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

 

[logbook]

12V -->> 7808 == 8V (+ cap to ground)
8V -->> 7805 == 5V (+ cap to ground)

5V -->> ferrite -->> prescalar (+cap to ground)
5V -->> TC11853 == 3V (+cap to ground)

3V -->> ferrite -->> preamp 1 (+cap to ground)
3V – >> ferrite -->> preamp 2 (+ cap to ground)

That all sounds fine.

Looking at page 4 of the prescalar data sheet the IN(bar) signal does not appear to be a differential input as I at first thought (red face). However this input should certainly be decoupled to ground as suggested by you and the data sheet.

Looking in more detail at the system, I am now concerned with the nature of the signal. The prescalar has a very limited range of operation, say -15dBm to +6dBm. I could write this as -5dBm ± 10dBm. At 2.4GHz the gain tolerance on the preamps is ±3dB, or ±6dB for the pair. That suggests that your input signal has to be -49dBm ±4dBm. Is this what you intended? I would have thought you would have wanted some sort of limiter in there or some sort of variable gain stage coupled to a detector (AGC loop).

The frequency range of the prescalar is also remarkably limited. I thought it would go a lot lower than 500MHz.

I wouldn’t worry too much about the impedance of the ferrite. Just use whatever is easily available. In 0603 size, some ferrites go above 1K, but you ideally want something that is characterised up above 1GHz so you may not get better than 100R. I haven’t checked what is available.

 

[mrkenneth]

Thank you for confirming the power rails.

The uPB1507GV prescaler does seem a little limited, but it is the only one I can find on Digi-key with a divide ratio of 64 and can go up to 2500MHz. The lower frequency range does not really matter to me since the lowest frequency I would like to measure is probably around 800MHz.

The input signal will probably vary from -45dBm to -30dBm, measured with an Analog Device AD8361 evaluation board (bad antenna ). In an application note by NEC (sorry, I cannot remember which), it said using two amplifiers in seris will result in a lower gain (due to losses?). Around 35dB with the uPC8181TB. I guess I am risking it somewhat; would the prescaler die if the input power exceeds +6dBm?

The AGC seems interesting. Would it fit between the last amplifier and the input of the prescaler? NEC has this variable gain amplifier which works from 800MHz to 2500MHz:
uPC8204TK -

http://www.csd-nec.com/microwave/english/pdf/PU10408EJ01V0DS.pdf

This is the best one NEC makes. Would I use an AD8314 (or the lower-cost Maxim MAX4003 alternative) RF detector for the controlling the output. The circuit would act more or less like a power regulator, right?
However, if it is possible without the additional circuit, I would like to leave it simple so I will not encounter as many problems. I believe I may need to enclose the circuit in a Faraday cage (using copper clad board) to reduce external interference from entering the circuit.


Here is an updated version of the board layout with the voltage regulators:

http://s92795644.onlinehome.us/scipho/design2.GIF

(it may be too wide for the forum so I am posting the link instead.)

It is still without the ground plane yet. The entire bottom side will be pure copper connected to ground. How far should each ground via be? I plan to outsource this board to a PCB fabricator (which I have never done before). If it is professionally fabricated, will the vias already be connected? Or would I have to drill a hole, connect a wire, and solder both sides?


Thank you for all the suggestions!

 

[logbook]

If you get a professionally made double-sided pcb there will be no need to join from one side to the other yourself. The pcb will have plated through holes as needed. (Also known as stitch-thru’s and Vias). Obviously you and your pcb package will have to tell the manufacturer where these vias are placed. This will all be done by the pcb layout package when you produce artwork files (typically gerbers). Cheap pcbs in FR4 should work ok for your application since the tracks are so short.

http://www.pcbpool.com/

Doing a "pool" run will save NRE costs for photoplots.

The "faraday cage" you are talking about is a screened lid, and yes you will need one. I would use tin plate, brass or copper for this lid. For production use you might have one CNC punched or alternatively chemically milled. For a one-off you could just cut one out from sheet using scissors.

Put plated thru holes in a pair of parallel rows down the amplifier, connected to the ground plane. Then you can solder wires through from the ground plane to the screened lid.

