I'm designing a PCB with a microcontroller ,CAN transceiver, sensor (I2C) and linear regulator. I want to make the PCB as small as possible, so my thoughts were to use both sides of a two layer stack up. I've never done this before, only ever using one side of the board for components.

  1. My primary concern is what should I avoid putting back to back? for example I'd make an educated guess that it would be poor choice to put the linear regulator directly behind the microcontroller.
  2. Should I avoid comm lines (I2C UART CAN) crossing over?
  • 5
    \$\begingroup\$ Ask your assembly house what the weight and size limitations are for bottom loaded board. \$\endgroup\$
    – Jeroen3
    Jan 25, 2018 at 10:16

2 Answers 2


First off, use a 4 layer board. Not only does it make layout easier but inner ground and power planes provides a barrier against front/back crosstalk. Also, 4 layer is not much more expensive than 2 layer

Second, lines crossing is nowhere near as bad as lines running parallel

  • \$\begingroup\$ So something like Top layer, Power Layer, Ground, Bottom Layer? Are there are no issues with power passing through the ground plane in a via? or should I have a small keep out zone for the copper fill where I'm passing power through ground or vice versa? \$\endgroup\$
    – Pop24
    Jan 25, 2018 at 9:32
  • 1
    \$\begingroup\$ @Pop24 Just regular vias connecting power and ground as close to the chips as possible. Don't forget decoupling capacitors. Also sprinkle decoupling caps around the board connecting power and ground to them. \$\endgroup\$ Jan 25, 2018 at 9:46
  • 1
    \$\begingroup\$ @Pop24 see my answer update to this \$\endgroup\$
    – Trevor_G
    Jan 25, 2018 at 10:49

Adding to Dirk's Answer

Be aware, mounting on both sides of a board may not buy you as much real estate as you might be imagining.

When it comes to board density, your ability to route traces tends to be a critical factor as density goes up. More layers helps, but then you fill up space with vias.

Double sided tends to make it MUCH harder to route unless you use buried or blind vias and use many MORE layers. The cost tends to go up a notch or two and reliability goes down.

A common trick though is to save room by putting small things like decoupling caps/pull-ups etc on the back. Since the power lines normally have vias close to the chip anyway, flipping them to the back is not so bad. If you have to add vias to do that it is pretty much a wash.

Also you need to be very aware of thermal issues, you do not want a device at 100C or even 50C on the back of a chip with lots of pins or a temperature sensitive analog circuit.

The other thing you need to be careful of with backside components is the silk-screen. If you use one on the back make sure it does not interfere with any vias, solder points, or test pads.

  • 1
    \$\begingroup\$ I agree. But: "like decoupling caps" - beware the parasitic inductance of the via. This may degrade your decoupling, rendering it useless in some cases. \$\endgroup\$
    – Manu3l0us
    Jan 25, 2018 at 12:27
  • 1
    \$\begingroup\$ @Manu3l0us yup, it is much more problematic for higher frequency or fast switching parts. \$\endgroup\$
    – Trevor_G
    Jan 25, 2018 at 12:30
  • \$\begingroup\$ Isn’t it also more expensive to manufacture with components on both sides? \$\endgroup\$
    – Michael
    Jan 25, 2018 at 16:45
  • \$\begingroup\$ @Michael yes but how much depends on the fab house and the nature of the parts. SOmetimes the difference is not much. \$\endgroup\$
    – Trevor_G
    Jan 25, 2018 at 16:48

Your Answer

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

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