My BPF filter wont work when I try to implement it

[koffp]

No matter what I do I can't get my 2 BPFs to work in real life.. One is a 5th order cheb from 500-570 mhz and the other is a 3rd order cheb from 500-540 mhz. I'm a new engineer and this is my first time actually implementing a filter i designed..

I calculated them correctly and the simulations matched up but when I hook it up to the spectrum analyzer and the VNA it shows the pass band being way off centered at about 350 mhz instead of 535 mhz for the 5th order and all the way down at 70 mhz for the 3rd order. The engineer who was here before me had a lot of year experience and his filters were also getting their center frequency skewed off from the 500s to the 300s(mhz) so it seems like there is some essential PCB layout design I am missing...

I'm at my wits end, I don't know what to do and i'm getting embarrassed in front of my coworkers by how long this is taking me to figure out. I know that my pcb trance geometry isnt perfect( not final revision) and that the parts have tolerances but i simulated it with the worst case senerio in terms on tolerances and it still worked.. I understand my bandpass not looking great but i don't understand it being skewed off by 200 mhz, especially since the engineering before me made the same mistake..

If anyone can notice anything i'm doing wrong it would mean the world to me. Thanks[/img]

[Odysseus]

Certainly, your layout seems unsuitable, assuming I'm interpreting your PCB screenshot correctly. A solid ground plane is usually required for good RF performance.
That said, I don't actually think your layout is the main culprit. More likely you used inadequate inductors with insufficient Q or SRF for your passband. Are any of them ferrite core? Some of them are so small I can barely tell they're present in your photo. They should all be size 0805 or larger with an air core.
Also, the design of your 3rd order filter is odd. You can see the same 70MHz peak in your own simulation screenshot.

[koffp]

odysseus

Thank u for you're explanation, I hope that's the problem.. I had to use these part beacuse of current avaliablity.. I didn't pay attention to the Q. I will try just ordering the through big hole version of them and pay attention to the Q.. or do u think it's better to just do microstrips. If microstips can u recommend an affordable

[Odysseus]

A microstrip filter isn't necessary for 500MHz. You just need appropriate inductors and maybe a better layout.
As an alternative to ordering through hole parts, you could wind some inductors by hand.

[koffp]

This is gonna go into a board that will be used in production so winding it by hand is not an option lol, thanks

[pigrew]

As has already been said, the layout looks questionable.

Do you have some EM simulation software like ADS, HFSS, Clarity, or microwave office? If so, it'd be an good exercise to simulate your layout to see if it matches your measurement. In addition, you may want to download spice/s-parameter models for the particular components you are using (which will include some parasitics).

Check that the manufacturer's website to make sure all components have a SRF > 1.5 GHz. NP0 capacitors <100 pF should be fine for these frequencies (in general).

It might not quite be necessary at 600 MHz, but I'd suggest going with a 4-layer board stackup, with a controlled impedances. This is pretty cheap from the likes of JLCPCB, but you may need to order from USA manufactures? (I personally like Sierra Circuits).

The GND pads of the components should be directly on the top GND plane, with vias close by. The long tracks to a GND via will add too much inductance.

Once you get into microwave frequencies, you need small component sizes. For >1 GHz, I'd only use 0402 or 0201 (imperial SMD sizes). Perhaps with 500 MHz, 0603 would be fine. The larger packages will have more parasitic series inductance. A 0.5 pF capacitor seems a bit small for 500 MHz... I think your layout will introduce parasitics of comparable magnitude.

JLCPCB has some example layout suggestions. Most of them are microstrip with the GND plane far away from the transmission line, but also CPW is OK to use (assuming you control the transmission line impedance correctly).

So... how to fix your current board? You might be able to improve the GND plane by soldering down some copper tape... might work, might not.

Also, it looks like some of your SMA connector's have non-soldered GND pads? You should solder all 4 GND of each connector (especially since there are not vias close to the connectors)

[koffp]

Pigrew

Thank you so much for the detailed explanation, I used ADS before but my current job doesn't have anything, looks like I gotta convince them. If I had ADS I would have just microstriped this already and called it a day. I can do micrstrip by hand, problems is that I will have to lay it out by hand in orcad and orcad PCB editor can only go down to 100um grid distance so that's sketchy but looks like I will have to try..