If you don’t have access to a spectrum analyser it is going to be difficult to establish how well your circuit is working and how believable the result is. A level detector at the input to the prescaler might therefore be a very sensible idea. You could then do any gain adjustment manually, moving the antenna for example.

RE your layout, I would firstly rotate the amp to amp coupling capacitor 90 degrees so the track goes straight from one amp through the capacitor to the next amp. Just take the signal path and make it run in horizontal sections as oriented to the layout print you have shown. Move the ICs so the main signal track runs horizontally (viewed on the screen). I wouldn’t like to say how much difference this makes at 2.5GHz, but it is better for the signal to not go around corners too much.

 

[logbook]

The MAX4003 looks like a useful device which could usefully be included after the first preamp (it couldn’t take the full signal into the prescalar.

Watch out for the techno-babble in the data sheet where it refers to the non-existent quantity "true RMS power" (where it actually should say true mean power).

 

[mrkenneth]

Thank you for the information about the vias. Now I can put as many vias as I want without the thought of having to solder every one with wire. :-D Previously, I had built a Faraday cage for an Analog Devices AD8361 evaluation board using single-sided PCB copper-clad material. I just used some copper/aluminium tape to seal the edges and soldered it down to the copper board. The results from the RF detector was much better after the Faraday cage was built (much less background radiation without an antenna attached).

AD8361 evaluation board:

Board enclosed in Faraday cage (PCB):

I think I can do the same for this board, except that the circuit board can form one side of the Faraday shield.

Thank you for the advice about PCB Pooling. I think a friend of a friend of mine can help me with the PCB fabrication. ;-)

I started another thread dealing with a separate RF detector project that I plan to do here:

http://www.eng-tips.com/viewthread.cfm?qid=102209

I apologise in advance if I am violating any rules for cross-posting.
In case you wanted to know, I will be basing the frequency counter on this circuit:

http://www.qsl.net/dl4yhf/freq_counter/freq_counter.html

The preamplifier and prescaler will be used to extend the bandwidth of the frequency counter (from 50MHz to 3GHz).


As for the possibility of overpowering the prescaler, I think I have found the solution! I found an amplifier whose saturated power output is around +3dB. It can replace the second amplifier stage (currently the uPC8181TB). It is the NEC uPC2712TB:

http://www.csd-nec.com/microwave/english/pdf/P11510EJ3V0DS00.pdf

It can replace the second amplifier stage (currently the uPC8181TB). The maximum input power of the uPC2712TB is +10dB and the saturated output power is only +5dB. (Some output vs. input power charts are on page 8 of the datasheet.) This way, the circuit can still be simpler, and I will probably make fewer mistakes that way. ;-)

Also, I think you are right about having the high-frequency trace in a straight line. I think that is why the amplifier is oriented at 45 degrees on the NEC evaluation board (page 6 of the datasheet). I will redesign the circuit board.
I also found an application note from NEC that seems to provide very good information on designing amplifier circuits:

http://www.csd-nec.com/microwave/english/pdf/aply/P11976EJ2V0AN00.pdf

It suggests using a feed-through capacitor for the power decoupling. Do you think I need it in my current circuit? I would need to buy ten at once at around $1.60 CAD each (compared to around $0.10 CAD for regular ceramic capacitors).

 

[logbook]

Thanks for all the additional data.

Using the characterised limiting stage is an excellent idea.

Using three terminal feedthru caps can be a mixed blessing. These components are often used on interfaces to the external world, where high current operation is required without causing volt drops. If you can afford some volt drop, as you can in your application, then using a simple ferrite bead/capacitor filter may be better. The reason is this: the three terminal capacitor works by having a ground lead inductance which is remarkably low. If you fail to achieve this due to insufficient vias or poor tracking, then the three terminal capacitor will give a worse result than the ferrite/capacitor solution.

If you decide to use the feedthru cap solution, make sure you have a via on each side of the component, right next to the ground pad. (These components typically have a ground pad each side of the main current path.) I wouldn’t like to say that one solution was any more guaranteed than the other in this case.

 

[mrkenneth]

Thank you for the information. I think I will stick with the ferrite/capacitor solution because of the much lower cost. I have chosen a 120-ohm Murata ferrite:

It is the only one that could balance cost ($1 CAD for 10) and still have impedance/resistance at higher frequencies. Since they are sold in quantities of ten, I added another ferrite before the 78L05 voltage regulator.

