Single sided 75Mhz board
LoopyByteloose
Posts: 12,537
Being abroad, I have limited resources and more concerns.
I have laid out boards on Eagle for the SX-28 and teh SX-18.
I am wondering about frequency limitations due to possible RFI or EMI as it seems a two-sided board with ground plane would be better.
Gunther's book mentions that the crystal and resonator oscillators generate Sine Waves, which reduces the RFI.· Some other devices generate square waves, that may create VHF band RFI.
I could use any sugestions as I would prefer not to upset·someone from the government here with RFI.
▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
G. Herzog in Taiwan
Post Edited (Kramer) : 10/12/2005 6:27:28 PM GMT
I have laid out boards on Eagle for the SX-28 and teh SX-18.
I am wondering about frequency limitations due to possible RFI or EMI as it seems a two-sided board with ground plane would be better.
Gunther's book mentions that the crystal and resonator oscillators generate Sine Waves, which reduces the RFI.· Some other devices generate square waves, that may create VHF band RFI.
I could use any sugestions as I would prefer not to upset·someone from the government here with RFI.
▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
G. Herzog in Taiwan
Post Edited (Kramer) : 10/12/2005 6:27:28 PM GMT
Comments
concerning EMI issues, it is very difficult to propose a certain layout which guarantees that the EMI values are below the limits. For one of my commercial SX-base projects, I went through the whole appoval process in an EMI lab (BTW: a very expensive matter).
When you hook up a scope capable of such high frequencies to the OSC1 pin, you will see a sine wave with a crystal or resonator connected to OSC1/OSC2 where external clock generators usually have a square wave output. So using crystals/resonators instead of external clock generators can slightly reduce EMI.
The major source of EMI is the "ripple" imposed on the power supply lines by the fast switching SX. Therefore it is most important to get rid of this "ripple". Here are some methods:
Place a filter cap with low parasitic inductance as close as possible to the Vdd/Vss pins.
Using a ground plane connected to Vss can work as a shield. On the other hand, feeding the supply voltage to the SX through two parallel traces of equal length if possible may be better.
Reducing the supply voltage e.g. down to 3.3V also reduces EMI.
Using EMI filters in series with critical signals leaving the PCB can help.
Reducing the gain of the SX oscillator circuit (using OSCHS2, or OSCHS1 instead of OSCHS3) can also help.
I did all my initial EMI test with two-layer boards but ended up in a re-design with four-layer boards. One of the the two inner layers is connected to Vss, and the other one to Vdd. This way, the inner layers make an almost ideal filter cap that dramatically reduces EMI radiated from the supply lines.
As you may have noticed, in the list above, I often used the words "can" and "may". Dealing with EMI comes close to reading a crystal ball
A while ago, there was an active thread in this forum (search for "EMI Failure"). There you can find many more details, and I suggest to post to this thread concerning EMI issues to make it alive again.
▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
Greetings from Germany,
G
I do understand the reason for 'can' or 'may' because you have no control over my design process.
I will consider redesigning for at least two layers, maybe later I can afford 4 when I really understand what I want.
In the interim, I will leave the fast clocking to the SX-48/52 proto board.
In the interim, I happen to have a supply of metal boxes that are quite cheap. This is similar to Kevin's suggestion
I can also design the boards to at least fit inside and ground to that.
From what I understand from my early Ham radio studies, a complete metal cover will eliminate most of the problems and require less from the board design.
Is there a formula or 'rule of thumb' for sizing the filter capacitor? Right now I am thinking 'huge', like a 1 Farad at 16volts.
▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
G. Herzog in Taiwan
Concerning filter caps, don't think "big", as this may be "small" in reality. I strongly recommend that you have a look at the "EMI Failure" thread because there I made a longer post concerning this topic. I'm sure you understand that I don't want to repeat this here.
BTW, if you look at the SX48/52 Proto Board, you will notice a total of four SMT filter caps around the SX. This is an ideal solution by two reasons: First, SMT caps don't have leads, i.e. the parasitic inductance is relatively low and second, with the caps in parallel, the parasitic inductances are also in parallel, so the resulting capacity is the sum of all caps where the resulting parasitic inductance is a fraction of the parasitic inductance of one single cap. On the other hand, there are relatively long traces carrying the clock signal which can "nicely" act as antennas for the clock signal, or one of its harmonics. So I would not take for granted that the SX48/51 Proto Board passes an EMI test.
▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
Greetings from Germany,
G
Am I getting EMI and RFI mixed up?· I'll take a look at the EMI thread.
As it seems....
You build it according to your best guesses. If you are not a good guesser, ask a better one and learn how to guess better. Then after you build it, you try to understand and improve or to fix its faults.
Some of my knowledge is very out-dated.
