Resistor footprint in Power Divider

[fred3991]

Hey, everybody,
I am trying to make a Wilkinson power divider 1-to-2. on a PCB using CPWG transmission lines. The frequency is 13 GHz. (Er 3.48, thickness 168 um)

I have built a model on using these components. (and using the multistage wilkinson power divider calculation from Microwave101).
And I am completely satisfied with the results.

However, when creating the layout I don't know how to properly place/take into account the influence of SMD resistor contact pad. For SMD size 0603 - (1.6x0.8 mm ) I need pads about 0.8x0.8.



When I did a simulation without considering these pads in the EM simulation - the results are more or less OK, (Yes, this is 1 stage only, i just tried to figure out what is the problem on smth simple )

But if I put a 0.8x0.8 pad (Or something similar) the results are terrible. (Transmission lines 100 and 200 um)

How to take into account the size of these pads, so that they minimally affect the performance of power divider?
Maybe I should choose a thicker dielectric substrate so that my lambda/4 lines are the same size as this resistor pad?
Maybe a tapper should be used?

 

[volker@muehlhaus]

Maybe I should choose a thicker dielectric substrate so that my lambda/4 lines are the same size as this resistor pad?

Yes, that should help due to (a) less step in width from line to pad and (b) less parasitic C to ground at the pad.

That said, I would compare the exact same testcase, not single stage vs. multi stage.

 

[fred3991]

Yes, that should help due to (a) less step in width from line to pad and (b) less parasitic C to ground at the pad.

That said, I would compare the exact same testcase, not single stage vs. multi stage.

This is without resistor pads (upper) - vs - with resistor pads (lower)

--- Updated Jul 12, 2024 ---

Yes, that should help due to (a) less step in width from line to pad and (b) less parasitic C to ground at the pad.

That said, I would compare the exact same testcase, not single stage vs. multi stage.

Are there any other options besides using a thicker substrate?
I have chosen the thickest substrate available, and still the width of the lines is too small compared to the Resistor pad.

I can't use a smaller resistor package as it would be impossible to solder by hand.

How should I deal with this problem? Maybe additional matching circuits between Lambda/4 <> resistor PAD <> lambda/4 or ?

 

[volker@muehlhaus]

How should I deal with this problem?

The main issue seems to be the extra shunt C from pads to ground. If you can't reduce pad size, you could cut out backside ground locally underneath the pads. This is something to try in Momentum, with the ground layer modelled as a "drawn" layer which must be meshed. This takes more simulation simulation time, but enables cutout in ground.

Another possibility to compensate shunt C is to insert series L on both sides of the shunt C. Maybe a short (!) length of your transmission line near the pads can be implemented with reduced trace width, to add such series L. Not sure if that would work.

My choice would be smaller SMD size, but hand soldering the small sizes requires practice indeed.

 

[FvM]

0603 seems quite large for 18 GHz. Doe you need 0603 power rating or can't you go for smaller package, e.g. 0201?

 

[volker@muehlhaus]

Another question: I am a bit surprised that thickness as small as 168 um is the thickest available substrate. Why is that?

 

[fred3991]

0603 seems quite large for 18 GHz. Doe you need 0603 power rating or can't you go for smaller package, e.g. 0201?

My frequency is 13 GHz,

I'm actually not sure if a 0603 package resistor would be enough as the input power from the PA to the input of the power divider should be Ppeak 36 dBm. but want to try with the 0603 first.

I am looking at the 0603 package also because they are in stock in my lab and also because the 0201 would be incredibly difficult to solder.

--- Updated Jul 12, 2024 ---

Another question: I am a bit surprised that thickness as small as 168 um is the thickest available substrate. Why is that?

this is from PCB manufact.

These boards are recommended here for RF.

However, I could probably just use IN3 instead of IN2 as Ground Plane, thus increasing the dielectric thickness?
Or is this not usually the way to do it?

 

[volker@muehlhaus]

However, I could probably just use IN3 instead of IN2 as Ground Plane, thus increasing the dielectric thickness?

No, I would keep the RF signal in the Rogers part, the FR4 material is too lossy.

But according to your screenshot you have the option of using 254um instead of 168um, so why not use that? Thicker is better to solve your problem.

 

[fred3991]

No, I would keep the RF signal in the Rogers part, the FR4 material is too lossy.

But according to your screenshot you have the option of using 254um instead of 168um, so why not use that? Thicker is better to solve your problem.

In the simplest ideal case to minimize the effect of the pad:
the 70.7 ohm line should be the same width as the resistor pad -
Or
the 50 ohm line should be the same width as the pad.

And then there shouldn't be such a big performance problem. Right? (if we consider the pad as an extension of the transmission line )
Is this the right approach for the design in general?


With a thickness of 254 um I can only get a 50 ohm line with a width of ~500 um, (for SMD resistor I need an 800 um pad).

They have it on their website that there is also a core 508 um option, and then my 50 ohm line should become also 800 micron like pad. I will try to find out from them.

 

[volker@muehlhaus]

Yes, I would test the differnet options using Momentum.

I think it is what I wrote above: the issue is not so much a distributed line issue (discontinuity from step in width), we can look at the pad as a plate capacitor which gives too much shunt C. And one option would be to cut out the griund underneath the pad, as I mentioned above. So you have multiple options now, and can choose which is easiest to implement.

 

[fred3991]

Yes, I would test the differnet options using Momentum.

I think it is what I wrote above: the issue is not so much a distributed line issue (discontinuity from step in width), we can look at the pad as a plate capacitor which gives too much shunt C. And one option would be to cut out the griund underneath the pad, as I mentioned above. So you have multiple options now, and can choose which is easiest to implement.

Ok, got it. Thanks for you support!)

 

[vfone]

Designing printed Wilkinson splitters I found that is better to don't have any ground on the top layer.
If you open any proffesional Wilkinson splitter, you will see they are the same..

https://global.discourse-cdn.com/business5/uploads/flightaware/original/3X/8/f/8ff3872b8e8cc7b19e9239a5505f2ad5561870ed.jpeg

 

[volker@muehlhaus]

I found that is better to don't have any ground on the top layer

You can build such transmission line structures without ground, but it is perfectly fine to add top layer ground if needed to fulfill manufacturing rules, e.g. metal density rules. Of course, extra capacitance from the side grounds must be considered to reach the target line impedance.

 

[biff44]

i am not going to draw the entire thing, but there is no need for coplanar line in the middle where the resistors are. Model that as coupled microstrip lines, and get rid of any ground plane underneath the resistors, like this, and it will work fine