First build in progress - Deliverance 60 adapted to two channels

[Asdrael]

Hey there,

first post, first build Actually first "and a half" as I finished a Rosamp SLO 30 kit last year, which ended up looking good inside and awesome outside, sounding great, and all of this on the first startup. Also I didn't die so bonus points right there. I guess training soldering on pedals first helped. I also build guitars but that's not on topic...

I was lucky enough to recently find some schematics of my former favorite amp, the Deliverance, from 3 different sources that all align and one local guy was nice enough to share his work on Eagle with me (if you read me, you rule thanks again). Decided to go from the single channel, no FX loop amp that the DL60 v1 was to a two channels with shared EQ and an FX loop. The schematic I got had some relays (G5V1) put in for the Less / More gain modes present in the original, and an independent second master.

My changes were to link the second master to the Less / More mode, as well as add the two gain knobs (Gain I and Gain II) on relays. Basically completely splitting the Less and More channels, as this was my main gripe with the original design (alongside the absence of loop). That meant adding a lot of relays. I am however *not* well versed at all in relays and only learning my ways through tube amps. I am hoping that first, this schematic might give ideas to someone if they want a great amp, and second, someone will point any potential mistake in the schematic. The core is right (hey it's a copy from a reverse engineered schematic), not 100% on the relay system though. Especially the G5V2 as a dpdt for the Gain 1 and 2 potentiometers. Seemed logical to go with a DPDT there but I am sure for some obvious reason it's a bad idea. Also not sure those G5V-X relays are the optimal solution due to their massive footprint, and if the 12V version is the way to go. They supposedly have a 75% / 5% coil switch actuation but am I really safe from potential fluctuations (hopefully close to none but still) of the 12.7DC rectified at the LM317?

All of it will end up on a PCB I'm designing now. Seeing it as a big learning experience in electronics and Fusion 360. But that might be a later post in the PCB subsection.

Here is the schematic (made for PCB printing with one board for the power tubes, one for preamp + power section):

Schem v4.png

So yeah, feedback welcome, shoot me etc

[jbrrrrr]

Very cool project - I'm interested to follow along as you build it. Post some clips when you've got it making some noise!

[Asdrael]

Made some progress and "finished" the PCB. Also known as I am not sure what I am doing and I did the best I could given my limited knowledge. Read a few PCB design basics articles and went for it. I paid attention to crossing, width, clearance, and obviously to grounding. Had some fun with rounding the 90° corners I couldn't avoid. I went with the power section ground plane branching into a star ground for the "signal" side of things and a star ground for the DC part of the circuit, with the grounds meeting close to the connection point to the chassis ground. Also should have the right orientation and spacing for the KT88. The PCB is done so the power tubes PCB and the power/preamp sections will be split.

PCB.png

I am triple checking all components right now for lead spacing and general footprint. As I am going for PP caps on the signal lines (and PET on the non-signal) there are some massive blocks here and there, but overall it looks like it'll fit nicely into a small enclosure.

As before, feedback welcome. It's my first PCB so I'm sure it's burning the eyes of a few people. I'll teardrop the vias and socket pins before sending it for production at the very least don't worry

[Lauri]

What's the clearance on the power tube pcb? I would increase it especially on anode pins and everything connected to them.

[Asdrael]

What's the clearance on the power tube pcb? I would increase it especially on anode pins and everything connected to them.

I have everything at 100mil+ on the power tube PCB except on the ground plate which is set to is 50mil (which I just realized now). I think it's fine for most lines since it will be coated with solderscreen but as you pointed out, too small for the plate pin and likely grid at the very least. Thanks! I will revise and bump either the plate/grid to 100mi or just the entire pour and be comfortable with it.

[Lauri]

I have everything at 100mil+ on the power tube PCB except on the ground plate which is set to is 50mil (which I just realized now). I think it's fine for most lines since it will be coated with solderscreen but as you pointed out, too small for the plate pin and likely grid at the very least. Thanks! I will revise and bump either the plate/grid to 100mi or just the entire pour and be comfortable with it.

Another thing to pay attention to is the thermal relief gap and thermal spoke width on the ground connections to the ground plane. Make sure the gap isn't too small or the spoke width too high or it's going to be difficult to solder components to the pcb.

[Asdrael]

Another thing to pay attention to is the thermal relief gap and thermal spoke width on the ground connections to the ground plane. Make sure the gap isn't too small or the spoke width too high or it's going to be difficult to solder components to the pcb.

