1
\$\begingroup\$

I am in the process of designing a PCB that has 6 layers, here are the details:

  1. Desigining for 50R signal, only one area of PCB is required for 50R.
  2. Freq. range 0.9GHz - 1.6GHz.
  3. 6 layer board with dielectric constant of each layer being the same.
  4. 1oz (35μm) copper on each layer.
  5. RF signal to be routed on top layer, GND layer to be chosen to optimise trace width.

At present going from Layer 1 to Layer 2 (see stackup image below), I get a trace width of approx 0.22mm.

QUESTION(1): If I were to cut a region out of layer 2 so that the GND plane for the RF circuit on the top layer became layer 3, can I assume the dielectric constant to still be 4.1 if both core/prepreg have Er = 4.1? And therefore I just increase the 'h' value in the equation for trace width?

QUESTION(2): Do I need to factor in anything relating to the missing copper on the inner layers or can I consider that the board will be made such that there is no air gap?

QUESTION(3): If the Er was different in between layers, how would that be dealt with?

enter image description here

\$\endgroup\$
2
  • \$\begingroup\$ What is your objection to .22mm trace width ? Sounds very practical unless you would want to transmit considerable power.. \$\endgroup\$
    – tobalt
    Nov 28, 2021 at 7:21
  • \$\begingroup\$ No specific objection, it's more that the tracking felt cleaner with the wider traces. \$\endgroup\$
    – deBoogle
    Dec 15, 2021 at 7:56

1 Answer 1

1
\$\begingroup\$

You are asking questions that only the PCB house can answer, that is, the dielectric constants of the materials. It is best that you contact the PCB manufacturer for their recommendation on layer thicknesses and widths for impedance controlled traces for your stackup. This will differ from the simple PCB trace width calculators in PCB drafting programs as they take in to consideration what end result of their process is.

Assuming the dielectric constant is the same for prepreg and core, you can add the layer thicknesses together. You may want to download the Saturn PCB Design Toolkit to examine your trace impedance options.

You also have options on the core/prepreg thicknesses. You have the center core (should be prepreg) thickness as 0.9mm. You might have a good reason for this, but, you could make that 0.9mm layer thinner and add thickness to your outer core (should be prepreg) layers so you can widen up your 50 ohm trace. Again, talking to your PCB manufacturer is a good idea.

As for air between the layers, there will be no air as the layers are pressed together in a vacuum. The presses apply a starting pressure around 70 psi, then increase the press pressure in the range of 300 to 500 psi during the cure process.

As for different dielectric constants between core & prepreg, impedance calculators can take this in to consideration. Typically, PCB manufacturers use Polar Instruments software to determine trace widths for impedance controlled traces. Polar's software uses a field solver. Polar's software is expensive which is why you talk to your PCB manufacturer.

As for your stackup, you'll find that PCB houses want the prepreg on the outside, thus, your board stackup should be:
top copper
prepreg
layer 2 copper
core
layer 3 copper
prepreg
layer 4 copper
core
layer 5 copper
prepreg
bottom copper

\$\endgroup\$
1
  • \$\begingroup\$ Thanks. I actually have Saturn already, I find it very useful. The stack up I showed in my question was from the board house (although labelled wrong admittedly). Your answer helped a lot thanks again. \$\endgroup\$
    – deBoogle
    Dec 15, 2021 at 7:58

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

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