EMI failure
XGen
Posts: 8
Greetings all,
My prototype board has just failed EMI test, and it failed quite badly.
The results where it failed.
149.49Mhz dBuV/m is 58 limit is 30
199.24Mhz dBuV/m is 51 limit is 30
249.05Mhz dBuV/m is 48 limit is 37
From this I'm assuming it is the Murata 50Mhz ceramic resonators causing the problems.
I have a series resistor going to OSC2 (which is 0Ohms atm), and hopefully I can make this 1k or 10k
to help reduce the EMI problem.
Unfortunately I don't have any way to test my device, my FM radio only goes to 110Mhz.
So here are my questions.
How can I test my device without spending $100k on nice test equipment ?
Has anyone used a SPREAD SPECTRUM CLOCK OSCILLATORS at 50Mhz http://www.mercury-crystal.com/ to
reduce EMI ?
Any other advice/tips ?
Oh, putting it into a metal enclosure had 0 effect. Think its because I have 2 holes in the box
Thanks
CC
My prototype board has just failed EMI test, and it failed quite badly.
The results where it failed.
149.49Mhz dBuV/m is 58 limit is 30
199.24Mhz dBuV/m is 51 limit is 30
249.05Mhz dBuV/m is 48 limit is 37
From this I'm assuming it is the Murata 50Mhz ceramic resonators causing the problems.
I have a series resistor going to OSC2 (which is 0Ohms atm), and hopefully I can make this 1k or 10k
to help reduce the EMI problem.
Unfortunately I don't have any way to test my device, my FM radio only goes to 110Mhz.
So here are my questions.
How can I test my device without spending $100k on nice test equipment ?
Has anyone used a SPREAD SPECTRUM CLOCK OSCILLATORS at 50Mhz http://www.mercury-crystal.com/ to
reduce EMI ?
Any other advice/tips ?
Oh, putting it into a metal enclosure had 0 effect. Think its because I have 2 holes in the box
Thanks
CC
Comments
I'm curious, how does one get a product tested for EMI ? How much does it cost ?
Bean.
▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
"SX-Video·Module" Now available from Parallax for only $28.95 http://www.parallax.com/detail.asp?product_id=30012
Product web site: www.sxvm.com
"It's not getting what you want, it's wanting what you've got."
·
Its costing me about $420, the South African Buro of services is testing it for me.
I need to comply with IEC CISPR22 ClassB
If it fails, they have given me two week where they would re-test it before issuing the test results.
I though he might have chimed-in by now.
Bean.
▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
"SX-Video·Module" Now available from Parallax for only $28.95 http://www.parallax.com/detail.asp?product_id=30012
Product web site: www.sxvm.com
"It's not getting what you want, it's wanting what you've got."
·
My suggestion is to get a RF meter with a wand designed for near-field RF measurement (no I don't know where to obtain one), you would move the wand near suspect traces trying to find the culprit. When you find what you think is the problem, you can add a parallel termination resistor to reduce reflections. Here is a page describing termination. Then measure the trace RF emission again to see if the resistor improved the EMI. Do this until you have reduced the EMI radiation from all problem traces, then redesign your board to either alter the trace lengths or add space to incorporate the termination resistor.
Doing this does not guarentee your EMI problems will go way because there are other potential sources of EMI, an alternate method to determine if improper termination is a problem is to alter the oscillator frequency. If you find that does not affect your EMI then the likelyhood that trace termination problems are the issue is reduced.
I do remember seeing a home built RF meter, I'll see what I can do about scaring up the reference.
One recommendation (which may be too late for your application) is to have a ground plane around the resonator.
What are you using for your OSC drive level ?
On my Video board I used OSCHS3 and when I changed it to OSCXT2 the current when down alot.
It was using the Parallax 50MHz resonator too.
It's worth a shot.
See this post:
http://forums.parallax.com/showthread.php?p=536213
Guenther talks about having the same problem.
Bean.
▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
"SX-Video·Module" Now available from Parallax for only $28.95 http://www.parallax.com/detail.asp?product_id=30012
Product web site: www.sxvm.com
"It's not getting what you want, it's wanting what you've got."
Post Edited (Bean (Hitt Consulting)) : 5/27/2005 9:18:57 PM GMT
I definitely will chime in here as I have made my own experiences with the SX and EMI issues.
Today I've been too busy with my "food-generatring" projects, so I could not reply to this thread in detail. Please allow me another day to collect some details before I address this matter.
▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
Greetings from Germany,
G
as others already mentioned, avoiding EMI sometines comes close to reading a crystal ball, and to black art, as Paul wrote. There are many different reasons, or combinations of reasons why excessive RF signals are generated.
With two of my commercially developed SX 28-based units, I went through EMI tests here, and the first prototypes showed results similar to what you have obtained.
Before getting into details, let's name some of the parts that can act as antennas (mostly for the clock signal and its harmonics) causing EMI:
- PCB supply traces
- PCB traces with the clock signal
- Cables or leads connected to the PCB
- Other components, or PCB traces
Filter Capacitors
As the SX is a clocked device, it does not draw a constant supply current but the current rises and falls according to the clock frequency. Therefore, a filter capacitor is usually placed and connected to the Vdd and Vss pins. You often find a 0.1 µF ceramic capacitor used for that purpose.
If this capacitor were an ideal capacitor it would perferctly do the job, filter out the ripple on the supply leads, and if there is no ripple, the leads can't radiate any RF signal.
Unfortunately, capacitors are not ideal. Simply spoken, a real capacitor consists of "parasitic" inductance in series with the capacitance where the inductance is mainly caused by the capacitor's leads, and the traces between the capacitor and the supply pins of the chip.
In order to reduce this inductance, the capacitor leads and the PCB traces between the capacitor and the Vdd/Vss pins of the SX must be as short as possible. Every 1/100th of an inch counts here, even an eventually used IC socket. When using a socket select a so-called "precision" type as they usually have shorter leads than the cheaper sockets with spring contacts.
Using SMT components allows for shorter leads, so if possible at least use an SMT type for the filter cap.
As I had mentioned, a real capacitor has an inductive component. A capacitor in series with an inductance is also known as absorption circuit, i.e. for a certain resonant frequency it acts as a short. You can make use of this fact, and select a capacity that, together with the parasitic inductance, builds a short for the clock frequency of 50 MHz. The only problem is that you don't know the value of the parasitic inductance. Therefore, you would have to try various values until you find one giving the best result.
I did some experiments with capacitors between 100...470 pf instead of the "standard" 0.1 µF filter capacitor which reduced the radiation by about 5 dBµV/m.
Clock Device
Well, although the clock device is the basic source for EMI (remove it, and EMI is gone
I have experimented with Murata ceramic resonators, crystals, and external PLL clock generators. While there was no big difference in EMI when using resonators, or crystals, external PLL clocks remarkably increased EMI. Obviously, the square wave signal with steep signal edges generated by the PLL caused the generation of stronger harmonics.
You can configure the gain of the SX-internal clock circuitry using the DEVICE OSCxx directive. For a 50 MHz resonator, the datasheet recommends OSCHS3. I tried lower gains using OSCHS2, or OSCHS1, and found that this reduced EMI by some dBµV/m. As Bean had mentioned, when using a lower gain, like OSCXT2, the supply current dropped a lot. Lower supply current means less ripple on the supply lines, i.e. less EMI. On the other hand make sure to select a gain that safely starts the oscillator on power-on within the expected range of supply voltage, and ambient temperature.
I also tried to use lower clock frequencies. For my applications, an SX clocked @ 20 MHz was still fast enough but this did not really reduce the EMI problems, just caused peaks at other frequencies, and more peaks in the tested frequency range, i.e. instead of peaks at 50, 100, 150, and 200 MHz, there were peaks at 20, 40, 60, 80, 100, etc. MHz, so I returned back to the 50 MHz clock very quickly
Supply Voltage
During my experiments with the prototypes in the EMI lab, we suddenly had a drop of the measured EMI signals below the allowed limits. It took me a while to find out the reason: Due to some component failure, the supply voltage had dropped down to 3.5 Volts.
Again, lower supply voltage means less ripple on the supply lines, and less EMI. Therefore, if possible, run the SX at 3.3 Volts, or even less (minimum is 3.0 Volts @ 50 MHz).
PCB Layout
You can never completely avoid ripple on the supply lines. Therefore, the PCB should be designed in a way that the supply traces don't act as antennas. You often read the suggestion that the PCB should have a ground plane. This sometimes can make EMI problems even worse - why?
Using a ground plane with the Vss pins connected to this ground plane means that the Vss supply has a realtively low impedance (which - on one hand - is fine). On the other hand, the Vdd lead remains as a trace of certain length, i.e. it nicely acts as an antenna for EMI signals.