Odysseus told me to use 0805 parts with air core though? So should it be small parts or large parts? Large inductors small caps?

[pigrew]

Pigrew

Odysseus told me to use 0805 parts with air core though? So should it be small parts or large parts? Large inductors small caps?

I mostly do >2 GHz, so maybe I'm a bit wrong. I'd use ceramic core... Use CoilCraft's inductor selector tool (for example). For your 330nH, ferrite core will have a Q of 2 or 3 at 600 MHz... usable but not good. They don't even list any appropriate inductors larger than 0603. The 0603HP-R33 looks like a reasonable part. Looking at one of their air core parts (2929SQ-331), it has a SRF of 660 MHZ which makes it unusable. Smaller is usually better, except when the ESR is too high.

Maybe your filter can be redesigned to have larger capacitors (>1pF) and smaller inductors (<100 nH)? Those values would be somewhat more ideal.

[koffp]

Pigrew,I see I'll just focus on making sure it's the right SRF and low q..

Sounds like it would just be easier to microstrip. Do u happen to to know any microstrip design software out there that's under like 2-4 grand? I can design microstrips myself also but I will have to lay it out by hand cuz we use orcad.. I used ADS in college I wish I had access to it still...

[Marsupilami]

Hey koppf,

Let's say you ruled out every boring thing, e.g. misplaced component values.
The problem with your concept is that the PCB trace segments will have capacitance and inductance in the same magnitude as your lumped components. The reason to have a board with such specific geometries is to have those as needed, not randomly. Every detail has to have a purpose. Why the trace is thinner or thicker at one place, why the ground plane is farther. Why the ground connection of a component is longer, etc.
If I had to make one guess then then looking at your 3 pole design the middle shunt 1.1nH has such a small value that even a bit of trace inductance can offset your whole thing. Moreover if you assume you have more inductance there, the exact thing happens what your measurements show: center frequency shifts downwards.
Google a pcb inductance and capacitance calculator and see what kind of magnitudes you get. You could then update your simulation with added lumped components approximating your PCB effects. The difficulty with that is going to be that because you have the funky shapes there's no easy solution to that without EM simulation and that is absolutely overkill.

Example just to illustrate how difficult it is to get your design right with a 1.1nH inductor:
Microstrip line with Er 4.5, dielectric thickness: 1.6mm (~60mil), trace width 2mm (~80mils) will have 0.35nH per every mm (40mil)

HTH
Good luck

[koffp]

Marsupilami

Thank you for pointing out how much the trace inductance affects it per millimeter. It seems like I have to do microstrip since I can't change the inductor value without the input and output impedance changing and it has to stay at 50..

[G0HZU]

The obvious problem with your design is that you have used a BPF topology that is only suitable for bandwidths greater than about 30%.
You end up with crazy L and C component values just like you have in your designs. 

You are trying for about 10% BW so you need to swap across to a different filter topology. Try the topology below for your third order filter. You can see that the component values are much more sensible. Even so this filter will misbehave if you lay it out badly. The 25pF shunt caps will have some package inductance and you need to ground these as directly as possible otherwise the filter response will degrade. Also try and avoid any unnecessary shunt capacitance at the node between C2 and L1. The same for the other two resonators.

A 25pF capacitor ceases to be a 25pF capacitor at 540MHz if you insert just a few nH inductance in your PCB layout. The effective capacitance at 540MHz will go up if there is a few nH added inductance.

I've shown 1nH in series with the 25pF capacitors and this nH represents the package inductance of a typical SMD capacitor. So this 1nH isn't really a component. You get it for free within the SMD capacitor.

Ideally, the 33nH inductors will need to be adjustable types. Otherwise, you can try fixed 33nH SMD Midi Spring inductors from Coilcraft and then use two caps to make up the series caps so you can fine trim the capacitance. Otherwise the filter response will almost certainly be off tune slightly if you use single, fixed value components everywhere.

[max-bit]

unfortunately, incorrectly made ground paths (GND) why such long and still rounded paths? Only this brings additional inductances

[cdev]

Could you upload just a simple, head on photo of the current filter?

