0
\$\begingroup\$

I have followed quite a few RF MCU based designs from Texas Instruments like CC3200, CC2650 etc and in all of them I did not have to worry about the trace impedance between the MCU pins and the antenna.

Their application notes mentioned that as long as the antenna is not far away from the MCU, there is no need to bother with impedance matching.

However now I am designing a RF (2.4GHz) based MCU from NXP, MKW21 to be precise. If you look at the hardware design guidelines, they mention that the trace impedance should be 50 Ω (page 6ff). Here is the pdf link .

Now, my design is space constrained, so the antenna will be kept as close as possible to the MCU. In this case do I still need to monitor the impedance of the track between the tuning circuit and the antenna ?

\$\endgroup\$
2
\$\begingroup\$

Short answer: Yes, you should.

Long answer: For digital signals, it's really true that signals on traces don't behave like waves much if the trace length is sufficiently shorter than the wave length. Now, a) at 2.4 GHz, \$\lambda = \frac cf \approx \frac{3\cdot10^8\frac{\text m}{\text s}}{2.4\cdot 10^9\,\text{Hz}}\approx 12.5\,\text{cm}\$, so the "\$\frac1{10}\lambda\$" rule of thumb might already be broken, and b):

An antenna is nothing but an impedance matching circuit between the impedance of the transmission line and free space. If you don't match your transmission line to both the antenna and the IC, you will have reflections on the interfaces between antenna and trace, and trace and IC, and hence, lose RX power, and hence, lose signal quality (in TX this typically isn't that critical, but still relevant).

Now, a short piece of mismatched will a) be pretty much inevitable and b) will not kill you, but really: you're only doing one RF signal on your board, most probably, so simply do yourself a favor and match that as good as possible. It's really not that hard – there's hundreds of stripline calculators on the internet, KiCAD integrates one, too, and you just have to enter your frequency, your board thickness, and your board's substrate relative permittivity (which you can look up, too – FR4 has 4.7, IIRC), and you'll get a trace width spit out.

For more info on matching lines, see Maxim's tutorial/app note on that topic.

\$\endgroup\$
  • \$\begingroup\$ Group speed isn't 3*10^8 m/s but substantially lower because of the permittivity of the FR4. Rule of thumb: 2 * 10^8 m/s. \$\endgroup\$ – Janka Jan 16 '17 at 10:07
  • \$\begingroup\$ @marcus I was looking into Microstrip line calculators and I noticed a strange thing, the impedance doesn't change with length of the microstrip or the section to input the length is not there at all. What is happening here? \$\endgroup\$ – jar Jan 16 '17 at 16:50
  • \$\begingroup\$ that is exactly what we call impedance matching: If the transmission line has the same impedance as the source or sink of the signal, you don't rotate around in the Smith chart. \$\endgroup\$ – Marcus Müller Jan 16 '17 at 18:00
2
\$\begingroup\$

2.4 GHz has a wavelength of 12.5 cm. If you took a piece of coax at one quarter this length (31.25 mm) and put a short at one end, the input to the coax would look like an open circuit at 2.4 GHz. It's called a quarter wave impedance transformer and can sometimes result in most of the power sent down the coax being totally reflected back to the source: -

enter image description here

\$\dfrac{Z_{in}}{Z_0}=\dfrac{Z_0}{Z_L}\$ (if \$Z_L\$ is a short then \$Z_{in}\$ is an open circuit.)

Actually, due to the speed that electricity travels in wire/cable/PCB being somewhat less than the speed of light, the quarter wave distance in an average 50 ohm transmission line is probably more like 21 mm at 2.4 GHz.

So, if you don't match impedances to the transmission lines (or vice versa) and, you are anywhere near the significant distance of 21 mm you will have problems with standing waves and possibly even cause damage to chips due to power reflection.

How much is "significant"? Most engineers will use a rule of thumb that if the cable is less than one-tenth the equivalent wavelength of the highest (or most useful) signal, then that'll be fine.

So 12.5 cm divided by ten is 12.5 mm and, taking into account the slower speed in coax, this becomes about 8 mm.

For a radio system like this I might be tempted to regard 4 mm as the maximum length of copper trace on a PCB where the impedance isn't controlled.

\$\endgroup\$
  • \$\begingroup\$ I was looking into Microstrip line calculators and I noticed a strange thing, the impedance doesn't change with length of the microstrip or the section to input the length is not there at all. What is happening here? Shouldn't the resistance decrease or decrease as I increase or decrease the length of the microstrip? \$\endgroup\$ – jar Jan 16 '17 at 16:49
  • 1
    \$\begingroup\$ Once your transmission line is correctly terminated in the characteristic impedance, length doesn't change this. It only changes with length when incorrectly terminated. \$\endgroup\$ – Andy aka Jan 16 '17 at 19:49

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.