PCB Draft (still new at this)

Help Support GroupDIY:

BluegrassDan

Well-known member
Joined
Mar 16, 2009
Messages
478
Location
Elizabethton, TN
Howdy everyone,

My soldering iron stayed cold during covid, but I'm now back to tinkering around. Putting my preamp and EQ onto a PCB has been a tall drink of water for me.

You'll notice the signal starts on the left and follows a U shape counterclockwise. I'm worried that this looks too sloppy.

Two questions:

1. How does this look so far? (From a general bird's eye view.)
2. Should I abandon this approach for a full ground plane, a few ground pours, and/or more than two layers?

Thanks in advance!
 

Attachments

  • Audio-Board-V1.jpg
    Audio-Board-V1.jpg
    135.2 KB · Views: 70

totoxraymond

Well-known member
Joined
Oct 25, 2013
Messages
132
Location
Paris - France
Hi,

I'm not fan expert at all in pcb design or tube builds, but after reading sime recent posts about hum problems, i figured heaters traces on pcb aren't a good thing. They will cause hum even with DC.

If i understood correctly, you'd be better usign twisted cables. This way you can run them away from yourr signal traces and reduce the hum.

Thinking of it, it's what has been done in all the tube amps i repaired.

But somebody more skilled than me might tell you otherwise.

Cheers,

Thomas
 

MidnightArrakis

Well-known member
Joined
Sep 25, 2015
Messages
80
Howdy everyone,

My soldering iron stayed cold during covid, but I'm now back to tinkering around. Putting my preamp and EQ onto a PCB has been a tall drink of water for me.

You'll notice the signal starts on the left and follows a U shape counterclockwise. I'm worried that this looks too sloppy.

Two questions:

1. How does this look so far? (From a general bird's eye view.)
2. Should I abandon this approach for a full ground plane, a few ground pours, and/or more than two layers?

Thanks in advance!
Dan: I'm just a "beginner" in the area of PCB design (see attached PDF file), but I think I can offer you some assistance.
  • TOPSIDE ROUTES = RED
  • BOTTOMSIDE ROUTES = BLUE
  • TOPSIDE SILKSCREEN = WHITE
  • BOTTOMSIDE SILKSCREEN = CYAN
  • TOPSIDE SOLDERMASK = BRIGHT (or, LIGHT) GREEN
  • BOTTOMSIDE SOLDERMASK = DARK GREEN

  • It looks as though the drill holes for your tubes are slots. If they are, that's gonna cost you plenty!!!
  • Your routing has several "acute angles", which are known as "acid traps" and those will cause your routes to loosen off of the PCB.
  • It looks as though the spacing between two routes is too small in places (what is the routing DRC setting)?
  • In what looks to be "C3" (small part up by "Audio In"), the two pads look to be shorted together by a RED trace. Is that supposed to be like that?
I am assuming that your PCB program is either EAGLE or KiCAD since those are the dominant FREE programs that everyone is using these days. If so, send me your actual CAD PCB layout file, as my PCB design program can import both of those files. Then, I will be able to take a better look at your layout and also be able to offer you some better suggestions.

While 4-layer boards are more expensive than your run-of-the-mill 2-layer boards, these days the cost difference isn't as much as it used to be. I have been thinking of re-designing a vacuum-tube radio transmitter and putting its filament DC voltage on the inner-layers like how you had mentioned. In thinking about it further, it may possibly even require a 6-layer board: L1 - TOPSIDE ROUTES, L2 - GND PLANE SHIELD, L3 - Filament-1, L4 - Filament-2, L5 - GND PLANE SHIELD, L6 - BOTTOMSIDE ROUTES. So, as you can see, the two GND PLANE SHIELD layers surround the two FILAMENT layers and act as a shield for the two outer routing layers. Just a thought.

What you are calling "Ground Pours" is commonly referred to as "Copper Pours" and in general, they are always a good thing. > BUT!!! < there is more to it than just flooding an area with copper!!! 1) The "Copper Pour" has to be connected to GND, 2) The "Copper Pours" on both sides of the board need to be connected to one another!!! YIKES!!! How do you do THAT??? Well.....doing that requires a boatload of what are called "stitching vias". What are "stitching vias"? "Stitching Vias" are independent vias that are connected to GND (or, whatever NET NAME your "Copper Pours" are connected to) and they need to be placed in such a manner as to connect a TOPSIDE COPPER POUR and a BOTTOMSIDE COPPER POUR together.

