RF PCB layout 5

[RichardMid]

Hi all

I am modulating a signal up to 433MHz. I am forced to use through hole components like regulators and variable resistors, and then of course the surface mount high frequency components. I would like to know if it will cause trouble if I use the RF and IF components on the same PCB. Should I try to seperate the low and high frequency components on the same PCB?

As I am unexperienced with RF and RF circuit board design I would like to ask a few more general questions. Is it necessary to use use decoupling caps on every connection to ground and Vcc. Should I try to ground the pins that need to be grounded as close as possible to the pins or doesn't it matter. Where can I find text on RF circuit board design e.g. hints and tips or rules of thumb.

Thanks
Richard

 

[melone]

Decouple EVERY POWER PIN!!!!!! (providing you have the space) Ground traces need to be short, fat and connected to a good ground plane. Minimize layer jumping, but add extra vias at each transistion to decrease impeadences. I am a big believer in the one solid ground plane, and therefore would not recommend trying to use seperate grounds.

Unfortunately, PCB layout / design is a specialty that cannot be easily taught by a few posts to a website. I would suggest finding a good layout person and bug them. We will try and answer as many questions as possible, but nothing beats having a mentor sit with you and critique your work.

Good luck and keep us posted on your progress!

 

[BrianR]

Further to what Melone said, you must also understand the performance of components over frequency when decoupling. Many capacitors are unsuitable for UHF use so some specific advice is in order here.

If you have the choice, then have one plane of the PCB all copper and use it as the ground with small islands removed for the via leads, but have all tracks on the other layer.

 

[RichardMid]

Thanks for the replies, it is exactly what I was looking for. Just one more grey area: I thought of using one side as ground plane, but what do I do with through hole low frequency components which will be present for oscillator tuning. Should I just leave a patch out of the grond plane with tracks there? I read somewhere that I should leave a patch out of the ground plane on the other side of a matching network. Is this necessary?

Thanks

 

[mrkenneth]

BrianR, you mentioned that "many capacitors are unsuitable for UHF use." Would the capacitor react in an unexpected way, or would the capacitance just be unstable? I cannot seem to find capacitors designed for microwave frequencies at Digikey at anything more than several pF. Would normal ceramic capacitors be okay?

How close should the ground planes be to other signals, such as Vcc or a high-frequency line? Also, how far should each ground via be? I am planning to get some 2-layer prototype boards professionally fabricated; will the vias be already connected, or would I still have to solder a wire to connect the layers?

Sorry for all the questions, I am new to high-frequency design too. Thank you in advance!

 

[BrianR]

mrkenneth, It can be quite difficult to identify a capacitor good for uhf from one that's not but some guidelines are:

1. Low self inductance. The inductance is derived from the lead inductance and the method of construction. Leads must be non-existant or very short in every case to minimise stray L.

2. Low loss factor or tan(delta). It is a function of the dielectric properties and the construction.

The actual impedance exhibited by the capacitor is (-jXc +jXl +Rloss) so you can see that once L becomes significant, you don't know what you have, except that the capacitor is not doing what you hoped.

Air spaced capacitors are best but mostly impractical through size. Miniature ceramics like chip caps are very good but if you need to carry much power then metal clad micas are worth a go. Where stable C is needed over temperature changes then a mica dielectric is best and ceramic is poor. Paper capacitors are useless at RF and so are electrolyetics of any kind.

An example of self inductance in action: a common brand 1nF disk ceramic with 1/8" leads will resonate at around 150MHz as will a 470pF disk with 1/4" leads. A simple calculation shows the 1nF C to have 1.126nH inductance. Metal clad mica capacitors are very good as as are chip capacitors. Neither have any leads and are constructed in low inductance fashion.

The loss factor counts when you need Hi-Q or high power.

 

[groundhog1]

To add to what Melone and BrianR posted..

The length of a part mostly makes up it's inductance. So if you have a long capacitor (long leads, or like a 1206 SMT), it will have more inductance. An 0402 package has the least inductance of the common package sizes. The circuit model is mostly a series RLC. So if the L is too high, your part will go through resonance and start looking like an inductor at your freq of 433MHz....and you originally wanted a cap!

The type of dielectric you pick mostly makes up the R in the equiv circuit.

You do want one continuous ground plane underneath specific circuits, but you can separate out big chunks.
If you have digital, power, low freq analog, and hi freq analog (RF) circuits on your PC board, you may want to separate to some degree, the ground planes. You want to make it difficult for undesired signals to travel on your ground plane and get into nearby sensitive circuits. You can put small slots in the grounds to separate them. Many times you can't totally separate the circuits but you can make the "bad" signal have to travel a very difficult path to get into your sensitive circuits. Some people connect separated planes with small choke type networks.

