Need guidelines for making ckt board

Posted: 1/28/2014 7:35:42 PM

From: SE Kansas

Joined: 3/29/2012

I will be building an 'Etherwave' theremin (the circuits from Hot Rodding, Electronic Musician) and will be having a ckt board made, after I design it (the board).  I have had several different boards made in the past for various projects, and am comfortable with that aspect.

I intend to make it a double-sided board, but would like advise on what signals should go on the top side, which on the bottom, or if there would be any restriction.  I don't have an actual 'Etherwave' board, or I would use that as guidance.




Posted: 1/28/2014 8:32:28 PM

From: Eastleigh, Hampshire, U.K. ................................... Fred Mundell. ................................... Electronics Engineer. (Primarily Analogue) .. CV Synths 1974-1980 .. Theremin developer 2007 to present .. soon to be Developing / Trading as . ...................................

Joined: 12/7/2007

Which tracks are "top" or "bottom" is generally irellevant - the only time one may be bothered about this is if there is another board or metal in close proximity.

General rules are the standard ones -

1.) Keep tracks carrying HF as short as you can and as far from other tracks as you can, you want to reduce track inductance and reduce both inductive and capacitive coupling to anything else.

2.) Power / ground rails are extremely important - define a main ground point at the place that ground from the power supply connects to the board, and as much as possible route grounds directly to this point with as few spurs as you can manage - Make ground track thick and short - one REALLY doesnt want any ground track or spur to have any significant inductance or resistance.

3.) You can lay power tracks over ground tracks - capacitive coupling between this is not a problem, in fact it can be beneficial.

4.) Anywhere you have space, add positions for extra decoupling (say 100n ceramic) capacitors between power rails and ground - you may not need to fit these, but have placement for as many as you can - it can be a life saver if you have troublesome noise on the rails.

5.) Think about the function of every track you place - if you can name nets on your schematic, give each net a sensible name so that when laying the board out you can instantly see its function (assuming your PCB editor can do this).. Its only if you think about what the track is carrying, what its impedence is, and things like that, that one can guess about the effect of other tracks close to it or its effect on these - This is where the art and science combine - Only a knowledgable electronics engineer can lay out a really good PCB - but with thought, anyone with reasonable understanding can lay out an acceptable / good PCB.

6.) Auto-routers are hopeless for theremin type boards unless one has a really high end EDA - With a high end EDA one can specify signal types, groupings and other conditional stuff at the schematic design phase, and the autorouter will usually make a reasonable job of applying these - you will still need to polish the layout a bit, but it can speed up the process... But most lower cost autorouters are a waste of time.


Posted: 1/28/2014 9:32:55 PM

From: SE Kansas

Joined: 3/29/2012


Thanks for the pointers.  I feel OK about laying out digital ckts, but this will be my 1st analog board.  We'll just have to see how it works out.




Posted: 1/28/2014 11:19:09 PM

From: Eastleigh, Hampshire, U.K. ................................... Fred Mundell. ................................... Electronics Engineer. (Primarily Analogue) .. CV Synths 1974-1980 .. Theremin developer 2007 to present .. soon to be Developing / Trading as . ...................................

Joined: 12/7/2007

Other things I forgot to mention:

a.) Dont put any ground fill at the RF side - keep this area as clear as possible.

b.) beware of any loops particularly near any inductors.

c.) remember that its not only tracks that radiate or are receptive to radiation / electric / magnetic fields. Even capacitors can couple to adjacent capacitors - and depending on their construction, you can find that if capacitors are close together, the circuit will misbehave - but if you turn either capacitor around it will stop misbehaving - even though there is no identification to indicate which way round the capacitors "should" be !

(it comes down to which leg is connected to the outer foil !) - I am very wary of this after having been bitten by it years ago - now I keep my critical caps away from each other if I can, or place them at right angles to each other.. Only had this problem once, but once was enough! ;-)


Posted: 1/29/2014 4:53:53 PM

From: Austria

Joined: 10/23/2013


" I intend to make it a double-sided board, ....... "

You do not need a double sided pcb. I built two Etherwave Theremins based on two different boards (one on a protype board!). Both with excellent results.

see :


The third one based on the second link obove (with a few modifications on the layout), I will finish next week.

Operating frequencies of the Etherwave are 275 and 450 khz, that is not a really a "High Frequency".

