[SOLVED] Microstrip filter implementation and simulation differences

[gzdeozc]

Hi everyone,

I have designed an interdigital microstrip bandpass filter on ADS working at X band frequency. Everything looks great on Momentum simulation. Then, I tried to implement it on pcb (RO3210), but its S21 response is really different from the results I have seen on momentum simulation. I expected some difference of course but I didn't expect such thing. What can be the reasons? What should I have taken care of? One reason I can think of is, I used vias very close to each other, can that cause a problem? Is there a rule for that?
And the other thing is some of my lines are too close like 5 mils away from each other. Is this practical? Can that cause problems?

Thank you in advance
Very glad if you post answers asap

 

[vfone]

If the vias you mentioned were placed also in the EM simulator (and using the right via model), there should be no major difference between simulated and measured results.

5 mils spacing could be the reason, because even for a 10 GHz design it is below the usual spacing limit.
I cannot recommend how much to increase the spacing if I don't have more information about design, but just try to make it larger.

Be sure that all the PCB parameters as Er, height, loss, etc., that you set in the simulator, match the real PCB parameters you are using.

 

[D.A.(Tony)Stewart]

Your interface connector and cable quality must be verified/ calibrated. What did you use?

 

[gzdeozc]

I use sucoform 86 as cable and sma connector to connect network analyzer. But input and output of the filter there are pads for measuring, i solder cables on them. I dont know if this causes problem and maybe calibration is not accurate. There are ripples on s21 response and wider than i saw on momentum simulation. What do you think?

 

[volker@muehlhaus]

Then, I tried to implement it on pcb (RO3210), but its S21 response is really different from the results I have seen on momentum simulation. I expected some difference of course but I didn't expect such thing. What can be the reasons?

From long experience in EM simulator support: the biggest error source in EM simulation is the user. We don't know what you have modelled in Momentum, so there could be some mistakes there.

In any case, if you have 5mils gaps, manufacturing precision can be a problem. You should measure the actual gap width and line width (=> microscope) and re-simulate with those dimensions.

 

[rfmw]

I would recommend to increase the minimal gap to roughly 0.2mm (~8 mils). That's a confident gap you can manufacture or etch yourself. Should be okay for x-band filter too. You mention about some pads that you solder the sucoform cables to. Those pads, if done incorrectly, are a sufficient reason that your performance is degraded (by a lot). Take a photo and show us your filter.

 

[gzdeozc]

https://obrazki.elektroda.pl/8005803600_1407931510.jpg

The filter is this. Are there anything incorrect on it?
Thank you very much

 

[D.A.(Tony)Stewart]

Try a Monte Carlo analysis on EM Sim , if possible.

 

[volker@muehlhaus]

Try a Monte Carlo analysis on EM Sim , if possible.

Why, and based on what? For Monte Carlo analysis, we need a good estimate of the dimension tolerances, and the related statistics.

Here, we have no measured dimensions and no statistics. The first step would be to measure the actual dimensions, and simulate with these values. No need for Monte Carlo analysis yet.

~~

Looking at the layout, I wonder how the feed was done in measurement, and how it was simulated.

 

[FvM]

I see a certain weakness in the "lonesome" ground vias connecting the ports. The ground pads are no low impedance ground, we can expect some crosstalk between the ports and an effect on S11/S22.

You can drill holes and connect the ports through the ground plane, e.g. using thin semi rigid cable.

 

[volker@muehlhaus]

I see a certain weakness in the "lonesome" ground vias connecting the ports. The ground pads are no low impedance ground, we can expect some crosstalk between the ports and an effect on S11/S22.

Absolutely! The ground connection of the ground pad isn't acceptable.

And above, gzdeozc mentioned that the cables are "soldered". Soldered from the top? If we look at the small dimensions of the filter, and then look at the large pads, and the large distance between the "signal" and "ground" pads, it is difficult to imagine how this could work. So much undefined wire length, not really small compared to the wavelength. All this undefined wire is part of the signal path ... not good.

The idea to use small semi rigid cable from the back side is great, this should give a much better transition from the coax to the PCB. Also, we don't need the bad ground pad with the lonely via then.

 

[rfmw]

I agree, you should have like 10+ vias on the ground pad and not just a single one. How did you solder the coax cables? Can you show that photo too?