You can also place different circuits on opposite sides of the ground if you have say a 3 metal layer board with the ground plane in the middle.

You can also put ground areas on the top layers between traces. then you put vias from these copper "islands" down to the main ground plane. What this does is make it easy for fringe fields to terminate on the closest thing which may be the ground islands and get sinked to ground. THis is instead of fringing further (in the absense of the ground islands) and terminating on the next signal trace over...

Thin dielectric will help lessen fringe fields. But will make any controlled impedance lines thinner than if you have a thick dielectric board.

groundhog1

 

[mrkenneth]

Oops, forgot that I will be using capacitors that are all surface-mounted. So ceramics or micas would be the only (economical) choice.

The power required is less than 10mA, so surface-mounted capacitors should be okay. There should not be much temperature change in my application, so ceramics seem like the least expensive choice at the moment. As the capacitors are just for decoupling, I don't think a little variance in capacitance would matter, right?

What size would you recommend? I will have to hand-solder them, but would having a smaller package work better at RF? I am thinking about size 0603s for both the capacitors and resistors.

I will check the datasheets for the capacitors that I plan to order. I think they are Panasonic. How much inductance and impedence can be tolerated for bypass capacitors?

Thank you BrianR for the excellent comments!

 

[logbook]

0603 should be fine up to 500MHz. Use small decoupling capacitors (<=1nF) if you want to have useful decoupling at RF. NP0 dielectric preferable to X7R or Z5U.

Watch power dissipation in the 0603 resistors. 63mW max, but really keep it down below 50mW if possible.

Mixing IF and RF on the same board should not cause a problem. The amplifiers are tuned for a different frequency and therefore the interaction will be minimised. When you have a large gain all at the same frequency you get problems due to feedback through the power rails and ground. Changing the frequency eliminates this effect.

 

[mrkenneth]

Thank you logbook.

Would using 0402-sized capacitors work better for frequencies up to 2.45 GHz? I will be using the capacitors for a pre-amplifier > prescaler > frequency counter. Thus, the quality of the signal is not important, as long as the frequency counter can measure the frequency. The CEL datasheet recommends a 10nF capacitor though...

I will check out the capacitors with NP0 dialetrics. As for the resistors, the maximum power passing through them will likely be lower than 10mW, so that should not be something to worry about.

 

[logbook]

MrKenneth

0402 capacitors of the same dielectric would be better than 0603 by virtue of their lower inductance. However, you have to realise that at these sizes the tracking can be more significant than the capacitor. There is no point in using an 0402 then using 6mm of track at each end.

At 2.45GHz you should not be using ordinary general purpose capacitors. Manufactures have RF ranges of capacitors that are properly designed and characterised for the high frequencies.

An 0603 is "06" long and "03" wide. You can get capacitors the other way around (short and fat) which obviously reduces the inductance. For "real" microwave application the capacitors are flat. Imagine cutting a square from a piece of paper. The resulting capacitor is ultra thin top to bottom giving exceptionally low inductance. The only problem is the physical circuit construction. You now have a 3D circuit as the top of the capacitor is now a mounting/connection point.

Having re-read your posting, I don’t think much of this applies to you. Your application is primarily digital. After the prescaler everything is calmed down anyway. Coupling with a 10nF ordinary capacitor should be ok because you are not interested in esoteric analog stuff like VSWR, insertion loss, power dissipation etc. In this case you will be able to run the capacitor well above self-resonance and it will still pass a signal. The decoupling capacitors in the preamp are the ones you should concentrate on to prevent interference from the prescaler getting back into the preamp.

 

[mrkenneth]

Thank you for the detailed response logbook.

I did not know about the "fat" capacitors before until you mentioned it. I checked some datasheets and found that the 0508 and 0612 capacitors have much lower inductance. I think I will use the 0612 sizes since the microstrip line to the connector must be 115 mils.

I also checked the thin RF capacitors that you mentioned, but I could not find any with a high enough capacitance. Also, the capacitors would be very hard to hand-solder because the tweezers have so little contact area with the SMD.

The power decoupling capacitors for the preamp and prescaler should not matter, right?

Thank you for your continued help!

 

[logbook]

Power decoupling should not be under-estimated, even for the prescaler.

Consider this: as a capacitor goes through series resonance, the phase shift rapidly changes by more than 100 degrees. Hopefully the attenuation is sufficiently high that any loop phase shift that becomes zero is also associated with a loop attenuation of at least 15dB. If not you can imagine nasty power supply related oscillations.