As for ground pins/pads on the ICs and capacitors, should I connect the pad to the ground plane using a +, to prevent too much heat dissipation during soldering? I usually do this with through-hole pads, but I am not sure whether I should do this with surface-mount and with an RF circuit requiring low ground impedance.

I have redesigned some parts of the board to accomodate the new preamplifier (uPC2712TB)'s 5V power (vs. uPC8181TB's 3V). The preamplifiers are also at a 45-degree angle so the entire trace from input to output is a straight line. Here is the board (the board is too wide, so I am using an external link):

http://www.mrkenneth.com/scipho/layout.gif

Hopefully, everything is in order.

 

[MacGyverS2000]

As for ground pins/pads on the ICs and capacitors, should I connect the pad to the ground plane using a +, to prevent too much heat dissipation during soldering? I usually do this with through-hole pads, but I am not sure whether I should do this with surface-mount and with an RF circuit requiring low ground impedance.


Curious on this one myself...

 

[MacGyverS2000]

As for ground pins/pads on the ICs and capacitors, should I connect the pad to the ground plane using a +, to prevent too much heat dissipation during soldering? I usually do this with through-hole pads, but I am not sure whether I should do this with surface-mount and with an RF circuit requiring low ground impedance.


Curious on this one myself...

 

[logbook]

The ferrites look good.

On your layout, I know you are trying to be conservative and not pack everything in too tight, allowing room for ‘expansion’, but perhaps a few numbers might persuade you otherwise.

The inductance of a piece of wire is generally considered to be around 10nH/cm, or 1nH/mm. I suppose 1nH sounds like so little inductance that it wouldn’t be a problem. Ok, well let’s do our sums.

Z= 2*PI*f*L

Since you are working at 1GHz and 1GHz ‘cancels’ nicely with 1nH, 1nH at 1GHz is

Z= 2*PI * 1E9 * 1E-9 = 6 ohms.

I would guess that you have 3mm in the power feed from the capacitors to the preamp ICs, meaning 18 ohms. That is rather a lot in a 50 ohm system. I would suggest using shorter tracks on these critical parts. Remember you can put any length in series with the ferrite, it just adds more inductance, a good thing.

By a "+" I assume you mean a "thermal relief". People worry about thermal reliefs rather a lot, especially CAD people. I do things like put cuts in ground planes and then leave an open space in the solder mask to bridge the gap if that turns out to be better. I don’t like limiting my options! I have never had any trouble hand soldering SM parts to these huge planes. In fact a board I have just had returned (populated) is using huge copper lands as the heatsinks for some 78M05 regulators and it uses multiple vias to sink the heat through to a plane on the other side of the board to get more heat-sinking!. These pads are never a problem for re-flow systems because the whole lot gets heated up in the oven. Same with solder wave soldering of DIP parts. The whole board gets heated, so who cares. Yes it can be problematic with a hand soldering iron. Just put in a number 8 bit and cut the legs off the offending part and the pins will come out.

I am always wary of changing an existing working design, so if it already had solder reliefs then I would leave them, or if the company always used thermal reliefs then I probably wouldn’t argue to change them (not worth the personal risk) but if given a free hand I would just not bother with thermal reliefs at all. I haven’t seen any experimental or theoretical work on the extra impedance caused by the thermal reliefs, but I would be interested to see some.

Having said that, it occurs to me that heat flux is analogous to electric current. If the heat has a hard job getting through the thermal relief, doesn’t that make it hard for the electric current as well?

I think a 2D simulation is called for …

 

[mrkenneth]

Yes, this is my first time creating my own surface-mount board, so I am leaving more space. I will only be using a normal fine-tip soldering iron to solder the components, so I am not too sure of my abilities. I have reduced the decoupling capacitor to the preamplifier from 2mm to 1.5mm. So the impedance should be 9 ohms now. I don't think I can shorten the traks any more. Here is the updated board:

http://www.mrkenneth.com/scipho/layout.gif

Thank you for the information about the thermal relief (that's the term ). How would it apply for hand-soldering? I am just starting this, so I guess I should experiment a bit. I am not too sure what you mean about cutting the legs off. Do you mean the actual IC?

