RF PCB layout
RF PCB layout
(OP)
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
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





RE: RF PCB layout
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!
RE: RF PCB layout
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.
RE: RF PCB layout
Thanks
RE: RF PCB layout
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!
RE: RF PCB layout
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.
RE: RF PCB layout
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
RE: RF PCB layout
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!
RE: RF PCB layout
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.
RE: RF PCB layout
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.
RE: RF PCB layout
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.
RE: RF PCB layout
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!
RE: RF PCB layout
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.
RE: RF PCB layout
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.
RE: RF PCB layout
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.
RE: RF PCB layout
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.
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.
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!
RE: RF PCB layout
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?
RE: RF PCB layout
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/P1076...
uPC8181TB - http://www.csd-nec.com/microwave/english/pdf/P1511...
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?
RE: RF PCB layout
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 …
RE: RF PCB layout
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!
RE: RF PCB layout
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.
RE: RF PCB layout
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
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/PU104...
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!
RE: RF PCB layout
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.
RE: RF PCB layout
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).
RE: RF PCB layout
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 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_counte...
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/P1151...
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/...
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).
RE: RF PCB layout
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.
RE: RF PCB layout
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.
RE: RF PCB layout
Curious on this one myself...
RE: RF PCB layout
Curious on this one myself...
RE: RF PCB layout
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 …
RE: RF PCB layout
http://www.mrkenneth.com/scipho/layout.gif
Thank you for the information about the thermal relief (that's the term
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!
RE: RF PCB layout
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.
RE: RF PCB layout
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.
RE: RF PCB layout
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.)
RE: RF PCB layout
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.