 

[gzdeozc]

Thank you for all you for comments.
The whole pcb is like this, https://obrazki.elektroda.pl/7856431500_1407956039.jpg
Still lack of vias?

The idea to use small semi rigid cable from the back side is great, this should give a much better transition from the coax to the PCB. Also, we don't need the bad ground pad with the lonely via then.

Can you describe it more? Do you mean soldering the coax gnd to the lower pcb and the inner conductor to the signal pad by drilling a via?

I will put a photo with coaxes. It is like the gnd of coax is soldered on gnd pads, and inner conductor is soldered to the input and output pads of the filter. It is actually huge considering the filter size.

- - - Updated - - -

Can you also offer me some documents/books about these practical issues?

 

[albbg]

I have had similar problems working in Ku band with a directional coupler.

I didn't use coaxial cable to connect the ports but connectors with the body screwed on the alluminium enclosure of the board (dimension rouglhy 5x5 cm). I found effects on S11 and S22 due to the connector that in the first attempt wasn't a microstrip type. However the main effect was due to a poor ground. Even if the bottom layer was a full copper plane the impedance of the ground was too high. The problem has been solved using a 1mm thickness carrier, made by copper, glued by means of an electrically conductive epoxy at both the bottom of the board and the enclosure.

This to say that the ground plays a fundamental role and just one via hole on the ground pad seems to me not enough.

 

[FvM]

Still lack of vias?

Yes, too far away from the port ground pads. The via distances are in a range where you can even get pretty resonances. One would expect a via fence around the square opening and particularly at the port ground pads.

A standard connection for the ports would be an edge mounted SMA connector with a short 50 ohm microstrip. Or a through connected SMA from the bottom side.

Can you describe it more? Do you mean soldering the coax gnd to the lower pcb and the inner conductor to the signal pad by drilling a via?

Yes. I was particularly thinking of small semi rigid cable, e.g. RG405U. Drill a hole for the 0.5 mm center conductor, enlarged to 1 mm on the bottom side. Outer conductor soldered perpendicular to the bottom plane.

 

[volker@muehlhaus]

The whole pcb is like this, https://obrazki.elektroda.pl/7856431500_1407956039.jpg
Still lack of vias?

The main problem is that the via spacing is much too large. Look at the resonator length, and compare it to the via spacing: the via spacing is around lambda/4, and even much larger near your ground pads. That doesn't work. If you want to ground that metal area, you need via spacing around the filter that is lambda/10 or less. In the outside area, far away from the filter, this is less critical, but I would also decrease the via spacing there.

I will put a photo with coaxes. It is like the gnd of coax is soldered on gnd pads, and inner conductor is soldered to the input and output pads of the filter. It is actually huge considering the filter size.

That's a problem then.

 

[shashy.br]

Hi,

I had implemented Microstrip Filters (HAIR PIN) for X band Application also and saw a shift of 400 MHZ , i.e i designed for 9.4 GHz with 600Mhz BW but ended up with a filter of CF 9 GHZ and 800MHz BW ....so i decided to fabricate a bunch of filters with varying CF and BW ...i analyzed all the filters found the simulation Filter that matched my filter requirements when fabricated.

I suggest you fabricate filters as i did and measure the differences and use the suitable filter design that matches your requirements. (the shifts occur due to etching tolerances as per my judgement)

1) i used RO 6006 ( i think it was 20 mil subs)
2) use lower copper thickness since it will reduce the etching tolerances
3) i got a insertion loss of 3.5 dB wort case for the filter

 

[rfmw]

How come you made the vias correct on the microstrip resonators, that is, they are so close that are touching each other, while on the ground the vias are too widely spread. You should use the same approach for the ground pads, where you solder the shield of the coax cable. Like I said, 10+ vias on the ground pads should be the bare miminum...

Thank you for all you for comments.
The whole pcb is like this, https://obrazki.elektroda.pl/7856431500_1407956039.jpg
Still lack of vias?


Can you describe it more? Do you mean soldering the coax gnd to the lower pcb and the inner conductor to the signal pad by drilling a via?

I will put a photo with coaxes. It is like the gnd of coax is soldered on gnd pads, and inner conductor is soldered to the input and output pads of the filter. It is actually huge considering the filter size.

- - - Updated - - -

Can you also offer me some documents/books about these practical issues?

 

[gzdeozc]

Thank you for your guidance, when I fix the grounding problem, it worked.