3
\$\begingroup\$

In this design I have separated the ground plane of the sensing/controlling circuit from the high-power 3-4 amp circuit. This is a current controller.

  • The ground planes are joined at the sensing resistors and control signal.
  • The Analog ground is provided by a DC/DC converter common.
  • The Power ground is the ground of the main power supply.

Did I do this correctly?

image of two-layer circuit board layout for review

Alright so I redesigned the board. I was able to keep all but one trace in the bottom plane. The is also a trench separating some of the high current traces from the control circuit. enter image description here

I am using both a top and bottom ground plane pour because this board will be made on copper clad; through hole components mounted on top can only be soldered (well) on the bottom layer. Now, this creates ground islands in the bottom layer. I tried to place the vias close to were the components terminate so the ground return path would not be altered that much.

enter image description here

One concern I have is that one of the traces to a BJT base is longer than I want... High input impendence makes it vulnerable to noise. I don't have enough experience making boards to know if this is bad design or not ( shown bellow) enter image description here

\$\endgroup\$
5
  • 1
    \$\begingroup\$ Much depends on details. In general, I avoid star-point returns as they can cause more problems than they solve in some circumstances. electronics.stackexchange.com/questions/185306/… If you add the schematic, the context will be clearer. \$\endgroup\$
    – Peter Smith
    Commented Sep 5, 2016 at 6:48
  • \$\begingroup\$ Personally, I never split ground planes because it tends to create radiated emissions problems. It can also make noise problems worse if implemented poorly. The important thing to understand is how current flows on the ground plane, and avoid placing or routing sensitive analog signals near where high currents are flowing. Note that "sensitive" means high impedance and/or high gain. If the impedance is low, or there is no gain applied, it may not be a "sensitive" signal. Even a mV shunt signal is not THAT sensitive. \$\endgroup\$
    – user57037
    Commented Sep 5, 2016 at 17:15
  • 1
    \$\begingroup\$ OK, this is what I am confused about: should I 'control' the ground return paths with routing rather just terminating everything directly into the ground plane. Do currents terminated in the ground plane diffuse in the plane or just find shortest distance to the power supply ground connection? \$\endgroup\$
    – Tony
    Commented Sep 5, 2016 at 23:54
  • \$\begingroup\$ Current finds the lowest impedance return path. But where is it returning to? That is what you have to understand. Digital signals routed over a ground plane will have high current density in the ground plane near the trace. The current density falls off as you move away. Switch mode supplies have high current density from input cap to inductor to output cap and also through diode, if any. Motors with any form of PWM control can cause large currents to flow. But I feel that analyzing that current path is fairly straightforward. This question is asked often here. Search for other answers. \$\endgroup\$
    – user57037
    Commented Sep 6, 2016 at 3:28
  • 1
    \$\begingroup\$ In general, you want to control currents by providing them an easy way to go where they want (low impedance). NOT by trying to prevent them from going where they want (which increases impedance). And then avoid routing victim signals in places where rapidly changing voltage and current are present. \$\endgroup\$
    – user57037
    Commented Sep 6, 2016 at 3:30

2 Answers 2

Reset to default
2
\$\begingroup\$

You are asking many questions here. Too many to answer thoroughly. So, I'll try to give you some general guidelines & layout hints.

A. In the two designs you present, the analog and digital ground planes are not separated anywhere near enough to be effective. All the common connecting area is detrimental. You want to have the planes connect at just one place. The position of that "place" on the PCB is important. In general, the connection of the planes should be made thru a wire jumper or zero-Ohm resistor.

B. Typically, the best place to connect the A-Gnd & D-Gnd is where they enter the PCB. In this case that would be near your edge connector. However, wire jumpers being cheap, you should place a number of optional connection jumpers along the dividing gap between the planes. When you get the board completely assembled, you can play with the various jumper positions to see which one is best. (You may find the optimum connection position varies according to the operating mode of your circuitry.)

C. The width of the A-D-Gnd gap matters. The planes will capacitively couple even though they are co-planar. The result is that you end up with a virtual capacitor between the two grounds which provides an inadvertent connection path thru which ground currents can flow. Typically, I make my gaps at least 0.125", but sometimes as much as 0.500 if I have the PCB space to do so and the noise situation warrants. You can test this effect in your prototype PCBs. Before you solder any components to the PCB, connect an LCR Meter between the two ground planes and measure the capacitance. It will likely be in the order of tens or several hundreds of pico-farads. Make a note of this value. When the board is completely assembled and you have tested it enough to become familiar with its inherent noise levels and performance, connect a capacitor of similar value to the measured value between the ground planes. The amount of noise increase you observe in doing so is roughly equal to the amount of noise contributed by the "embedded" inter-plane capacitance created by the proximity of the A & D Gnd planes. This exercise will tell you if you need to make the gap even wider.

\$\endgroup\$
0
\$\begingroup\$

Split ground planes are usually joined at the power source:

http://www.analog.com/library/analogDialogue/archives/46-06/staying_well_grounded.html

This arrangement tends to minimize signal crosstalk from one plane to the other.

\$\endgroup\$

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.