distance from Propeller to crystal?

tad4shi

Hey everyone,
what should be the maximum distance from the crystal to the Propeller chip?
is a few inches okay?

Thanks!

kwinn

tad4shi wrote: »

Hey everyone,
what should be the maximum distance from the crystal to the Propeller chip?
is a few inches okay?

Thanks!

Probably not! The further away the more likely you are to have problems. I would never place a crystal more than an inch from the oscillator pins on any board I design, and normally place it closer than that. If space is a problem I would place a remote oscillator on the board and feed the clock signal to Xin of the Prop chip.

Mike Green

Have a look at the pictures of the various Propeller boards that Parallax sells. You'll notice that the crystal is always mounted adjacent to the Propeller chip. More than about an inch and you'll have problems with noise and the extra lead length will increase the capacitance to ground and in parallel with the crystal which will shift the frequency of oscillation and increase the loading on the crystal, maybe preventing oscillation.

jmg

tad4shi wrote: »

what should be the maximum distance from the crystal to the Propeller chip?
is a few inches okay?

Define 'a few inches' ?
Why do you need to have a large spacing ?

There are smaller Xtals available, Digikey show a clock-cylinder in 5MHz and also a SMD one at (8.00mm x 4.50mm)
Or you can use a smaller resonator - not quite as precise as a xtal, but comes (4.50mm x 2.00mm x 1.19mm H)
Or, you can use an oscillator - slightly more cost, but that can place further away, & they come as small as (1.60mm x 1.20mm)

DigitalBob

On my board layouts I go 0.200" (almost 1/4" or about 5 mm for you metric heads) from the prop pins and never had any issues. I never had a reason to go any further. with a 5mhz crystal

Phil Pilgrim (PhiPi)

Close proximal location of the crystal to the Propeller is a given. Don't mess with it.

-Phil

Peter Jakacki

Keep it tight and clean, don't cross over or run other signals with these lines, especially the crystal input since it is such a weak signal and any bit of noise that get's injected into that input will destabilize the whole chip. If possible have a ground plane around and under the crystal. There are many styles to choose from and the old HC49, even the 1/4 height is, well old. I have used compact cylindrical crystals, either 6MHz or 10MHz and since the leads are so close together it is easy to route this on the board.

btw, I took a screenshot for the layout on one of my older pcbs that uses this kind of crystal. Even though the Prop is SMD, it gives you an idea.

CtlAltDel

Hmm...I think I see a couple of areas of dead copper on that PCB, Peter

Peter Jakacki

CtlAltDel wrote: »

Hmm...I think I see a couple of areas of dead copper on that PCB, Peter

Yes, so did I when I did the screenshot. Not sure why as I normally have "remove dead copper" option ticked!
I still had some leftovers of that version and checked them but they were ok, so I guess I used a bad version of the artwork, in fact as I just checked it the ground plane wasn't assigned to a net for some reason. Forcing it to ground and re-pouring fixed it. But obviously, that wasn't the same artwork that was used for the pcb.

Tracy Allen

The xtal pins sit between two power pins on the Q44 package. So, which do you keep closest to the chip, the bypass cap or the xtal? I use a layout with a 1206, 10µF cap close in, and a 7x5mm 5MHz xtal next out, as seen in the screen shot. The other 3 bypass capacitors for the Prop are standard 0.1µF. The main thing, again, is to keep the xtal leads short and shielded from noise, but also you don't want to add a lot of extra capacitance. The Prop is supposed to take an 18 or 20pF crystal.

Mark_T

I'd suggest putting the decoupling caps on the underside, reduces cross talk between all power/ground pins and all
signal lines, and frees up board real estate topside... I tend to use 1206 components underside, usually just decoupling
caps, and hand-solder them after doing the topside in the oven.

I've also put the xtal on the underside to allow all 32 signal pins to be laid out tightly topside.

Phil Pilgrim (PhiPi)

Mark_T wrote:

I'd suggest putting the decoupling caps on the underside, reduces cross talk ...

That all depends upon the board's objective. If it's to be mass produced, put all of your SMD components on one side to reduce assembly costs.

Also, I regularly hand-solder 0603 resistors -- no problem (and I'm pushing 70 and near-sighted). 1206s are huge! The trick is to tin one pad, to adhere the part (held by tweezers) to that pad with heat, then to solder the other pad.

-Phil

Cluso99

On my Prop boards I put the prop and microSD on the top. All other parts are on the bottom - bypass caps (0603 and 0402), regulator (sot23), xtal (3225), reset resistor (sot229? It's smaller than the sot23).
I have no problem hand soldering although the 0403s are really pushing the envelope. But mostly I use an IR oven - I know that's cheating
My biggest problem is hand placing. At 66 my hands slake a little so I have to stop breathing for placement
I do the underside first - I make these in larger lots. The tops I do in lower volumes as that is the expensive part. As my oven is temp controlled quite well, by placing the boards on a larger old bare pcb wrapped in tinfoil, this prevents the soldered underside from heating too much to let the components move.
OSHstencils make good cheap Mylar stencils for the solder paste.

Oh! By using 0.020" via holes for the xtal on the pcb underside, those holes can be used to fit a watch can xtal instead in the via holes.

Beau Schwabe

If you are SYNCing more than one Propeller, the distance can be much further up to a foot or more... See thread below about half way down.

https://forums.parallax.com/discussion/98874/propeller-demo-syncing-multiple-cogs-together-and-syncing-multiple-propell

quickengprojects

It depends on the nature of your project and space limitations. It is preferred to put a distance not more than one inch. However, if budget is no problem for you, you can buy oscillator that comes with high accuracy and precision.

Mark_T

You can't really hand solder 0603's without have a ultrafine bit, which means either changing iron bits or
having two irons - I can't be bothered with that! 1206 is convenient to have as you can route a trace under
a 1206, and you can have bulk decoupling in that size too. 1206 is also convenient for working directly on
strip-board.

For toaster-oven use I tend to stick with 0805, just easier to work with. I found out the hard way that
0603 LEDs don't seem to have polarity markings on them, which meant making a jig for working out
which way round they were!

Tracy Allen

I've sometimes put components both passive and active on both sides, but lately I've tried to keep the SMT on one side, yes, for reduced assembly costs.

About bypass capacitors on the opposite side though, I've seen analysis and experiments which suggest that vias are relatively high impedance paths. Other things being equal, the capacitor next to the Vss/Vdd pins on the same side as the CPU will better suppress dips and ringing on the power supplies than a capacitor on the bottom that has to support currents through a via. Also, SMT components on the bottom break up the ground plane. The ground plane is best when it is continuous, except for strategic breaks and a minimum of bottom traces.

The crystal voltages and currents are quasi sine waveforms. I believe that means that the crystal can be a little further away than the bypass, which has to supply sub-nanosecond level demands.

scope shot: red=xtal input, yellow=xtal output.