Looking at the AD8361 evaluation board again:

Near the top-right corner of the board at the RF In, is there a reason why the ground area beside the microstrip is tinned with solder? Is it for lower impedance with the bottom ground plane?
Also, any advice on the solder mask?

Thank you for the help!

 

[MacGyverS2000]

Ken,

Some personal experience with thermal reliefs, YMMV.

I designed a board with a thermal sink 15mm x 25mm for an SOT-89 regulator, more than enough heatsinking for the power I was going to be pumping through it... but I forgot to include thermal reliefs, and this was going to be hand soldered.

Try as I might, my 50W iron (Weller WES50) couldn't heat that plane up in a reasonable amount of time to melt the solder and not overheat the regulator. In the end, I used a Dremel to chop out a moat around the regulator, making the island a more reasonable 10mm x 10mm. Still, it took a good 5-10 seconds before the iron could heat it up enough to melt the solder.

I put a small bit of solder on the iron to enhance heat transfer to the plane. Set the iron on the plane until the solder melted. Quickly moving the component onto the plane so the plane couldn't cool off too much (and letting the component warm a bit), then I applied heat again to melt the solder a second time and attach the component. Needless to say, I didn't do too many of these boards

For a one-off board, add the thermal reliefs and leave the soldermaks open in case you need to bridge it (highly suggested for hand soldered boards). If you'll be production soldering these, there's no need for the relief, as mentioned.

 

[logbook]

When talking about cutting the legs off, I was talking about desoldering DIP parts which were soldered into ground planes without thermal reliefs. It is safer to cut the legs off the part and pull the legs out individually, rather than trying to desolder the whole package at once.

You will note that the evaluation board does not use thermal reliefs.

I did a 2D simulation on the resistance with and without a thermal reliefs, and the resistance went up by 30% on the comparison I did.

You should ideally be using two soldering irons, one for the 0603 parts and one fat iron for the bigger parts. I think MacGyverS2000 has too small an iron, or too small a bit.

This is quite an ambitious first SM project. Nevertheless I don’t think you will have too much trouble if your basic soldering technique is good on non-SM parts.

The solder strips on either side of the output trace of the evaluation board are a mystery to me. They are being used as a combined microstrip and coplanar waveguide. Removing the solder resist would seem to have no effect at all on the ground plane, unless they are allowing the user to put a little semi-cylindrical tunnel over the output trace to fully screen it.

I wouldn’t worry about the solder resist on your board. Just use the solder resist to protect against solder splashes, as you would on any other board.

 

[mrkenneth]

Thank you MacGyver and logbook for the responses.

I guess I will leave a thin line around the SOT-89 regulator and bridge the ground connects after the soldering is finished.

As for cutting the legs off ICs, I might want to reuse them later so... I guess ruining a single IC is better than ruining an entire board. Thanks for the suggestion.

I think Analog's evaluation board uses thermal reliefs for the ground connections for the resistors and capacitors. I had to look really carefully to find it.

What simulation program did you use? I would like to try some of the programs. (I have never used SPICE or similar software before.)

I will be using a larger soldering iron (that I normally use for through-hole components) for the heatsinks and the ground connections of the SMA and USB connectors. I will get another fine-tipped, low wattage temperature controlled soldering iron for the surface-mount components. Thank you for the suggestion.

I will have to practise soldering and desoldering some ICs and 0603 parts on spare boards first.

Logbook is probably right about the tinned solder strip there to allow for adding a grounded shield. (Actually the microstrip with the tinned ground beside it is the input. The output is a DC voltage on the left side of the board.)

 

[MacGyverS2000]

Just an offhand comment about the soldering irons...

You mention getting a low wattage version for SMD. What you want is an iron that has a decent temp control to it. Higher wattage is usually confused with higher heat, but this isn't necessarily the case. A higher wattage iron allows the iron to replenish its heat more quickly as it is wicked away by larger heatsinks, but it will not raise the temperature of the iron's tip.

50W is more than adequate for most SMD work, but you may want more power if you find yourself needing to solder parts to large ground/power planes. It's better to have extra power rather than too little.