And, by my using the term "boatload", I mean "TONS" of them!!! You need to think of each via as being a teeny-tiny resistor and by having lots and lots of vias placed within a "COPPER POUR", which is effectively the same thing as having gobs of resistors in parallel. And, what happens when you have resistors in parallel? The overall resistance is reduced. So....."The More The Merrier" when it comes to "Stitching Vias" that are placed within "Copper Pours". And, since the "Stitching Vias" are only vias within a "COPPER POUR", the drill size and via pad can be much smaller than a component pad. You could use a drill size of 10-mil with a 14-mil pad (which will give you a 2-mil annular ring) because the via is embedded within a "COPPER POUR".

In any case.....I could give you a much better assessment if I had your actual PCB layout file. I tried enlarging your image file and after a bit, it just became too fuzzy to easily read anything. Your call.....

/
 

Attachments

  • JBW-Designed -- Various PCB Designs - 2D & 3D.pdf
    2.5 MB · Views: 34

abbey road d enfer

Well-known member
Moderator
Joined
Jan 22, 2008
Messages
12,661
Location
Marcelland
1. How does this look so far? (From a general bird's eye view.)
IMO you have concentrated on making a well organized layout, with resistor aligned like tin soldiers. If it was me, I would have a less neat arrangement with components laid out in a manner that optimizes trace length, at the detriment of looks.
 

MidnightArrakis

Well-known member
Joined
Sep 25, 2015
Messages
80
In my assuming that you are using PCB-mount tube sockets and that the tube sockets have rectangular PC-pins, you still want to use a circular drill hole in your board to fit the tube socket pins into. If what I am seeing in your PCB image file are truly slots, the PCB fabrication shop is going to charge you plenty to create that many tiny slots, especially at the circular angles that they are all at. "Circular Holes" are what you want to use, NOT slots.

How do you determine what size hole will fit a rectangular shape? First, calculate the "Diagonal Cross-Section of a Rectangle". As an example, I have a 9-pin tube socket right here with me. The PCB-pins measure 13-mils thick by 50-mils wide. So, you would need to calculate what the "Diagonal Cross-Section" of that rectangle is. Second, then add - 10-mils - for some clearance. That will determine your drill size.

Then, you will need to determine how large your component pin-pad size will be. This will be primarily determined by how close your pin-to-pin spacing is and how much "annular ring" you wish to have. If you are going to have your PCBs wave-soldered, you can get away with a 10-mil annular ring. But, if you are going hand-solder your PCBs, then you'll probably want an annular ring between 25-mils to 40-mils, depending upon the space available. Plus, don't forget to oversize your solder-mask reliefs by 5-mils. If your solder-mask pads are the same size as your component pads, you run the risk of there being some solder-mask over your pads should there be a layer misregistration during the fabrication process.

Again.....I could provide you with a much better analysis and assessment if I had your actual PCB design file.

GOOD LUCK!!!

/
 

MidnightArrakis

Well-known member
Joined
Sep 25, 2015
Messages
80
When I wrote my last response to you, I forgot to include one additional piece of information that is rather crucial with obtaining your drill size. When I wrote "First, calculate the "Diagonal Cross-Section of a Rectangle". Second, then add - 10-mils - for some clearance. That will determine your drill size".....there is one more final step in determining your final drill size.

- AFTER - you have completed the 2 steps above, you then need to have an actual "Drill Size Chart" available. Simply take whatever number you came up with after your calculation PLUS the additional 10-mils and then - ROUND-UP - that number to the next nearest size shown on the "Drill Size Chart". THEN.....you will have your actual drill size for your tube socket pins.

Since I do all of these things automatically without having to think about them, it's easy to not include something when relating these steps to someone else who has never done this before. I apologize for my forgetting to include this final step earlier and I hope this information proves itself useful to you.

/
 

Bo Deadly

Well-known member
Joined
Dec 22, 2015
Messages
2,524
Location
New Jersey, USA
IMO you have concentrated on making a well organized layout, with resistor aligned like tin soldiers.

I don't see that at all. The board looks just fine to me and I'm super picky. Resistors and capacitors have a tendency to line up like that especially when switching over a sequence of parts. I don't see a lot of traces crossing over unnecessarily and where they do cross over they're not parallel.

I would definitely do a ground plane though. When I do a layout, I start with a ground plane and try to ignore the ground wires. After getting a few of the major traces routed, I actually ratsnest the ground plane to get rid of the air wires so that I can see what's what better. At the very end I also add a top ground plane (just because you can and it's less of a burden on the manufacturer but mostly because it helps keep the board from warping) and a bunch of vias all around to connect them.