A better solution would be to use separate traces for Vdd and Vss in parallel, and of equal length when possible. This means that both will act as antennas but with a 180° phase shift. Thus the radiated RF signals compensate each other. You still can have a ground plane on the PCB but you should only use it as a shield between the supply traces and other signal traces.
In general, supply traces, and signal traces (especially the ones connecting the board to the "outside world") should not be arranged in parallel over longer distances, if possible. This avoids that RF signals on the supply traces are induced into signal traces which then - together with externally connected leads - would again act as antennas.
For the final design of my PCBs, I decided to use 4-layers where the inner two layers are pure supply layers, i.e. one connected to Vdd, and the other connected to Vss. These two supply layers make up an almost ideal capacitor with low parasitic inductance for filtering the supply voltage. The top and bottom layers both also have ground planes where these are only used a shields, and not to supply the Vss potential to any of the components.
Avoiding Radiation of External Leads
For additional safety, you might consider to run signals that are connected to the "outside world" through EMI filters like LCL filters. For example the Digikey P9808CT-ND item which has a maximum filter effect @ 100 MHz. You should place such filters as close as possible to the PCB connectors.
Another method to keep external leads from radiating is to use ferrite beads around such leads close to the PCB connector. In my experiments, I finally found out that this was not necessary because when you make sure that the source of this evil is handled properly, external leads have nothing to transmit, and therefore don't need filters.
Metal Enclosures
Yes, I also had this idea - briefly spoken - it did not work. You always have at least the supply voltage going into the box. RF does not care that this actually is an input - it uses it as output! In real life, there are more than just the supply leads connected to a device - IOW, more antennas.
I'm pretty sure that a metal enclosure, designed according the rules for RF devices with filters for all in- and outgoing signals would help against EMI but I think this is more expensive than taking care to eradicate the sources.
BTW, Ubicom once has published an application note concerning EMI. As I'm not sure if this document is publicly available. I simply have attached it to this post.
I hope that my experiences with reducing EMI generated by the SX helps you and others. By no means do I claim to be an expert in this area. I hardly had to learn my lessons, and I welcome everybody to share his experiences with us because EMI is an important topic when you want to "go commercial" with the SX (as with any other device).
▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
Greetings from Germany,
Günther
Post Edited (Guenther Daubach) : 5/28/2005 8:36:55 PM GMT
in my previous post, I forgot to mention that my boards passed the EMI tests, after I have changed to the four-layer design, together with EMI filters in series with the power supply lines, and some other I/Os.
▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
Greetings from Germany,
G
I have a pdf on the subject that I have found to be of great assistance.· Unfortunately, it is just a bit too large to fit in the maximum permitted attachment of this here forum.
If you send your email, I shall be happy to forward it directly.
Bongo
Are you saying that changing the frequency from 50MHz to 20MHz had no effect ?
I would have thought that (if nothing else) the lower current draw from a lower frequency would make the EMI lower.
Anyone,
I have access to a high frequency spectrum analyzer from work. How would I use it to determine relative EMI from a design. I realize the EMI levels would not be calibrated, but at least I could try different things and see the relative effects on EMI.
Would I just use some kind of simple antenna ?
Bean.
▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
"SX-Video·Module" Now available from Parallax for only $28.95 http://www.parallax.com/detail.asp?product_id=30012
Product web site: www.sxvm.com
"It's not getting what you want, it's wanting what you've got."
·
using a 20 MHz clock instead of 50 MHz did actually result in lower EMI values but the values were still above the limits, and - as I had mentioned - there were more harmonics within the range between 30 and 250 MHz.
▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
Greetings from Germany,
G
It looks like 99% of the people I've spoke with so far have said 're-design PCB'.
So here is what I'm going to try. There is a company in S.A that helps with EMI development.
(only found out about them this morning) Go to them with my prototype boards, and see if I can get it through the test by changing the settings Bean suggested. Otherwise it is going to mean a redesign of the PCB. [noparse]:([/noparse]
The worst thing about this EMI is I don't have access to equipment where I could test with.
Guenther, thanks for the post, I thought my only problem would be my resonator.
I'll keep you all updated.
I have access to a high frequency spectrum analyzer from work. How would I use it to determine relative EMI from a design. I realize the EMI levels would not be calibrated, but at least I could try different things and see the relative effects on EMI.
Would I just use some kind of simple antenna ?"
Yes, for poking around near-feld on a PCB, for an indication as to which area is radiating hardest, you can easily make uncalibrated but useful antennas.
