1
\$\begingroup\$

I have a PCB board with the stackup shown below. I want to calculate what would be the impedance (and capacitance too?) of a 5" PCB trace on the L1 layer.

How to calculate it?

enter image description here

For example, I am trying to use this calculator (https://www.eeweb.com/toolbox/microstrip-impedance/), what should be the value of the fields?

\$\endgroup\$
  • \$\begingroup\$ The link you posted has a diagram showing what "T", "H", and "W" are. "Er" is a clunky way of writing \$\varepsilon_r\$, which is another name for "Dk", which is given on your stackup chart. \$\endgroup\$ – The Photon Oct 4 '16 at 4:54
  • \$\begingroup\$ I know "W" = Width?, "H"=Height? (is that 2.1mil for L1?) and what is "T"? I guess where is the place to put the LENGTH of the trace? \$\endgroup\$ – user1406716 Oct 4 '16 at 4:55
  • \$\begingroup\$ "T" is the thickness of the metal. In the "Thickness" column of your table. The characteristic impedance does not depend on the length of the trace. \$\endgroup\$ – The Photon Oct 4 '16 at 5:03
  • \$\begingroup\$ So a 2" trace or a 4" trace would have the same impedance? and What should i use as the Capacitance? \$\endgroup\$ – user1406716 Oct 4 '16 at 5:04
  • \$\begingroup\$ The same characteristic impedance. That is not the same as having the same impedance. You should probably research transmission line theory to understand what you're getting in to. \$\endgroup\$ – The Photon Oct 4 '16 at 5:05
2
\$\begingroup\$

trying to figure out how I can replace a 4" trace with an equivalent RLC Circuit.

First choice: Don't. Use the 'tline' element in LTSpice instead.

Second choice: You can model a transmission line with a sequence of pi or T sections. If you use a different transmission line calculator, for example the Saturn PCB one, or this online one, they will output capacitance and inductance per unit length in addition to the characteristic impedance.

Say your calculator says the capacitance is 1.7 pF per inch and the inductance is 12.2 nH per inch. Then you can break up your 4" trace into as many sections as you want. Each section of length L (for example L=0.4" if you break your 4" trace into 10 sections) will have 1.7 \$\times\$ L pF and 12.2 \$\times\$ L nH, arranged in either a pi or T circuit.

Keep solving your circuit with this set-up, increasing the number of sections each time, until your results stop changing (this step is why it's easier to just use a built-in model than to try to make an LC model yourself). The higher the frequencies present in your circuit are, the more sections you'll need to achieve an accurate model.

\$\endgroup\$
  • \$\begingroup\$ It might be better to suggest the ltline, even if it tends to be sluggish given certain conditions. The tline is a rather simple approach, and it overshoots easily, even in ideal conditions: try, for example, a current source with pwl 0 1 0 1m, two or more tlines with Td=1 Z0=1 and a terminating 1 Ohm resistor. Plot all the intermediary voltages and you'll see what I mean. Alternatively, it might be even better to model your own RLC, even at the cost of extra elements/nodes, because then you can also model coupled inductors. Of course, there will be a penalty... \$\endgroup\$ – a concerned citizen Oct 4 '16 at 7:31

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.