critique request - draft PCB for MILA tube pre

I'm building a dual channel MILA in a shallow 2U unit and need it compact so I've drawn a PCB. This is only my second attampt at PCB design and my first involving valves, so I'd really appreciate any pointers where I might have gone wrong (ie: potential sources of noise)

- Super simple layout because I really suck at etching boards.
- Ground pour everywhere. Is that a good thing?  ???
- The footprint of components is either taken from measurements of parts I have, or from the datasheets. All resistors are Dale 1/2W, the 1uF and 4.7uF caps are Solen 630V
- Pads are provided for heater wires, but the intention is that the heater wires would be a twisted pair run under the board and as far away from the board as possible. Heaters can be powered by 6.3v, 12.6v, AC or DC.

Schematic: http://musiciansgig.com/mila/MILA1-Updated.pdf

Note: This initial design is provided for feedback purposes only. It is not to scale and has not been built.





Thanks for any tips  

Since you'll be yanking tubes in and out you might want to consider adding extra physical support.

You should add a fifth support screw in the middle of the board, between the tubes. Maybe under that 270 resistor, or near the 1M resistors left side. With only a few tube changes and a little bad luck, you'll be otherwise damaging the PCB.

Another tweak, you can actually squeeze that bottom left screw in the actual corner with slight shift of those range connectors.

Did you know you can connect those bigger molex screw terminals together? That way you could have a 4-way connector for the range (instead of two side by side) and more physical support as well. Same could be done for 5-way molex for the input trafo/DI area (instead of 3-way and 2-way side by side).

+1 for more screws, placed in strategic positions

the way I see it, you should put screws physically close to the molex-es, make it three screws (one in the middle of the molex strring), so that the board is firmly held in place and won't bend if you mess with _cables_ in your box (when built) if you are tweaking something...

the other thing is: I would use fatter traces for the ground/masse (around molexes you thin it down considerably).

Thank you both very much for your advice. I will take it on board and post a revised layout tomorrow.

Disclaimer: I don't have all that much experience in audio tube circuitry; most of the tube work I've done was for RF systems. Having said that...

andrew_k said:

- Ground pour everywhere. Is that a good thing?

Click to expand...

In this case, probably not.

First, you've got a couple of ground loops. How much of a real problem that is remains to be seen, but if you can avoid them in the design stage it's best to do so. Second, ground fill makes for parasitic capacitive coupling to other traces and to components, and you usually don't want that. I'd be especially careful in keeping ground away from the grid connections and the snubber resistors (R6/10/14/15 in NYD's schematic). Finally, you have pretty high voltages on what I suspect will be an uncoated home-etched board, and while the clearance between B+ et al and ground looks like it complies with the official standards (IPC-2221), your boards will probably have more contamination than the standard tables account for. While it might be overkill I'd try to keep at least ~1cm between B+ (including the plate connections) and everything else, especially stuff that's connected to the outside world. (Have a look here for more on this subject).

As for the rest of the board:

- the power resistors (R17/22) will get warm to hot, capacitor life is inversely proportional to temperature. Keep them separated if you can; especially in the top right of your board the caps are closer to the resistors than I'd like.

- you can get the board a bit tighter if you sit down and play with parts placement a bit more. F'r example, by flipping the gain connector around you can eliminate that wire bridge in the top left. (The idea is to get the design tight enough to keep it from turning into a radio receiver while not being so tight that it turns into a radio transmitter).

- consider your power distribution, especially ground current flow. This may be the RF engineer in me speaking, but if you can't star ground everything then at least minimize the distance between the ground ends of those supply decoupling caps and the relevant cathode networks. I'm particularly thinking about C9/R7 here; there's quite a bit of (inductive) ground trace between the two on your board.

- others who are more in the know may want to correct me here, but I believe that depending on transformer and off-board wiring that Zobel (R4/C1) will do more good when it's mounted directly at the transformer.

And to answer the question that you didn't ask: the MILA looks like it's begging to be P2Ped. Mount the tubes on an aluminium L- or U-profile, and wire up the parts directly to the tube sockets and a bit of terminal strip. Alternatively use a terminal board. While PCBs are nice if you need to make a few dozen that are exactly the same, a P2P construction is much easier to modify if it turns out that you've built an AM radio transmitter.