One would be just a length of co-ax cable, with half an inch or so of the shield stripped off at the end, so there's a simple stub of the central core sticking out. Cover it wih gluey heatshrink, and go probing. It's a tradeoff between length, frequency and sensitivity, but don't get too hung up on it - it's just a location tool, and works well. (If your spectrum analyser doesn't have quite the sensitivity you need, for such feeble antennae, pre-amps turn up on ebay pretty often, and have almost no downsides (and act as a sacrificial front end to the priceless attenuator / mixer stage in my out-of-maintenance spectrum analyser)
For lower frequencies, especially chasing power supplies, I also use 5 turns, on a 1" diameter, of wire wrap wire, between the core & shield of a coax cable.
Note also that, if you're hunting for spikes, what you see may well not be coming from your equipment. Turn it off, to see if they go away. I've spent more time than is funny chasing down cellphones, taxicab radios, and FM radio stations. This weekend's project was to start building a quiet room at home for chasing EMC. Naturally, the wall panels (and door) I've got are 2" taller than the room I'm installing it in, so I've been stripping floorboards and ceiling panels out. I'm never going to be able to sell this place [noparse]:)[/noparse]
Steve
Are you making a "faraday cage" room. That would be very useful for testing.
I will give your idea a try when I get a chance.
Bean.
▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
"SX-Video·Module" Now available from Parallax for only $28.95 http://www.parallax.com/detail.asp?product_id=30012
Product web site: www.sxvm.com
"It's not getting what you want, it's wanting what you've got."
·
http://www.emctest.com/pdf/ShieldSelGuide7181.pdf
It's all very simple stuff, except for the door, which contains more brass than I've ever seen in one place before - ridiculously heavy.
I suspect you'd get very similar results by just lining a room with sheets of steel, and carefully rivetting / soldering the joints. The door would need some care, but with careful design, and interlocking overlaps, I suspect it'd work fine. Maybe wouldn't last as long, (or look as impressive) as the Lindgren one, but the price and weight would be much, much better.
(That said, since I'm building the chamber smaller than it originally was, if anyone in the UK wants to make me an offer for some steel-clad chipboard sheets (some with floor tiles) and associated assembly hardware, let me know...)
Steve
Bongo,
I'm also interested in this document - is there any URL or FTP site from where it can be downloaded? If not, you would do me a great favor eMailing it to g.daubach@mda-burscheid.de
▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
Greetings from Germany,
G
Same here on your document.
Smartdim@aol.com
I don't have accress to a spectrum analyzer here. Instead, for informative tests, I'm using a scanner with a frequency range from 20 to 500 MHz, together with a "near field probe" similar to what SteveW described. Of course, this is not really a test equipment but it is at least good enough to determine relative changes in radiation.
No matter which equipment you are using - in order to make relative measurements, it is highly important to always reproduce the same conditions, i.e. same position of the board, the "antenna", all cables connected to the board, and the position of any obstacles around that might act as reflectors. Therefore, it is a good idea to use a lot of sticky tape to keep all these items in position. Fortunately, there is no radio station transmitting on my "favorite" 1st harmonic @ 100 MHz otherwise, I think I'd have a problem, or would need a quiet room like Steve.
▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
Greetings from Germany,
G
before keeping you too busy sending around the document by eMail, I volunteer to put it on my WEB space for download by anyone being interested.
▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
Greetings from Germany,
G
And I cannot direct you to a URL, have forgot where I found this little gem..........
bongo
thanks for eMailing me the EMI document. I briefly skipped through it, and I agree that it contains a lot of helpful information.
In the meantime, I have posted it on my webspace - it can be downloaded from www.g-daubach.com/docs/emi276.zip
▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
Greetings from Germany,
G
Very interesting reading, and in my case, very timely.
Cheers,
Peter (pjv)
It doesn't dwell as long as I'd think appropriate on the vital importance of slowing edges down, as much as possible, wherever possible, before they become a problem.
Clocks don't want to look square - a sine wave (for fast stuff, or a square wave with substantially sloping edges for slow stuff), will work perfectly, and will radiate orders of magnitude less. Series launch resistors are pretty cheap - certainly cheaper and easier than trying to stop the noise once it's generated.
Similarly, fast buses often benefit from taking the edge off them with launch resistors, and systems can even run faster, since you don't need to wait for reflections to die down. (Note - those edges that look so nice and controlled on your 50MHz 'scope may well be vicious, ringing-infested monsters in real life...)