Sometimes they just say something (photos) thats clear.

[nctnico]

odysseus

Thank u for you're explanation, I hope that's the problem.. I had to use these part beacuse of current avaliablity.. I didn't pay attention to the Q. I will try just ordering the through big hole version of them and pay attention to the Q.. or do u think it's better to just do microstrips. If microstips can u recommend an affordable

500MHz is at the low side for a microstripline filter. What you need to do is:
- Use a double sided board with a ground pour on both sides but keep the pour 2mm away from the signal traces.
- Use inductors that have a self resonance way above the operating frequence
- Put the components as close to eachother as the outline allows
- Make sure there is a via connecting each capacitor to the ground plane as close to the capacitor as possible.

I have build similar filters myself on double sided boards; it is definitely doable. What may help is to use a 4 layer stackup or thinner board (0.8mm for example) so you can make the signal traces thinner and thus easier to route.

[koffp]

Thaks GHOZU, I didn't know I could change the topology like that

Nctnico so I can't use microstrip? I will try both options while I'm doing tests boards thanks

[cdev]

It has to be mass-produced.

That's often the problem,

This is gonna go into a board that will be used in production so winding it by hand is not an option lol, thanks

If you can make literally almost any kind of coil in a utterly predictable, reproducible manner you have also quite possibly solved your problem.

[cdev]

Getting a sharp response in a filter is usually gotten by using smart construction techniques, like offsetting the loops at perpendicular angles so that they dont influence one another. Shielding them may also help.Generally larger coils have more Q and make sharper filters. Skin effect matters, which is why coils are often silver plated. Using tubing or fatter wire also helps. If a coil requires a bit of tuning when its done with a variable cap, thats not a show stopper for me personally. Its kind of expected with some designs. Just design it so adjustment falls in the middle of some standard, stable part's range. Its interesting how what I would call social factors are impacting manufacturing, and why.

[Joel_Dunsmore]

For sure the first place to start is the parasitic elements in each component you use. Each capacitor has a series inductances (as another post said, 1 nH is a good guess to start with).  And each inductor has a parasitic shunt capacitor in parallel, maybe 0.2 pf up to a pF or more depending on the size of the inductor.  If the Self-Resonance Freq is given you can compute it.  And as also stated, you need to watch that you don't rely one very small or very large values of inductors and capacitors. I guess a rule of thumb is keep the reactance between maybe 10 and 250 ohms, so that 0.3 pF series cap is quite small to use for a 500 MHz filter, and as well the 330 nH inductor is quite big, each having reactance of over 1000 ohms at a freq of 500 Mhz.  That likely means you can't get the cutoff shape you hope for with the number of elements you would like to use.  Welcome to the real world.  Resimulate your filter after adding parasitic elements and see what the simulation shows.  That's a first order effect.  Ground via inductance and layout give a lot of second order effects that can build up as well.

[BigBoss]

You requested very sharp skirts to attenuate the sidebands. Therefore realizing such filter is almost impossible with lumped components at that frequency
Either you have to loosen the specifications or you should find a Distributed solution.
Also, components' tolerances at that frequency become very unstable so the filter response will also be undesirable.
Your layout is also too bad. Because the node between very high inductor and very small capacitor is very sensitive. A small amount of stray capacitance shifts the response to the sky.
There are some transformed based solutions. If they are connected in cascade, they may behave well. If you're agreed for 4-5 dB attenuation at center frequency, Distributed Filter on a cheap FR-4 substrate will give you
a consistent response.
 

[BigBoss]

An Implementation on a Rogers Duroid 6006 substrate.

[virtualparticles]

I noticed one thing in your layout which I see many engineers do. The connection traces between components look very wide, the same as the 50 ohm in and out traces. The impedance within a filter is not 50 ohms. It is much better to use skinny traces to connect the nodes and factor the trace inductance into the design. Having additional trace capacitance to ground is usually not helpful. For modeling you have to use an RLC or S-Parameter model which actually corresponds to each inductor, you can't use the idealized inductor. You can often use idealized capacitors as long as you check the self-resonance is high enough. Inductor Q usually dominates the loss.

A rough estimate for trace inductance is 20 nH per inch for a skinny trace.