Mounting Filter on PCB

[J0hn]

Hi,

I had a lump element bandpass filter (BPF). I had connect SMA connectors to the filter directly and measure the performance, everything was perfect. The bandpass frequency i looking at is between 500 MHz to 2 GHz, hence is pretty low frequency.

But when i attempt to mount the BPF onto the FR4 PCB (refer to diagram), the measured return loss was bad. I suspect that the solder pad on the PCB form a shunt Capactance effect, hence affect the performance. I attempted to do a matching circuit (LC circuit) but still fail to improve the return loss.

With the filter mount onto the PCB, i had measured the S2P file and i had put into ADS to design a matching circuit, hopefully that i can reduce the return loss but still fail. Is there any way that i can design the matching circuit or any measure that i can take to improve on the wideband matching, anything that can be done to improve the return loss. Any person had experience on that?

Thanks.

 

[Borber]

Your picture is only simbolic. It does not show how the layout of GND looks like. There should be a lot of vias to the ground plane on the bottom.

 

[J0hn]

Yes. The ground consists of VIAs.. The drawing is not drawn to scale, is just a rough sketch to illustrate/aiding my explaination. Sorry if the drawing is poorly done or misleading.

Would you have any advise to improve on the return loss?

 

[Borber]

Besides the input line and output line must be of correct impedance, the connectors on both sides must have proper grounding.
Is your filter in closed box or it has opened bottom? Check return loss without the PCB once more and with opened and closed bottom.

 

[toonafishy]

You should always remove the ground plane under the input and output pads. Otherwise, the shunt capacitance can be high and can be very difficult to tune out.

 

[biff44]

Most filter launch problems occur when there is a poor connection between the board ground plane and the filter ground plane. 2 GHz is a pretty low frequency, so you should be able to get it to work well. You need to make intimate contact between the two ground planes in as close a proximity to the center connection. In other words, you should have 6 or so ground vias surrounding the center conductor launch point. the via path between ground plane 1 and ground plane 2 should be the thickness of the PCB, nothing longer!

If your path from PCB center conductor to filter center conductor is 0.02 inches, but your path for ground plane return currents is 0.1 inches, that is your problem. Make the ground path return also be 0.02 inches, like in the test fixture.

An ideal way to achieve all this would be to cut a rectangular hole in the PCB, and directly connect the bottom of the filter housing to the back side of the PCB. Anything else will add via length between the two ground planes, and screw up the response. The longer the ground return path, the worse the response gets screwed up.

 

[micro_mory]

I experienced similar phenomenon.

It is added series chip inductor(about 2nH) to connect near pad, the return loss is improved.

I think ...
keeping filter's high Q , matching circuit must be directly connected to filter.

Best regards

mory

 

[J0hn]

By adding the serie inductor to improve the return loss, i had tried this method before, it work fine for narrow band, but it didn't really help much for the wider band.

Added after 12 minutes:

Most filter launch problems occur when there is a poor connection between the board ground plane and the filter ground plane. 2 GHz is a pretty low frequency, so you should be able to get it to work well. You need to make intimate contact between the two ground planes in as close a proximity to the center connection. In other words, you should have 6 or so ground vias surrounding the center conductor launch point. the via path between ground plane 1 and ground plane 2 should be the thickness of the PCB, nothing longer!

If your path from PCB center conductor to filter center conductor is 0.02 inches, but your path for ground plane return currents is 0.1 inches, that is your problem. Make the ground path return also be 0.02 inches, like in the test fixture.

So, by increase the number of ground vias, will that help to reduce the return loss? Thanks.

 

[biff44]

Traditionally, mounting the filter will look like a parasitic series inductance.

The traditional matching method is to shorten the ground return lengths (of which more vias is a solution), AND to add some shunt capacitance at the center conductor launch pad (to try to match out the series inductance with a shunt capacitance, by forming a 2 element LPF whose cuttoff frequency is higher than the mounted filter's passband).