Impedance of transmission line

Thread Starter

phoenixyx

Joined Feb 8, 2017
12
Hi,

I am trying to make a 50ohm transmission line. I have made it using the coplanar wave guide with ground plane.

I have come to the conclusion that the track has to be quite wide to get the correct impedance.
This again become a problem when I arrive at the components which are 0603(0201 im) size, and the track is way to wide for the components.

What happens if I drop down to 0.5mm the last 0.5 mm of the track, will the impedance change for the whole transmission line. If so, will the track width be limited to the width of the tuning component footprint?

Also, the via will introduce some capacitance to the track, what is the best way to place the via, close to the antenna element, or close to the input on the Microcontroller?

Thanks in advance

upload_2018-10-3_8-17-12.png
upload_2018-10-3_8-21-17.png
 

cariban

Joined Aug 14, 2018
69
What is the operating frequency? Your track is wide because the height to the reference plane is too large. Do you have to use 0.8 mm height?
Another option is to use bigger capacitor size, for example EIA-0603. Anyway it does matter or not depending on your operating frequency.

The same is for your question about via.
 

Thread Starter

phoenixyx

Joined Feb 8, 2017
12
Hi, Thank you for your answer, sorry for my late response.

My operating frequencies are 2.4Ghz and 1.542 Ghz.

I changed the track width and clearance and came up with this:
upload_2018-10-16_14-30-23.png

I have ordered the PCBs, and are measuring these with a VNA at the moment.

I find that the Impedance is much lower than calculated. I have tried to find the reason why.
What I find is:
Calculated impedance should be 49.9 ohm
Measured impedance is found to be around 34-36 ohm
upload_2018-10-16_14-34-7.png
Blue is 2.4Ghz line, pink is 1.542 Ghz

Measurements have been done like this:
- calibrate VNA with open, shunt and 50ohm (2x100ohm resistors)
- solder coax onto PCB, solder 50 ohm at other side of transline.(2x100ohm again)

Measurements seem to be ok as I measure another transmission line the same way, and this come out with close to correct values.

Any ideas on what can make the impedance come out so low?
 

cariban

Joined Aug 14, 2018
69
Hi, Thank you for your answer, sorry for my late response.

My operating frequencies are 2.4Ghz and 1.542 Ghz.

I changed the track width and clearance and came up with this:
View attachment 161669

I have ordered the PCBs, and are measuring these with a VNA at the moment.

I find that the Impedance is much lower than calculated. I have tried to find the reason why.
What I find is:
Calculated impedance should be 49.9 ohm
Measured impedance is found to be around 34-36 ohm
View attachment 161671
Blue is 2.4Ghz line, pink is 1.542 Ghz

Measurements have been done like this:
- calibrate VNA with open, shunt and 50ohm (2x100ohm resistors)
- solder coax onto PCB, solder 50 ohm at other side of transline.(2x100ohm again)

Measurements seem to be ok as I measure another transmission line the same way, and this come out with close to correct values.

Any ideas on what can make the impedance come out so low?
I would definitely suggest you to use normal microstrip line than coplanar transmission line. Your gap to GND plane in the top layer s = 0.11mm. This a very small number and the tolerance is very difficutly to be controlled. Also you need field solver to get good result for coplanar lines. Empirical formula is not accurate enough for coplanar lines.
 

cariban

Joined Aug 14, 2018
69
I see, then its back to the wide lines of the microstrip.

Thanks again
How long is the track? If it is rather short, for example less than 10mm, there should be no problem to use wide track. There may be some discontinuity, but it is not a big deal at 2.4GHz.

Of course the best solution is to change the PCB stack-up to avoid too large height to the reference plane. It is may be too late for your case. If you really want to stick on coplanar waveguide, try two things:
1. Use field solver to calculate the impedance;
2. Use as large gap as possible. Find out the maximum track width you feel comfortable, then adjust the gap to have 50 Ohm impedance.
 

Thread Starter

phoenixyx

Joined Feb 8, 2017
12
Great tips: -)

I think I will try out the microstrip and see how that works out, might change to 4 layer to get the internal GND plane closer, and what I can do with that.
 

cariban

Joined Aug 14, 2018
69
Great tips: -)

I think I will try out the microstrip and see how that works out, might change to 4 layer to get the internal GND plane closer, and what I can do with that.
I am glad to hear the progress. Just comment another thing. If it is not too late, add a PI impedance matching network somewhere to compensate the non-ideal factors later if necessary. In reality no matter how good you design the layout, there are always some non-ideal factors, for example via stub, non-ideal components, etc. I guess your signal is narrow band, a Pi network is sufficient.
 
Top