If the preamp has 30dB gain and the power supply rejection is only 20dB you can see the possibility of instability. Good quality power supply decoupling in the preamp is therefore important. It is of course inadvisable to use a common power rail between preamp stages and output stages. There needs to be not only capacitive decoupling at each stage but resistor/inductor/ferrite "isolation" from the power rails to increase the power supply rejection ratio at high frequencies. The bigger the resistor/inductor/ferrite you can put in series with each stage’s power supply, the lower the requirement on the decoupling capacitor.

I would use solder paste and a hot air soldering gun to solder the paper thin capacitors to the mounting pads. There is then something called a "solder pre-form" or just "pre-form" which I believe are used for microwave interconnects, but which I have not used myself.

 

[mrkenneth]

I am thinking of powering everything from a battery (thinking of using a 12V 7Ah sealed lead-acid :-D) so the power supply not be very noisy.

Would a 1nF and 10nF 0508-sized capacitor for power decoupling (both preamplifier and prescaler) be okay? How large should the inductor be? Does the package matter as in the case with the capacitor?

Also, I will have to use a 78L03 and 78L05 to regulate the voltages down, since the preamplifier wants 5V and the prescaler wants 3V. Does this change anything (except for the additional decoupling capacitors before the regulator)?

How do I isolate the power rails between the preamp and output stage? Do I separate the two with a series capacitor and inductor? If so, how large should they be?

Sorry about all these questions. This is my first time designing a RF circuit.


P.S. I don't think I want to bother with the paper-thin capacitors. I still have not mastered my surface-mount soldering skills, and I don't even have a hot air soldering station. :~/

 

[logbook]

78L03 and 78L05 are nice linear regulators. They will not generate noise. The efficiency will be horrible (3V from 12V means less just than 25% efficiency) but then you are probably not worried about that. Just watch out that they will not deliver their "banner spec" 100mA with that much volt drop (too much heat to get rid of).

Question: Why do you need a capacitor at all? Admittedly a rhetorical question. If you have something taking rapidly changing currents then the regulator might not be fast enough to respond to the changing load. If you don’t have such loads then you don’t need huge capacitors. People normally use a 10µF somewhere near the regulator to handle the lower frequency current changes. Additionally, the 1nF and 10nF capacitors you have suggested will be fine.

How do you isolate the power rails? They are already isolated. You have one running on 5V and one running one 3V. Here is the situation: The prescaler changes state and kicks a little current transient into the power rail. You don’t want this transient to find its way back into the preamp. In order to get there it now has to go "backwards" through one regulator onto the 12V rail then "forwards" through the other regulator. This gives excellent immunity at modest frequencies. There is still ground coupling, but that cannot be easily eliminated.

Don’t worry too much about power supply isolation for this design. Get your hands a bit dirty and you will learn more than anyone can tell you. If you suspect interaction between the stages when it is built then you can cut one section out of circuit to prove the point.

When I started on surface mount parts I was using 1206 components. A contractor did a design for us using 0603 and they looked far too small. Now I am using 0603 most of the time and the 1206 size looks HUGE! This is just something you get used to with practice.

When I was talking about using inductors to separate the power supplies, that is for high current use. Suppose you load is 1mA. You can put 100R in series with the power rail and you will only get a 100mV drop. The extra impedance in the power rail gives the decoupling capacitors something to work against and gives good filtering to power supply noise. Unfortunately if your load current changes then it changes the power supply voltage. Thus you might pick 10R. You can’t sensibly go below 1R. In that case you might use a ferrite bead. These are tricky little beggars. They are say 1R at DC but can be as much as 300R above 10MHz. That is very convenient for power supply decoupling. Or you could use a good RF choke (inductor). In many respects the ferrite beads are nicer because the impedance is more resistive than an inductor. If the stage is taking 50mA you are forced to use either a ferrite bead or an inductor. Remember, all I am trying to do is to prevent a transient in one part of the circuit getting into another section of the circuit by means of the power rail.

I hope this makes sense. It is a lot to write down in a few words.

 

[mrkenneth]

Thanks for explaining everything! I understand it perfectly now!

The preamplifier uses 23mA and the prescaler uses 19mA. There will be 2 preamplifiers, which translates into 46mA for the 78L03, and 19mA for the 78L05. As for the efficiency, the 7 amp-hour battery should be good enough. :-D

The leads to the battery will probably be quite long, so would I need anything more than decoupling capacitors? Perhaps I should add a surface-mount ferrite or inductor?

I have included an image of the circuit I have at hand right now:

I still have a lot to do. ;-) I will add a ground plane after I finish routing all the components.