I don't do tubes but I think DC heater lines would be just fine (except maybe one trace next to V4 running parallel to one of the heater lines). The parallel routing looks good too just in case there's a little AC. Maybe add some 0.1uF ceramics at the pins? But definitely don't use the 0V ground plane.
 

abbey road d enfer

Well-known member
Moderator
Joined
Jan 22, 2008
Messages
12,661
Location
Marcelland
I don't see that at all. The board looks just fine to me and I'm super picky. Resistors and capacitors have a tendency to line up like that especially when switching over a sequence of parts.
I'm not "super picky", but part of the art of good PCB design consists in moving components, no matter how they appear in the netlist, until some result is achieved. Minimizing trace length is generally a good choice, along with minimizing capacitive coupling between antagonizing traces.
I would have moved the tubes so that more space was left on the side of the PCB.
Putting all the related components on the same side of a dual triode is looking for trouble.
 

BluegrassDan

Well-known member
Joined
Mar 16, 2009
Messages
478
Location
Elizabethton, TN
Thanks for all the detailed responses, especially Midnight. Attached is a new screenshot.
  • Top (red) layer is now ground plane. Bottom layer (green) traces.
  • By using a ground plane more traces could be shifted from top to bottom.
  • I nudged the layout to make sure traces were as direct as possible with fewer sharp corners.
  • Added a series of signal ground vias across longer top layer traces.
  • I never have liked those PCB mount tube sockets, so I converted them to a standard chassis mount that will be hard wires to pin-corresponding pads.
  • Traces = Heaters 100 mil, B+ 50 mil, audio 30 mil.
  • Vias = 30 mil drill holes, 60 mil vias
  • Clearances = Ground plane 30 mils, traces 7.87 mils (default)
I moved the input transformer off the board so it can live near the front panel.

Again, I appreciate everyone's good advice. I'm used to turret boards and point-to-point stuff.
 

Attachments

  • Board-with-ground-plane.jpg
    Board-with-ground-plane.jpg
    205.4 KB · Views: 29

Bo Deadly

Well-known member
Joined
Dec 22, 2015
Messages
2,524
Location
New Jersey, USA
I would have moved the tubes so that more space was left on the side of the PCB.
Putting all the related components on the same side of a dual triode is looking for trouble.

Fair enough. With the impedances used by tube gear, the length of traces and capacitive coupling effects are much more important. So in general I would agree that the board is could be a little bigger so parts have the space to intersect with one another better and then the high impedance / high gain nets can be shorter.
 

Winston OBoogie

Well-known member
Joined
Jun 3, 2004
Messages
2,543
Location
UK.
I'm probably just too old fashioned, but I don't use ground plane's or pours for discrete analogue circuits. The one time I did, which was for a commercial product, is the only time I got some noisy current dumps into my audio.

Maybe I just don't know how to do ground plane's right, but I just lay things out as if I were building point-to-point.

Ground follows signal, each stage has its respective decoupling capacitor connected to that stage's ground point, get that current loop around the active device as small as possible, but don't go crazy, leave enough space for dissipation etc. if it's tube...

Then signal goes onto the next stage, rinse and repeat.

P.S. Good placement of components always takes takes precedence over appearance. Any art in the thing comes from a good layout not in how it might look on the wall. (that dig wasn't aimed at your layout Dan :) )
Pick and place machines don't like diagonally placed parts but, damn the torpedos, if that's a better placement I'm doin' it.
 
Last edited:

abbey road d enfer

Well-known member
Moderator
Joined
Jan 22, 2008
Messages
12,661
Location
Marcelland
An indiscriminate copper-pour is not a proper ground plane. RF ground planes are elactrostatic shields and waveguides.
Audio ground planes are part electrostatic shielding, part ground trace reinforcement. As such, it must operate as a reinforcement of the existing ground traces, that are supposed to be laid in accordance with "ground follows signal". For proper performance, a ground plane often must be segmented, in order to separate nodes that should not meet.
The typical beginner's mistake is, after producing a good lay-out that works flawlessly, decides to improve and does a copper pour, that connects the reservoir caps ground to the other sensitive grounds. The ground plane must not comprise the capacitors ground, nor the mains xfmr CT. It should leave the return of a significant load alone, too.
Eagle, which is the only PCB package I know well enough, allows drawing the contours of multiple ground planes, but I think all decent software packages offer that possibility.
 

Winston OBoogie

Well-known member
Joined
Jun 3, 2004
Messages
2,543
Location
UK.
Good stuff. You're absolutely spot on.

after producing a good lay-out that works flawlessly, decides to improve and does a copper pour, that connects the reservoir caps ground to the other sensitive grounds.

But that bit where it works flawlessly is where I stop.

Nothing I do now requires further assistance. I'd probably hand over anything that did to someone like yourself.

My default pcb package used to be Protel but I'm now on Mac so, anything decent that's free is a winner.
 

