Very thin RF trace - Is it a problem to handle the Bluetooth power

[simbaliya]

The context is as follow:

My PCB thickness is very thin, and my PCB supplier gives me calculation of a microstrip impedance line for 50ohm, which resilts in a trace width of 75um, trace length about 20mm.

The trace is connecting output of RFIC PA to BAW filter, the application will use Bluetooth Low Energy.

My question is, assume the supplier calculation is correct that I get 50ohm for this line, RFIC PA output and BAW input are design with 50ohm, will this very thin 75um trace be a problem to handle the power transmitted by Bluetooth @ Low Energy for worst case scenario?

 

[vfone]

The 75um trace it will work fine at +10dBm RF power, but I think this width is very unusual for a normal PCB trace.
The parasitic inductance of the 20mm trace will be pretty high (about 20nH), and you have to compensate somehow using a matching capacitors. Have to put all the inputs in a CAD simulator and see what you get.

 

[FvM]

If it's actually 50 ohm impedance (80 µm FR4 substrate?), it has no parasitic inductance. Just higher resistive losses according to the small width, but no problem with 20 mm length.

 

[simbaliya]

The 75um trace it will work fine at +10dBm RF power, but I think this width is very unusual for a normal PCB trace.
The parasitic inductance of the 20mm trace will be pretty high (about 20nH), and you have to compensate somehow using a matching capacitors. Have to put all the inputs in a CAD simulator and see what you get.

Thank you for the reply, mayI know how do you estimate the 75um trace being able to handle 10dBm?

And if the trace is not 50ohm, but 30ohm or 70ohm, but length become shorter than 6mm, what will happen then?

- - - Updated - - -

If it's actually 50 ohm impedance (80 µm FR4 substrate?), it has no parasitic inductance. Just higher resistive losses according to the small width, but no problem with 20 mm length.

The PCB is flexi, total thickness is around 0.2mm, 4 layer, so the substrate is even less than 80um.

If the trace is actually not 50ohm but 30ohm or 70ohm(my supplier is really new to RF PCB, I am not very confident about this impedance calculation), will the resistive loss in the trace become an not acceptable issue?

 

[FvM]

O.K., flex print isn't FR4 but Kapton (Polyimide) and has lower Er. Standard flex substrates are 2 and 3 mil, coverlay must be considered for the impedance calculation as well.

The impedance can be calculated e.g. with Saturn PCB toolkit if you know the actual stackup.

 

[vfone]

In fact this is the problem. For a 75um microstrip line put on a very thin substrate, will be very hard to keep the 50 ohms impedance. I understand this is a normal PCB design, and not an LTCC or IC project.
The microstrip line with a length that is 285 times longer than its width, for sure will have some parasitic inductance that needs to be compensated. An EM simulator could say everything about this issue.

 

[volker@muehlhaus]

In fact this is the problem. For a 75um microstrip line put on a very thin substrate, will be very hard to keep the 50 ohms impedance. I understand this is a normal PCB design, and not an LTCC or IC project.

I disagree. If the substrate is thin, but with reasonable tolerances, there is no problem at all. It might be unusual to people working on thick PCB substrates, but narrow lines are quite common on thin substrates. No problem.

The microstrip line with a length that is 285 times longer than its width, for sure will have some parasitic inductance that needs to be compensated.

That's wrong. The only thing that matters is line impedance. If matched to 50 Ohm, the length is not relevant.

 

[vfone]

Yeah, this I was thinking about. Tolerance. In a standard PCB development (no LTCC, no RFIC design), with this very thin substrate and high length/width ratio, to keep a decent tolerance will be almost impossible. And when I mentioned "compensated" I refer to impedance matching. Read my first post about "matching capacitors".
Doesn't matter too much if the affected line needs impedance matching, because when is done, everything will work just fine.

 

[KlausST]

Hi,

Read my first post about "matching capacitors".

A properly terminated (with a resistor) signal line does not need a capacitor. There is nothing to compensate.


Klaus

 

[vfone]

"Properly terminated resistor" meets very rarely the condition "required terminated resistor". But caps helps to bring the naughty line where you want..

 

[KlausST]

Hi,

I don't get your idea.
A properly designed and terminated (without capacitor, without inductance, just a resistor) has neither capacitive nor inductive character.

Please give an example where a "capacitor can bring any benefit" then.

********
Let's imagine you have a piece of cable....and you find out it needs to be terminated/compensated with an xxx value capacitor.
What will happen when the cable is twice as long as before?
You need twice, or half or the same capacitance value?

For a properly designed cable ... the length does not care.
Imagine: maybe there is a signal on the line....with wavelength of 1m .... it can't know whether the cable is 10m or 50m long.

Only when the wavelength is longer than the cable .... it makes a difference...
But in this case the demand for an impedance controlled cable is about useless.

Klaus

 

[FvM]

Flex PCB are often used for high speed interconnect, e.g. SATA and USB 3.0 with up to 6 Gbps. Transmission lines are mostly 90 to 100 ohm differential pairs, manufacturing of fairly tight tolerated impedances (+/- 10 %) doesn't seem to be a problem. It translates to about +/- 10 to 15 µm trace width tolerance, which is obviously manageable in flex PCB production.

Requirements for 50 ohm single ended transmission line are quite similar to 100 ohm differential.

 

[vfone]

The original post is about RF Bluetooth signal which works on 2.4Ghz (not SATA, or USB 3, or any high-speed digital), and is about single ended transmission line (not differential).

If happen that this single-ended microstrip line doesn't have the desired impedance of 50 ohms (most likely at given data), the easiest way to bring the circuit to 50 ohms is to use matching capacitors at the ends of the line.
Depending by other factors in the circuit, sometime only one cap at one end of the line will do this job.
If this long microstrip line goes to the antenna (looks like) things are even simpler, because the line and the matching capacitors could be integrated into antenna matching network.

 

[KlausST]

Hi,

that this single-ended microstrip line doesn't have the desired impedance of 50 ohms

I agree.

matching capacitors could be integrated into antenna matching network.

I agree, too. But antenna is something different...


Klaus

 

[FvM]

If happen that this single-ended microstrip line doesn't have the desired impedance of 50 ohms (most likely at given data), the easiest way to bring the circuit to 50 ohms is to use matching capacitors at the ends of the line.

Yes, compensation elements may be used.

There's however no reason why the designed impedance would be "most likely" missed. Particularly it's not systematically too inductive, as suggested in previous posts.

 

[cariban]

75um is pretty fine to conduct 10dBm power, no any problem. Even all the power is dissipated in the track, you may not see any temperature change. The power is just 10mW.

The down side is that for thin tracks, it is very hard to get controlled 50 Ohm impedance. There are always some variations caused by PCB manufacturer, such as width, etching slope, resin distribution of prepeg, thickness of prepeg, etc. If your board is 0.2mm, it may be better idea to use microstrip line, with reference to the bottom layer. Then the track should be much wider (about 0.35mm if Dr = 4.6) and easier to get precisely controlled impedance.

Another suggestion. BAW filter is usually very narrow band filter. The BAW filter performance is very sensitive to the source/load impedance. It is highly suggested to put a PI impedance matching network at both input and output port of BAW filter. Then you have the option to tune the source/load impedance to 50 Ohm if needed.

- - - Updated - - -

Yes, compensation elements may be used.

There's however no reason why the designed impedance would be "most likely" missed. Particularly it's not systematically too inductive, as suggested in previous posts.

vfone may actually mean the production tolerance. It is more difficult to control the impedance for thin wires.