Placement Guidelines – Tips & Tricks by Circuits-DIY.com


Now you can commence with the actual routing. Typically, I follow this process:

  • Start by routing all decoupling capacitors first, connecting them from the VCC-IC pins to the capacitors themselves and from the capacitors to the ground (GND) layer.
  • Proceed by routing all IC-GND connections to the GND layer, utilizing vias when necessary.
  • Next, route all clock (CLK) and crystal (XTAL) signals.
  • Following that, route all high-speed digital signals, such as buses and memory interfaces.
  • Afterward, route all low-speed digital signals, including enable signals and chip-selects.
  • Then, route the VCC connections to the capacitors, completing the power delivery network.
  • Lastly, do the left-over signals like LEDs or Buttons.

Please see: Our Top 10 PCB Routing Tips by PROTO-ELECTRONICS.com or PCB Design Guidelines for Reduced EMI, Texas Instruments or The Top 10 PCB Routing Tips for Beginners, Autodesk or PCB Design and Layout Guide, Microchip


At this stage, your layout is considered 'finished.' Take a break to allow yourself some time away from the design.

After the break, resume the process and scrutinize the layout for any small details that may still need attention, refining it to achieve a state of near-perfection.

This additional examination is crucial because it often helps uncover significant issues that may have been overlooked earlier in the design process.

Evatronix PCB Layout

If you adhere to these procedures, you can achieve a well-designed layout like this with minimal time and effort. However, it's worth noting that the complexity of your project may vary, and accordingly, the time required may differ as well.


You can find further ressources here:

Rayming PCB&Assembly Guide on 4-Layer PCBs

Weller-PCB Discussion on common 4-Layer stack-ups

12-Rules to properly desing a PCB stackup by PROTO-ELECTRONICS.com

PCB Reliability: Design Guidelines for Manufacturing, VSE

Reliability Analysis (RA), MATEK

Design for Manufacturing (DFM) , Altium

PCB DFM Guidelines – Design for Manufacturing, FS Tech

PCB Layout Design for Manufacturability: 5 Mistakes to Avoid, Matric

Key Elements Affecting PCB Manufacturability, PcbCart

21 Design Mistakes to Avoid on Your PCB for Mass Manufacturability, Predictable Designs

10 Tips To Improve PCB Design For Manufacturability, JHY

  • \$\begingroup\$ Thanks so much for the long post!! Really appreciate this as I'm still very new and unsure of the factors I need to consider. I do have another question though, if I place the crystals one on top of the other so that the crystals sort of "sandwich" the PCB, would there be any issues? Not too sure exactly what issues there could be so can't really specify on this sorryy \$\endgroup\$
    – Yeo
    Jun 30 at 12:32
  • \$\begingroup\$ @Yeo Indeed, there can be potential issues to consider. However, it's important to note that these issues are typically more relevant when manufacturing PCBs intended for high-volume applications such as automotive systems with millions of units sold annually. In your case, these concerns may not be as critical, especially since avoiding vias in CLK lines can be advantageous. \$\endgroup\$ Jun 30 at 12:34
  • 1
    \$\begingroup\$ @Yeo But, as other commentators have pointed out: Spend a fair time on your schematic first. Make sure, all components required are present. Only then think about layout & routing! \$\endgroup\$ Jun 30 at 12:35
  • \$\begingroup\$ Thank so much for the great advice! \$\endgroup\$
    – Yeo
    Jun 30 at 12:39
  • \$\begingroup\$ @ElectronicsStudent - Hi, To comply with the site rule for content copied into a post from elsewhere, can you please add a link back to the original source webpage for any of those images which you copied or adapted from elsewhere and did not completely create yourself? I saw you mentioned the source URL in the (unfortunately invisible) HTML "alt text" field for this one image. Thanks for that, although that needs to be added as an actual link. I was going to do that for you, but the other images need source links added too. Thanks. \$\endgroup\$
    – SamGibson
    Jun 30 at 12:49

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge that you have read and understand our privacy policy and code of conduct.

Not the answer you're looking for? Browse other questions tagged or ask your own question.