JDB.

Wow. I've just read your post three times to try and make sure I don't miss anything. I'm not going to pretend I understand it all, because I don't, but I certainly want to 
I have saved the article on Circuit Separation and will read it on my train journey to work in the morning.

The primary thing I'm struggling to grasp is where the ground loops are. My only valve experience prior to this is scratch-building a few guitar amps on eyelet boards or tag strips, and in those cases grounding has been easy as I've always used a fat bus wire and laid out the components as much like the schematic as feasible. The only reason I have started on a PCB is that I need it as compact as possible to fit two into my existing case along with PSU and a pair of VU buffers. I really should have bought a deeper case but I got what I could afford and I have to make the best of what I've got. Also, the oft-referenced MILA turret layout didn't appeal to me due to the orientation of the controls (I need a long thin board with pots at front) and other less important factors. Similarly the L-bracket approach is something I considered as I have some salvaged shielded noval sockets on brackets, but again I ran out of room when trying to fit everything comfortably in the case. One option I haven't fully investigated is punching socket holes in the back panel of the case and mounting them there.. I will take some measurements tomorrow to see if that's a viable alternative. I would certainly feel more confident building on tag strips or turret board.

Back to the ground loops... I infer from your post that the loops are where ground points early in the circuit are next to ground points form much later, or in the case of C9+R7, ground points that should be adjacent are separated?  My unschooled eye sees it all as one big blob of ground on a circuit board, whereas in guitar effects and the sort of simple devices I usually build I can clearly see when ground to a component is being fed from multiple locations.

Thank you for taking the time to write such a thorough response 

While designing the PCB will be a rewarding experience, I would still personally go for a p2p turret layout with a fat copper group bar with MILA, for noise performance reasons. I have actually done this with great success. I made my own layout because I wanted some customisations and a better ground implementation. I could post the layout here if you're interested.

You mention you have 2U case. Even if it's not deep enough for more conventional turret positioning, it still means you have "two levels" of space for use with turret layouts. You can mount the tubes on top of transformers or the turret board (with custom L-brackets). Lots of options here.

One can actually design a PCB with a "ground buss wire" (a large diameter bare copper bus wire) or a copper bar for the sensitive "signal ground". There are tricks to use best of both worlds.

Some examples of technique can be seen in jeff Rowland amps, but not for ground afaik.

Kingston said:

I made my own layout because I wanted some customisations and a better ground implementation. I could post the layout here if you're interested.

Click to expand...

I have interest in seeing this, you could email it to me and I can store it on my server.

Thanks

Matt

Kingston said:

While designing the PCB will be a rewarding experience, I would still personally go for a p2p turret layout with a fat copper group bar with MILA, for noise performance reasons.

Click to expand...

I'm leaning towards this option following the responses in this thread. Better the devil you know 

I have actually done this with great success. I made my own layout because I wanted some customisations and a better ground implementation. I could post the layout here if you're interested.

Click to expand...

Yes please! I had started on my own prior to the PCB layout, but wasn't very happy with it.

You mention you have 2U case. Even if it's not deep enough for more conventional turret positioning, it still means you have "two levels" of space for use with turret layouts. You can mount the tubes on top of transformers or the turret board (with custom L-brackets). Lots of options here.

Click to expand...

Hmm. Very interesting. Thank you. I will get out all the major components and a ruler on the weekend to further explore my options

tv said:

One can actually design a PCB with a "ground buss wire" (a large diameter bare copper bus wire) or a copper bar for the sensitive "signal ground". There are tricks to use best of both worlds.

Click to expand...

Yes, I had briefly considered that last night, glad to see it's not an entirely crazy idea. Perhaps even the unconventional option of running the ground bus horizontally up the middle of the board to allow maximum access for grounded components...

Lots to read, think about, and try out. Thank you!

not as pretty as your version, but look at the differences to see where your ground loops were...  basically you only want your ground plane to go where it is needed, and not make any loops.  i'm sure there's still room for improvement, but just a quick mod to illustrate the concept.

ed

Excellent, thank you Ed. That's much easier to analyze than pure theory.

