4
\$\begingroup\$

For my final project I have to measure multiple signals up to 10MHz with a TMS320F2809 processor which is clocked at 100MHz.

I have the following layer stackup:

  • Top Signal
  • Ground
  • Signal
  • Signal
  • Source
  • Bottom Signal

On the signal layers do I have to put a polygon plane? Is it a good idea to connect to the ground? Will it act as a capacitor between the trace and the ground polygon?

According the following description on the top and bottom layer should be routed only low frequency. Which range is low frequency)(1Hz up to ?)? I tried to follow that description, but when two IC was within 1cm range I routed on the layer where the ICs are.

\$\endgroup\$
3
  • \$\begingroup\$ Regarding "low frequencey": AFAIK, up to 20 MHz may behave as "low frequency" if there are no particular signal problems. Lots of Arduino clones only use 2-layer PCBs, running at 16 MHz with no problem. \$\endgroup\$
    – Jon Watte
    Aug 24, 2013 at 23:08
  • \$\begingroup\$ I'm curious to know this myself, for what it's worth, I always do ground polygon fills on signal layers because it's better for the environment (less waste material production since less copper needs to be etched away). But it does not seem like this is industry standard (looking at the Raspberry Pi, for example). \$\endgroup\$
    – Zuofu
    Aug 25, 2013 at 17:39
  • \$\begingroup\$ @JonWatte The arduino's don't really run at 16 MHz, in that most of the signals are much, much slower. Only two traces carry signals at that frequency and those are usually well controlled. If you were running a 16 MHz 8-bit wide databus, though, two layers may not be enough. \$\endgroup\$
    – Chintalagiri Shashank
    Sep 10, 2014 at 11:17

3 Answers 3

Reset to default
3
\$\begingroup\$

It is not necessary to put polygon pours on your signal layers. However, there are a few advantages to adding ground pours.

  1. Ground pours on layers adjacent to the power plane will help with power plane decoupling for high frequency signals >500MHz. Henry Ott does a good job of explaining this. http://www.hottconsultants.com/techtips/decoupling.html

  2. Ground pours can be used as part of an impedance controlled transmission line called a Coplanar Waveguide.

  3. Adding polygon pours can help balance the copper distribution on multilayer boards and will prevent bowing and twisting of the PCB during manufacturing. here is a link to some good information about this http://www.multi-circuit-boards.eu/en/pcb-design-aid/copper-balance.html

  4. Polygon pours on outer layers can be used for thermal dissipation.

\$\endgroup\$
1
\$\begingroup\$

Adding a ground pour on the top and bottom can help to reduce EMI. They're also required for some impedance controlled traces. If you do add ground pours, make sure that they are via stitched to the main ground plane (in your case, layer 2). Do not have any islands of copper that aren't attached to anything. Most of the advanced EDA tools like Altium allow you to control this with design rules.

\$\endgroup\$
1
\$\begingroup\$

Adding ground pours in the signal layers will help to maintaing copper balance, which is important in multilayer boards. These ground pours should be stitched to ground power planes with multiple vias.

\$\endgroup\$

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.