As you can see, the two preamplifiers on the left are currently sharing one power rail. Do you see any problem with that? Should I add something in between, or would the decoupling capacitors be enough?

I know all the components seem too spread apart, but I am leaving some room in case something goes wrong so I have more room to desolder them. All of the unlabeled components are capacitors, either 0508 or 0603.

If you see anything weird, please let me know!

Thank you for your continued help, logbook!

 

[logbook]

I would check your 78L03 data sheet. You have 48mA out with 9V drop. That is 432mA nominal. Let’s say half a watt worst case. The regulator won’t be damaged but will shut down if overheated. You may need additional copper to act as a heatsink. You need to look at the degrees celsius per watt figure from junction to ambient then figure out how hot the junction is getting.

Use surface mount ferrites into the power rail of each device, with a separate one for each amplifier.

Take a look at your layout and view the tracks to the coupling capacitors. The tracks are longer than the body length of the capacitor. The coupling is therefore dominated by the track inductance rather than the inductance of the capacitor. If those capacitors are costing extra money, that money is wasted. I don’t think the coupling capacitors are a critical application because it will be driving a 50R load. For the decoupling capacitors you have routed the power tracks through the capacitor pads which is totally correct – well done.

I couldn’t find the datasheets for the amplifiers using a websearch on 1507GV and PB1507. Who is the manufacturer?

 

[mrkenneth]

Argh! Digikey just cleared my cart! So now I will have to add my parts again!
Anyway, I just checked the datasheet for the Microchip TC11853 (sorry, it wasn't a 78L03, but a LDO regulator), and I am glad you mentioned it! The absolute maximum input voltage is 6V! Do you think I should connect the input of the 3V regulator to the output of the 78L05? (The 5V regulator outputs 100mA and can stand 300mW) The dropout voltage of the TC11853 (3V regulator) is 400mV at most. Should the power go like this?:
12 (or regulated 8V) input -> (ferrite?) -> 78L05 -> ferrite ->
prescaler AND TC11853 (3V regulator) -> 2 X [ferrite -> preamplifiers]
What do you think?

As for the coupling capacitors, how close should they be? Would rotating them 90 degrees be better? The 0508 capacitors cost around $0.30, while the 0603 capacitors of the same value cost around $0.10, both in quantities of 10. The difference is not too large if they yield better results.

The uPB1507GV preamplifier and uPC8181TB prescalers are both manufactured by NEC. Here are their datasheets:
uPB1507GV -

http://www.csd-nec.com/microwave/english/pdf/P10767EJ3V0DS00.pdf

uPC8181TB -

http://www.csd-nec.com/microwave/english/pdf/P15114EJ2V0DS00.pdf

Do you think I can connect the output of the prescaler to the input of the frequency counter using a USB cable? The maximum frequency from the prescaler should be 50 MHz at most, and a USB cable should be able to handle much higher. The power can use the same cable. Would that be okay?

 

[logbook]

You’ve got some problems here:

Putting the 3V regulator from the 5V output is ok, apart from the fact that you will then melt the 78L05. It is a common mistake to look at the current rating and forget the power.

You have 46mA at 3V and 19mA at 5V. Hence you will have 65mA at 5V. The drop from 12V will be 7V.

7V x 65mA = 455mW. Use a fat regulator, 78M05 and you will be ok.

Your circuit is wrong. The 1507 is labelled as a preamp and that is actually the prescalar.

The 1507 has a differential input. One input is IN; the other with a bar over it is the inverted phase input. You have connected them both together and will therefore get nothing in. You should drive it differentially, but you only have a single-ended amplifier. I don’t know if you could AC couple into just one side. I would recommend using a miniature 1:1 RF transformer to get a differential signal.

Sorry, run out of time tonight …

 

[mrkenneth]

I forgot to mention that I decided to use a big 7805 1.5A regulator for the frequency counter circuit (which has quite a few LEDs). So I can run the 78L05 off the 8V rail, and the resulting voltage drop would only be 3V. 3V X 65mA = 195mW, much lower than the rated 350mW.

I am very sorry for the incorrect labelling of the ICs. (The yellow text was added afterwards, and I mixed up the model numbers.) I have corrected the text in the image above. Thank you for looking at it so carefully!

I must have missed the dash above the IN for the uPB1507GV. I thought they were supposed to be connected. Thank you for noticing!
Do you think I should just follow the test circuit (on page 15 of the datasheet) and drive the prescaler single-ended?

I will take your suggestion and use 0603 capacitors instead of the more expensive 0508. I can find 0603 capacitors more easily than 0508 ones in case something goes wrong.

As for the ferrites, what should the impedance be?

Thank you for your continued support!