Things as trivial as putting LED current setting resistors between the pin (close to the pin) and the LED, rather than between the LED and the power rail, mean that the high frequency noise from inside the die is coupled to a much shorter antenna. That's worth a few dB, especially on a SX design, with its noisy die and (conventionally) not very much exernal hardware.
Stopping EMC before it starts is definitely worthwhile, and far, far cheaper than trying to keep it inside a metal box, with filters on all the wires.
(For a living, I design far-too-much electronics into far-too-small plastic boxes, and then have to get the results through the tightest flavour of CE regulations, and then a bit more, to avoid annoying herringbone interference patterns on the UHF TV signals. Aargh [noparse]:)[/noparse]
On your 4 layer layout. Do you NOT connect Vcc and Gnd to the planes until they reach the SX ?
IOW: Do you run them parallel from the board connector to the SX then at the SX they connect to the plane layers.
Or is it better to connect to the plane layers right at the board Vcc and Gnd connector, then just connect from the plane layers to the SX ?
I hope you understand what I'm asking... I'm having a hard time explaining it.
Bean.
▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
"SX-Video·Module" Now available from Parallax for only $28.95 http://www.parallax.com/detail.asp?product_id=30012
Product web site: www.sxvm.com
"It's not getting what you want, it's wanting what you've got."
·
It looks like I have sorted my EMI issues out.
1. OSC drive level
I tried to use OSCXT2 but my clock would not start up, but it would start with OSCHS1
So I left it at OSCHS1, originally it was OSCHS3
2. I made my series resistor going to the pin OSC2, 1.5KOhms. (I dont have a 50+Mhz scope but I'm assuming this would make my square wave somewhat rounder.
Notes for nex time:
See what effects a spread spectrum oscillator has although I'm not sure if these work at 5V.
Try and completely understand Bongo's .pdf file
See if I can understand those funky formulas that Paul Baker linked to wrt Trace Termination.
Ooh and about that company that helps with EMI development.
They want $840 per day to use their RF lab. After a day in the Lab they would look at my device and they make some recommendations. Tell me how to redesign it.
Outstanding question:
The appnote AN3EMI.pdf ( SX28AC EMI Evaluation: EMI Results and PCB Design Considerations ) shows a simple board layout on page 8. I'm assuming the 2 squares connected to the resonator is for that 10K series resistor. I think this is the series resistor that bean is referring to in his other post.
What about the external caps ?
What about the series resistor to OSC2 ?
How would u program such a device ?
AFAIK you do not need to disconnect your resonator when programming the SX, right ?
Thanks to all who helped me. (and saved me plenty of $$)
XGen
http://www.elexol.com/Images/EIO24_LARGE1.jpg
If he is selling this device then he should have passed some form of EMI testing I would think.
on my 4-layer boards, the Vdd and Vss pins of the SX are connected to the two inner layers, where one is the Vdd, and the other one the Vss supply layer. IOW, the two inner layers do not contain any signal traces, just two large planes (with holes here and there where signal connections are plated-through from the top to the bottom layer - IOW, the inner layers look a bit like "Swiss Cheese". This means that I do not use separate traces for supplying the SX as the two inner layers build a capacitor coming close to ideal, i.e. having a low "parasitic" inductive component. The Vdd/Vss board connectors are both connected to the associated inner supply layer (with an additional L-C-L EMI filter between the Vdd connector and the supply layer) as are any other component supply pins.
I also have ground planes on the top and bottom layers which each are connected to the inner ground layer with several plated-through connections. I have taken care that the outer ground planes are not used as return paths for the supply currents of any board's components in order to avoid that supply current flows through these ground planes, i.e. component pins that need to be connected to Vss are plated through to the inner Vss plane but are not directly connected to the outer ground planes. So the top and bottom ground planes just act as shields for the embedded signal traces.
During my EMI tests, I never had a problem with noise radiated from any of the signal traces because all of them are switching at relatively low frequencies compared to the clock speed of 50 MHz. Nevertheless, this does not mean that such traces do not generate any radiation because the signal edges are still steep, and therefore can be the source of EMI. So using ground planes as shields on the signal layers makes sense in my opinion. I'm not using any signal trace terminations except the input impedances of the component's inputs driven by SX outputs, and I also have pull-up resistors on the I²C bus lines that connect three different boards. One board with an SX acts as master, another one with a second SX acts as slave, and the third board has a chip card reader installed. I have placed pull-up resistors for SDA and SCL on all three boards, and I'm using a shielded cable for the bus. In addition, on each board (except the one with the chip card reader) I have added L-C-L filters between the SDA and SCL connectors and the board's traces.
