Electronic – how to reproduce a matching network of a vendor

impedance-matchingRF

I'm trying to create a board using the BGT24MTR chip from infinion. I noticed that they said that there is a Tx/Txx impedance.

enter image description here

To compensate for this impedance they created a matching network.
enter image description here

Since I'm trying to use a different board stack up, I have to redesign this matching system. I tried calculating the impedance of each of the lengths
enter image description here

Here's my breakdown of the major components.

Width Length  Ω     diff Ω   diff Ω single
.3    .55     68.5     82     61
1.15  1.6     31.19    22.2   16.5
.5    ∞       53

I thought that I was trying to use the smith chart to get the impedance to be purely real around 5/3 after the second rotation so that when it is renormalized it would be purely in the unit circle in the center, but every way I looked at using the smith chart led to results that are far away from being matched.
enter image description here
Any suggestions on what they are doing to match this?

P.S. The new board stack up is FR408 1.6mm thick. 1oz copper on both sides (1.4mil,35um). Frequency is 24 GHz

Best Answer

Your use of the smith chart is correct, but your numbers are a little off due to the wavelength you used (6.5mm).

In stripline, the fields are completely contained inside the substrate. The fields are partially in air around a microstrip line, resulting in an effective permittivity which is lower than the relative permittivity of the substrate. Wavelength can be calculated using the effective permittivity or the delay (Tpd). Both are available from your impedance calculator. Er effective is 3.0635. Tpd is 5.8e-9 s/m.

\$ Wavelength = \frac{c}{\sqrt{E_{r}} \cdot f} = \frac{1}{T_{pd} \cdot f} \$
\$ Wavelength(w/ E_{r}) = \frac{c}{\sqrt{E_{r}} \cdot f} = 6.5 mm \$
\$ Wavelength(w/ E_{eff}) = \frac{c}{\sqrt{E_{eff}} \cdot f} = 7.1 mm \$
\$ Wavelength(w/ T_{pd}) = \frac{1}{T_{pd} \cdot f} = 7.1 mm \$

The difference between 6.5mm and 7.1mm may seem small, but check out the difference in return loss.

\$ Z_{out}(\Lambda:6.5mm) = 33-j24 \Omega \$ >>>> \$ ORL=9dB \$
\$ Z_{out}(\Lambda:7.1mm) = 46-j14 \Omega \$ >>>> \$ ORL=16dB \$

For a sanity check, match from the load to the conjugate of the generator. In other words, start at a load of \$50\Omega\$ and go towards the chip. You'll end up around \$20.8+j20.2\Omega\$. This is typical for most output stages, since they're usually low resistance and capacitive.

Your method of matching will provide a decent ballpark, but I'd like to point out a few important sources of error.

  1. Tx & Txx are intended to be 100ohm differential signals. The small spacing between them produces an additional shunt capacitance. You need to include the extra capacitance, or use a coupled line model.
  2. The datasheet doesn't say how they measured the Tx/Txx load impedances. Did they measure at the PCB output port and try to de-embed everything up to the chip? I'm skeptical of the accuracy without knowing where they came from. Additionally, I think these are the impedances looking into the Tx/Txx ports. I would call the load impedance the conjugate of the printed values, or the impedance presented to the Tx/Txx ports. It's all unclear.
  3. The package pad (footprint) will have a different impact on a different board stackup.
  4. I don't see anything to cancel mismatch from the launchers. The launchers will perform differently on a different board stackup.

The matching network they used is simple and probably low loss. I guess you could call it a stepped-impedance match. I don't know. It's a plus to avoid shunt components or stubs, and the high Q resonances they might produce.

Related Topic