Regardless of whether I persevere with building the PCB or revert to a tagstrip/P2P layout, I will do a revision attempting to incorporate all the great suggestions in this thread.

Version 1.1



Changelog:

• Ground loops addressed (hopefully!)
• Zobel network moved off-board; to be attached to IN_TX secondary
• IN_TX 1 connection to jack 1 switch moved off-board
• Gain control traces re-routed to avoid need for jumper
• Multiple mounting holes added for better support when replacing valves
• More space cleared around components prior to first gain stage in an attempt to reduce the chance of interference
• More space around B+ traces and power resistors

One piece of advice I couldn't implement was getting the ground point for the first triode's cathode resistor closer to the ground for the smoothing cap. Not sure what, if anything, to do about that in the layout's current state  ???
Admittedly I'm tempted to add a pad next to the filter cap's ground and a pad next to the cathode resistor and just run an off-board wire between the two. That seems like a nasty hack to me, but at least it gets the cathode resistor away from the input trafo's ground..

Some wanted to see the p2p turret board layout I mentioned earlier. I had to clean it up since I originally made it to be a mere drilling guide (those red dots).

Now the actual connections and part numbers are visible, but it's not a document which I would call graphically rich, and it might be confusing. But then, if you're implementing any of this you'll have to fit your part sizes there. It's going to need some finetuning whatever the case.

The mirrored layout is exactly like I did my two channels. I reference ground to chassis at one single point and nowhere else: at first PSU filtering cap. Some experimentation is needed here. Maybe you want to connect XLR pin1's here, maybe you don't.

It isn't visible in the layout drawing, but please, shield all your wires everywhere and TOO MUCH. If you're not sure about it, shield some more! There are plenty of shielding points to grab on that fat ground bar. Best be safe than sorry.

http://www.michaelkingston.fi/files/mila-1_turret_layout_kingston.pdf

And then eventually you'll have a tube preamp with -80-90dB hum at max gain (a ridiculous 60-70dB of gain depending on your input tx). Which means that most of the time you'll have all the noise well below -100dB.

By the way I built a super simple CRC supply like in NYD schematic for a two-bottle preamp years a go, but couldn't make it free of ripple. I used a more Gyraf G9 like regulated supply on this one instead.

Great, thanks for sharing that.
I like the idea of mirroring the layout for dual channels, I think I'll borrow that one 

Kingston, I've made some minor adaptations to your layout to suit my parts and have a brief question about grounding -

http://notinteractive.com/stuff/audio/mila/mila-dual-layout_0.1.png

Thinking of ground currents, should the ground bus be split for the two channels with each channel leading from input to star ground, as I've done?

I think your ground flow is fine, but only in real life test will you know for sure. In this one, yes it needs to be split in the middle.

But why did you change it? now you have two ground references from the two channels, two wires. If you don't split in the middle and take your two busses to chassis from there, you only need one, and flow is more like in the schematic (which is already tested and proven extremely quiet).

[edit]

also, R13, R16 C5 group is missing connection to ground

Kingston said:

But why did you change it?

Click to expand...

Only because I'm used to grounding the bus at the input end in guitar amps. I accidentally overlooked your B- reference in your drawing and for some reason thought you were grounding from the input end of channel 1. I will change it to ground from the middle.

Thanks again 

Hi andrew_k,

Any update on your project? I am doing my version of a Mila pcb.
Kingston and craptical and others helped me complete a turrent version
(very sturdy).
I had to clean up the wiring and use shielding to get it quiet but it sounds
great now. I read pcbs are not the best for this type of project but I want to try
and see if I can etch one and see the results. My pcb is 2.75" by 8". My component layout is similiar to my turrent board version. I am going to place the tubes on a separate custom metal bracket. I might need to space the pads a little. How big should the traces be for the B+ and B-?
Anyway update when you can.
Good info on this thread...

PJ

I abandoned my PCB design because everything was going to be too cramped and I was fearful of noise due to squishing the PSU next to the preamps.
I moved to an external power supply and adapted Kingston's turretboard layout to suit my needs

http://notinteractive.com/stuff/audio/mila/mila-dual-layout_0.2.png

Sorry I can't help with your question about trace thickness, I don't have any experience or training to base an answer on  ???