Matador

Well-known member
Joined
Feb 25, 2011
Messages
2,061
Location
Bay Area, California
ff
Thanks for all the detailed responses, especially Midnight. Attached is a new screenshot.
  • I never have liked those PCB mount tube sockets, so I converted them to a standard chassis mount that will be hard wires to pin-corresponding pads.
  • Clearances = Ground plane 30 mils, traces 7.87 mils (default)
If your sockets are off board, you don't need the large circular tube layouts...in fact, you don't even need the traces running to them: you can just wire directly from the source of those traces and go to the sockets.

When I do tube PCB's that send wires to remote tube sockets, I tend to cluster the tube connections into triple headers for triodes (plate, grid, cathode), 4-pin headers for pentodes (plate, grid, cathode, and screen/suppressor). This gives discrete 'wire bundles' that lead from the pcb to the socket and cleans up a lot of the wiring mess. As an example, for a regular dual-triode, there will be a triple wire bundle (with it's own header) on the PCB leading to the first triode, and a second leading to the second triode. This gives two, 3 wire assemblies that lead from the pcb to the socket.

In fact, if your sockets are remote, you don't need to route heater traces on the PCB at all, you can just install twisted pairs to the sockets leading directly from your regulation circuit.

Lastly, I would bump up your trace clearance up to 10 mils or larger. I always make clearances half of trace width, so for your layout, I would set it to 15 mils.
 

BluegrassDan

Well-known member
Joined
Mar 16, 2009
Messages
478
Location
Elizabethton, TN
Okay...let me give more info to clear up the assumptions:

This PCB is based on a version that I have already prototyped via turret boards. (That EQ section alone is what led me to convert this to PCB!)

It uses a cable-tethered external power supply, so there is no issue with PSU filter cap grounding locations, EMI from the power transformer, etc. It is incredibly quiet.

The tube sockets will still be mounted on the board, not the chassis.

With that being said, I have ZERO experience with PCB layout and appreciate all the insight. Not having the 3rd vertical dimension offered by PTP wiring is challenging for my beginner brain.

It would be pretty simple to "snake around" a thick ground trace that follows the signal. Would that be better at preventing potential ground noise?
 

BluegrassDan

Well-known member
Joined
Mar 16, 2009
Messages
478
Location
Elizabethton, TN
The other challenge is fitting two of these PCBs into a 17" wide space with room for mounting the input and output transformers. It's currently 6.5" x 9.5". I suppose things could be shifted upward a bit and the three triodes' caps and resistors shifted right for a bit more space between components.

Another thing would be wiring the heaters directly to the tube sockets, which would get rid of those huge 100 mil traces. Come to think of it, that would really clean things up a lot and allow for better component placement and routing.
 
Last edited:

BluegrassDan

Well-known member
Joined
Mar 16, 2009
Messages
478
Location
Elizabethton, TN
Here are some screenshot board samples including one showing ground plane clearances.

I spaced out the tube components a bit more, omitted the heater traces, increased clearances to 15 mil, and made all traces 30 mil. It will have 2 oz. traces, so 30 mil should be plenty, right?

Top (red) layer is signal ground plane with only a few traces.

Again, this will have an external PSU. Does this layout look like it works, or should I remove the signal ground plane in favor of traces? Or make separate ground pours?...one for V1 and V2, another for the EQ section, and a third for V3 (makeup gain) and V4 (buffer), for example.

Anything else to beware of?

Thanks in advance!
 

Attachments

  • Board,-V2-biggest.jpg
    Board,-V2-biggest.jpg
    188.9 KB · Views: 12
  • Screen Shot 2021-06-22 at 1.34.06 AM.png
    Screen Shot 2021-06-22 at 1.34.06 AM.png
    320.8 KB · Views: 8
  • Screen Shot 2021-06-22 at 1.58.21 AM.png
    Screen Shot 2021-06-22 at 1.58.21 AM.png
    192 KB · Views: 9
  • Screen Shot 2021-06-22 at 1.58.41 AM.png
    Screen Shot 2021-06-22 at 1.58.41 AM.png
    231.4 KB · Views: 9
  • Screen Shot 2021-06-22 at 1.59.00 AM.png
    Screen Shot 2021-06-22 at 1.59.00 AM.png
    242 KB · Views: 16
Last edited:

abbey road d enfer

Well-known member
Moderator
Joined
Jan 22, 2008
Messages
12,661
Location
Marcelland
I believe it could "work". In the absence of a schemo it's a little difficult to judge. I believe the way some caps are grounded needs discussing.
Reistors should be near the electrode they are connected to. E.G. R7 & R8 should move West or even better North. R11 North, R12, R14 West.
For signal, 12 mil width/12 mil clearance is adequate, but for B+ and anodes, you need at least 24 mil clearance.
 
Last edited:

Latest posts

Top