Sorry, no call sign as my parents put a stop to the Ham radio (about 1960 or so).·The neighbors didn't want me interfering with their TV reception. I did have a 20meter WWII reciever and transmiter that were ready to go, but never put more than a dummy load on it and just listened to code.
▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
G. Herzog in Taiwan
Post Edited (Kramer) : 10/12/2005 7:03:08 PM GMT
Anyone interested should read it instead of asking Gunther, et al to repeat it.· Use the Search function to locate it.
▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
G. Herzog in Taiwan
I agree with you, a two layer board with a gound plane on one side, and a power plane on the other will be better than one with ground planes on both sides. As you said, it depends a lot on the gaps caused by component traces. So it requires a careful layout, espacially to avoid "islands", i.e. areas that can't be connected to ground or power at all. With ground planes on both sides, you can connect such islands to ground on the other side of the board in most cases by placing vias.
After the experiences I made in the EMI lab, I decided to swich to four layers to avoid EMI problems as good as possible. The extra costs for four layers are not that high, compared to the additional time I might have spend in the EMI lab to get a two layer board "quiet" enough. BTW: I have also provided ground planes on the two outer layers. Maybe it would have even be better to provide a power plane on one outer side. This way, the four layers could be sequenced power - ground - power - ground acting as a very good filter cap.
▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
Greetings from Germany,
G
1. use SMS components for the OSC, even if you have to hand solder them. After all, the most are two capacitors and one resistor.
2. eliminate putting a 4 pin SX-Key/Blitz interface on the actual board as and addition added feature. Build an adapter/converter. You can unplug the 3-pin resonator and used the socket to get 3 of your 4 required leads to a small adapter board for the SX-Key. Since it is temporary, the V+ could be a flexible wire that jumps to a pin in any convienent location. When you remove it, the long leads go with it.
3. use the 3 pin resonators with built-in capacitors to further avoid parasitic inductance problems.
In this way, you still have the ability to program in place, but you will only have additional EMI from the programing interface when you are actually using the adapter.
I hope you can visualize what I am talking about.
That leaves the I/O and the Power supply lines. Much of the talk above and in the excellent prior posting address those problems.
But, it seems that I/O should not be as bad because it is genrally not clocking as fast as the OSC.
▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
"When all think alike, no one is thinking very much.' - Walter Lippmann (1889-1974)
······································································ Warm regards,····· G. Herzog [noparse][[/noparse]·黃鶴 ]·in Taiwan
reducing the length of PCB traces carrying OSC signals is always a good idea. Nevertheless, external capacitors required for some resonators/crystals don't really cause parasitic inductance problems, and the OSC traces - to my experience - are not the major source of EMI. As mentioned here before, and in more detail in the "EMI Failure" thread, the major sources of EMI are high frequency signals imposed on the power supply traces due to the fact that the SX (like any other switching devices) does not draw a constant supply current. Instead, it increases and decreases at the clock rate, or at a fraction of it. Therefore, filtering (or buffering) the supply voltage is the main issue for reducing EMI.
As Dan mentioned, if a radiating trace can't be avoided, it is important to have another trace of equal length, as close as possible in parallel where the current flow in this trace is inverted by 180 degrees. This way the electromagnetic fields emitted by the two traces will compensate each other because they are 180 degrees out of phase. Ground planes act as shields to a certain degree but I even saw designs with two separate, parallel supply traces going from the chip's Vdd/Vss pins to the power in connector, or regulator output, both surrounded by a ground plane, instead of connecting the device's Vss pin directly to the ground plane.
▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
Greetings from Germany,
G
I suppose that I should order some 3.3volt low drop out regulators, too. That seems to be a win/win for battery operations - more juice and less EMI.
I had not really considered making a commitment to lower power designs or hybrid power designs before this as I have struggled with a lot of procurement problems when buying standard +5 components [noparse][[/noparse]Like the MAX232 chip]
I suppose I could just power the microcontroller at +3.3v [noparse][[/noparse]maybe by using a separate regulator], then shift to another logic family powered by a +5v regulator as required.
Ribbon cables are used to reduce 'cross-talk' by grounding every other lead. Do they have an EMI dampening effect too? I have been wanting to use them for building 'daughter' boards for the SX-48/52 proto board.
▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
"When all think alike, no one is thinking very much.' - Walter Lippmann (1889-1974)
······································································ Warm regards,····· G. Herzog [noparse][[/noparse]·黃鶴 ]·in Taiwan
instead of using two different regulators, you might consider using other components that also allow for 3.3V operation, like the MAX2323. In this case, you even don't need a regulator. When you use four rechargeable batteries, the initial supply voltage will be around 4.8V, and the system will safely operate down to 3.3V, or even below without the loss caused by the regulator.
▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
Greetings from Germany,
G