The only thing you should note are the areas of the antenna coils. Bad capacities near the pitch antenna coils could make the Theremin very unlinear.





Posted: 2/14/2014 2:14:20 PM

Joined: 9/30/2012

Hi! Fred, when you say "make ground track thick and short", how thick is acceptable? Is 800mm ok? I guess the same goes for the +/-12V tracks.
And what about the other tracks? About 500mm will do?
The thickness of the track is determined by the passing current or are there more parameters that need to be considered?

Posted: 2/14/2014 4:22:34 PM

From: Eastleigh, Hampshire, U.K. ................................... Fred Mundell. ................................... Electronics Engineer. (Primarily Analogue) .. CV Synths 1974-1980 .. Theremin developer 2007 to present .. soon to be Developing / Trading as . ...................................

Joined: 12/7/2007

Hi Blala,

Ok - 800mm for a track? - in my books 800mm is about the width of the whole board! ;-)

So "The thickness of the track is determined by the passing current or are there more parameters that need to be considered?"

Yes - With low current circuits, its not primarily about current carrying capacity of the track.. its primarily about other factors.. And its real difficult for me to give you any numbers.. Lets look at factors you need to think about (these are not in order of importance):

1.) track has resistance, which causes voltage drop dependent on the current through it - Thicker the track, lower the resistance, lower the Vdrop, changing currents less likely to cause appearance of signals. The lower the current, the less Vdrop.

2.) Inductance (probably a lot more important than resistance for low power HF circuits) - narrower longer tracks have higher inductance than short fat ones - the same kind of effect as resistance, but frequency dependant - so high frequency signals pass through track less easily than low frequency ones.

3.) Capacitance. The fatter a track, and its proximity / overlap area to other tracks, will determine the capacitance between these tracks.

4.) Combined effects of all 3 above, which with HF can result in tuned circuits being created and cause active components like regulators or opamps to oscillate, or can cause HF ringing for fast transients.

In terms of ground and power supplies, these tracks can be laid close together because capacitive coupling is usually advantageous between them. You will be capacitively coupling these tracks anyway..

Because power supplies and ground are capacitively coupled, you regard them all as "ground" from a HF perspective, so you dont want any of these tracks to have capacitive coupling to antenna related circuits - or at least no unintentional coupling.

So, trying to think of numbers.. Just off the top of my head without any science I can quote to justify what I say, for the frequencies and currents in the EW, I would say..

Probably something like 5mm width track for a length of 50mm as a main ground "buss" - double this width for every doubling of length.

If you decouple every supply well (good 100n capacitor at supply points to IC's etc) then power tracks can be half this thickness.

But the trouble is that ive got lazy - I lay my board out instinctively, then if I have any doubts about inductance or whatever on a track, I port the design over to my PCB analysis software which tells me the inductances etc, and I can even insert signals and see radiation / coupling patterns etc.. But I dont do this often..

And in reality, unless one is going to manufacture boards, one can get away with a lot.. Hell, I have even had quick knock-up theremin circuits working on plug-in breadboard (NOT advised).

I tend to over-caution, in the belief that most people will try to get away with less than I suggest, and therebye get it "right" LOL ;-) .. In your case you seem to have done the opposite! I would say that for the EM design no track width above 10mm is probably "needed" and unless your layout is "unusual" 5mm is probably as wide as would ever be "required"... But theres nothing wrong with making power and ground tracks wider IF these dont cause coupling issues to other high impedence tracks carrying signals, particularly HF signals.


Oh - for signal tracks, all the above apply (resistance, inductance, capacitance) but have different trade-offs... One wants low inductance for high frequency signals, and these are the most awkward, because you also want to avoid coupling these signals to other tracks - so best to keep these short and as narrow as possible (within reason) probably 2mm width max, but 1mm or less  is about what I usually use - Audio signals are easy to handle, and short narrow (1mm or less) helps reduce capacitive coupling from HF signals.

But its an art form - all sorts of factors I dont even think of come into play - the angle of the bends on tracks, where one places vias and the relationship of vias to other vias or component pins (you can unintentionally create excessive inductive / capacitive coupling by wrongly placing vias and the tracks connecting these - effectively creating a "turn" or loop through the PCB) .. And I am by no means an artistic pro PCB designer - good analogue PCB design (as opposed to autorouter churned out digital board design) is an awesome feat IMO, as it combines good understanding of the circuit with art and incredible patience.