On my planes I was using 10mil/10mil for spacing and width. Considering the size of the pads and what will go through, I think I might have the other problem in that my spoke width will be too small... However, the main "branch" of the star ground is a 150mil track so no thermal relief built in. I should change that and make it a "pour line" with the same rules I suppose otherwise I might burn something. Most of my components however connect to it via a rather normal width track, like 50mil max.

It seems however that Fusion can't change the thermal relief gap, just the thermal spoke width. So I think I'll go with 10/20 or 10/25, that seems more in line with what I will be trying to solder and why.

Thanks a lot for the feedback again, really helpful! Makes me realize there is even more left to learn and fix than I thought.

[LOUDthud]

The Heater lines in the preamp are too narrow. Most texts on PCB design will give you an equation for minimum line width for a certain current, but they don't tell you what the Voltage drop will be. In many cases the Voltage drop will be more than you would like.

The lines between the series filter caps should be increased.

Pad sizes on power resistors should be increased.

[Asdrael]

Change log, as much for me as to thank the advisors:

What's the clearance on the power tube pcb? I would increase it especially on anode pins and everything connected to them.

Changed it to 100mil around the higher voltage parts.

The Heater lines in the preamp are too narrow. Most texts on PCB design will give you an equation for minimum line width for a certain current, but they don't tell you what the Voltage drop will be. In many cases the Voltage drop will be more than you would like.

Good hint. Read up a bit and found some nice calculators. My voltage drop would have been around 0.35V on V1 with my setup. Would have been theoretically fine, but better safe than sorry: I doubled+ the width where I could and I should be closer to 0.15V, which would be 12.55V DC.

The lines between the series filter caps should be increased.

Doubled. I was initially under the assumption that I could half the thickness of the initial trace because R//C/R//C but I got room, so back to max width.

Pad sizes on power resistors should be increased.

Note sure what you mean by power resistors there. The resistors on the power tube part, the power section around the filter caps, the resistors feeding the plates or just every single resistor with a 1W+ rating?

Thanks again for the pointers. Board looks more solid now.

Edit: got motivated, increased the pad size of basically every resistor 1W+. they were all rather small indeed, now they are 75 or 100mil diameter depending on the size of the resistor.

[Asdrael]

Progress made according to the feedback above. I also increased the clearance from the "first" filter cap pins that will see 450V+ to the ground plate just in case (100mil, those who see less than 250V stay at 50mil). Looks a bit more like swiss cheese but should be less prone to accidents. That may very well be excessive but I don't see a downside.

The schematic hasn't changed so I am still praying I got the relays right. The PCB now looks like this:

PCB.png

Also 3D renders are cool:

3D1.png

And even better in a chassis (not 100% on size yet, might go for slightly bigger):

3D2.png

3D3.png

I have to see how to move the preamp tubes in the chassis so everything fits better, or just buy a larger one, but so far... so good?

Edit: yeah looks more relaxed in a Dumble case if I want to keep some space between the 12AX7 and the transformers.

Dumble.png

[Asdrael]

Since I definitely want to try to stick to the smallest form fact I realistically can, and that I didn't like the fact that the heatskink was hugging the side of the case and bumping potentially into the power switches I went back to the drawing board.

I am not sure it is a good idea but I wanted to give it a shot. I have seen the main power board being separated from the other PBCs, but never the power board "mated" with the power tubes board. I suppose heat could be an issue for the capacitors but given they are mounted "upside down" and there is significant distance... I am not sure it should cause an issue. It just means I have to be careful with the off board wiring, as the heaters for the power tubes will have to come from the side and either fly over the Grid trace (with over 1 inch clearance that shouldn't be an issue) and be close to a plate cable going to the OT from V5 (issue or not? no idea) or come from the other side, a few inches away from the off board cables coming from the PI and going to the power tubes. Obviously the heaters will be properly twisted and come 90° to everything (and will be on quick connect crimp plugs).

Obviously, there is something I am overlooking so I'd be glad for pointers. Right now it has the big advantage of fitting no problem... Example below with more or less the position and spacing the 2 boards will have.

PCBbis.png

3Dbis.png

[Asdrael]

So, almost everything electronics related has been ordered and received. The pcb is ordered but still on the way. Just in time for me to realize that I made one spacing slightly too large (7.5mm instead of 5mm for a silver mica… so nothing major).

I went for a Hammond 1444-1783 aluminium chassis but damn, I didn’t think 1,2mm (0.05”) thickness for the aluminium would feel that flimsy. Probably going to return it, I don’t really want a bent chassis day 1. Just have to find a thicker equivalent which proves to be difficult in the EU, so it might be custom.