In general, I think the major problem is reducing EMI generated from the SX clock and its harmonics. SteveW correctly mentioned that it is best to slow edges down before they become a problem. But the point is that even if the clock signal at the SX OSC1 pin has a nice sine shape, the SX internally will convert it into fast edges superimposed on the supply lines. To my experience, direct radiations from the lines between the OSC pins the resonator, and any resistors around can be held low when the traces are kept as short as possible and when they are embedded between shielding ground planes. A "nice" antenna for direct radiation of the clock signal can also be the 4-pin header for the SX-Key. Therefore, I don't have one on my boards. Instead, I'm using precision sockets (with short pin connectors) for the SX28. So I can program the SXes outside of the boards. In case I want to debug an SX on the boards, I use a "home-brew" adapter socket (you can find a description in one of my very early forum posts).
XGen,
sorry that I did not address your mentioning of spread spectrum oscillators so far. To be honest, I don't have any experience with such devices. I can imagine that they might help to "wipe out" the sharp peaks at 50, 100, 150, etc. MHz while using a fixed-frequency clock device. I.e. you will have many peaks around the center frequency and its harmonics with less energy for each of them - but this is only theory - I don't have any practical experience.
Hey, the URL you have posted showing the SX52 with "miles" of copper between the OSC pins, the resonator, the parallel resitor, and the SK-Key header either indicates that they don't have an EMI approval or that direct radiation from the clock lines is not as critical as we are assuming
Concerning the AN2EMI appnote, the 2 square pads are there for a parallel resistor, not for a series resistor, and the two round pads are there to connect any external shunt capacitors between the two outer resonator pins and ground. You don't need these when using a resonator with internal caps, like the ones sold by Parallax. Note that the plane connected to the SX Vss pin, the resonator and the shunt cap ground pads is not connected to the ground plane on the other side of the PCB. This is because they want to keep the shielding ground plane free of supply current flowind through it. On the other hand, the other planes shown are connected to the bottom ground plane by several vias, so they act as additional shields.
Concerning programming: As long as you only want to program the SX, there is no need to remove the resonator/crystal or any other clock device connected to the OSC1 pin as long as it can stand the higher programming voltage Vpp (about 12 Volts) applied to this pin during programming. On the other hand, when it comes to debugging, the SX-Key must have direct access to the OSC1 pin, i.e. no other clocking device connected. The "default design" provides a jumber that can be pulled to disconnect the clocking device while debugging. As mentioned before, two additional jumper pins, the jumper itself, and the required PCB traces are "nice" little additional antennas, so you should avoid them. Use a debugging adapter instead, and don't care about EMI while debugging. I assume that the SX-Key will generate the "better" signals in this case anyway
BTW: The $840/day for the EMI lab is on one hand a remarkable amount but - on the other hand - compared to the EUR 2,000+/day an EMI lab is charging here in Germany, this is a bargain. So I think, next time, I come to your place, have the tests made there and spend some more fine vacation days.
▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
Greetings from Germany,
Günther
PCB Trace lengths. Guenther (The Master) is correct about lengths being resonant, in adddition to just length, it is a very good idea to make all outputs going to a single area of the PCB (kinda like addressing or controls lines the SAME length, even if it means hand-routing zig-zags to ensure like length. Same true with Inputs. Square waves beginning at about 40MHz can cause harmonics into the GHz!
Highest speed data signals, clocks, oscillators get routed FIRST. DO use ferrite beads in DC power traces, but if possible use a complete ground plane in one layer of the board. In a four layer design, I would recommend top-layer=signals (clocks, oscillators, high speed signals), 2ndlayer=ground. If you have an analog ground for video or A/D use ferrite beads for interconnect on a different layer if possible. 3rdlayer=power. Use plenty of caps as Guenther reccomends hand distributed semi-regularly around the board, and epecially close to high speed edge generators such as the CPU, clock/oscillator, etc. Bottom layer more signals. For an unusually high speed board of any type, especially for Class A FCC testing (I forget the Canadian and Europeans class names), go to 6 layers and use extra ground planes.
Finally, never, ever, ever break the ground plane for purely digital signals, you've just created a slot antenna. I know from experience, that when that happens, a 125MHz FDDI networking adapter first article that costs over $10K to build made a great three room motion detector, but really sucked as a networking card