"You do not need a double sided pcb." - Betabox

Absolutely true! The main advantage of double sided is its easier to do a layout quickly, and it (often) enables smaller board size - And double sided is probably essential for all but the simplest SMD design... But for something like an EW board, no real need for DS.

If one is getting boards made by a Fab, there isnt any real price difference between SS and DS, so its worth doing a DS design - I often lay my DS board out as if its SS, with only straight tracks (links) on the component side - this allows me to etch my own SS prototype board and easily fit the links to replace the tracks on the component side, but then (after the board is proven) send the DS layout for manufacture so I then dont need to fit the (often extensive) links.

Posted: 2/14/2014 7:54:53 PM

Joined: 9/30/2012

Fred, thank you for your detailed answer, much appreciated! :)

Although, a noob and silly i guess question: HF circuit means high frequency circuit?

"Ok - 800mm for a track? - in my books 800mm is about the width of the whole board! ;-)" - wasn't thinking at all when i wrote that!


That's my first PCB, and i know basic things about electronics, so problems and questions come up all the time, at every step. I have just finished routing, with the layout shown in the "Hot-rodding your Etherwave Theremin" pdf, but i have no idea if my vias will create problems, or if my tracks are well placed. I selected 1.250mm track width for the ground and power tracks, and 0.7mm for all the other tracks. (i used KiCad)


Here is a photo:


I would really like some feedback on this :)

Posted: 2/14/2014 8:52:31 PM

From: Eastleigh, Hampshire, U.K. ................................... Fred Mundell. ................................... Electronics Engineer. (Primarily Analogue) .. CV Synths 1974-1980 .. Theremin developer 2007 to present .. soon to be Developing / Trading as . ...................................

Joined: 12/7/2007

Hi Blala,

Yeah, HF is High frequency .. To be honest, when I first came to TW I was arrogantly saying that the frequencies in theremins were so low they shouldnt be called "RF" or even "HF" - But I was wrong! ;-)

I looked at your layout - not closely, but...

I suggest you look at Bitbox layout -  personally, I would have made the ground tracks a bit thicker in places on his layout, but thats just me.. He has his EW working without problems, and thats worth more than a bunch of theory!!

In particular, your routing 'round the variable inductors and HF end of the circuit doesnt look ideal - you want tracks here short and tidy - and in this area Bitbox has done the job far better IMO... I am NOT saying your layout wont work - it may work well..

Apart from which, its always good if you have the chance to see how someone else lays out a circuit you have also done a layout for - you see things you never thought of. I do not regard myself as a PCB designer - given the choice of designing a board or copying one, I certainly choose the latter! ;-) But many times I have been required to get a dysfunctional layout operational - and often its easier to take the existing layout and change it a bit than to redesign the whole board..

Im sure there must be quite a number of EW clone board designs on the web by now - find as many as you can, and use the ideas to produce your own - or just pick the tidiest and copy it!

@betabox - You do exactly what I do in terms of using DS and laying the board out for straight links so it works as a SS board! - I have no problem making my own DS boards, but its the through-hole plating thats the problem - its actually easier to insert links than to try to get traces to connect from top to bottom I find.

Oh - one other thing - I tend to connect ground to my inductor cans - I dont like leaving anything "floating" unless I absolutely must.


Posted: 2/15/2014 6:02:16 PM

Joined: 9/30/2012

So, just finished routing the layout posted in the topic "My Etherwave PCB" from wannes dn, with some minor, i hope, changes. I used the front side of the board for the "jumps" that he has and i also added the buffer stage that i saw in other topics near the 10-pin connector. I will also have the antenna circuits on separate pcbs.

But i have a question: What is the purpose of the track leaving from the right end of R16 (just above Q8, at the left part of the pcb) leading to a pad that is not connected anywhere?

There is another not connected pad coming from R8 (above the 10-pin connector), but i guess that goes at the pad on the track connecting C18 and R15 (ground)? Is it really necessary since C18, R15 and all the other parts on that side, that need to be grounded are already grounded?


wannes_dn's pcb:
(the updated pcb that he posts a bit later has some extra parts [ ] what are they? )

my pcb:
(i will redesign the power supply circuit according to betabox's pcb)

You must be logged in to post a reply. Please log in or register for a new account.