PCB Layout

[dsavitsk]

I am trying to do my first PCB layout, and would like to get comments about how to proceed.

The schematic is as follows (it is basically the cathode follower from MJ's book with the addition of R1):

It is a basic cathode follower used for a buffered passive preamp. The idea is that one can use any 9 pin mini (12ax7, 6dj8, etc), and simply use the appropriate resistors. It should be pretty easy to change this to an octal for 6sn7 types as well.

Here is my first go at a layout.

C1L and C1R are sized for solen 1uF caps standing on end. They could also be jumpered, perhaps. R1 is for safety and can be left out in most cases. R2 might also be able to be jumpered. C2 is something like a 4.7uF film cap (like a solen) mounted off the board. It stretches from the pad by its label to the pad by R6. The resistors are all 2 watt (mostly because I like Kiwame's), though I have not done the math to figure out what they need to be. Any comments, esp w/r/t/ the grounding and the B+ power, and the heaters.

I am trying to fit this on the ExpressPCB special deal size board (3 boards for $60), so I don't want to go any larger. I am not sure I'll actually ever get anything like this made, but it seems like a decent and simple project for learning.

-d

 

[Voodoochile]

This might not be what you had in mind... but I'd proceed by building it up on terminal strips, laid out similarly to your PCB layout. You might have a revelation during the build, and will no doubt find something you wish to change.

Just do one channel even, and use a cheap pot initially.

I made a neat little phono stage using the expressPCB deal, but I decided to build the thing on perfboard first. Sure enough, before I was done I had some things I wanted to change.

 

[dsavitsk]

This is as much about learning to design PCBs as anything else. I'm not sure I really even have much of a need for these buffers, I'm just curious. Also, the cost per board is less than just one of the output caps, so even that is not much of a consideration. So, back to the board ...

 

[skyskraper]

one thing drilled in to me by AMB about pcb layout is to use 45 degree angles and not weird ones. it took a bit of thinking to get used to it but it's not too hard when you do get used to it and is way more aesthetically pleasing too

for some boards pcbfabexpress seems to be cheaper then expresspcb. however the downside to that is you can't submit expresspcb files. if you do register with them my user name is "skyskraper" if you want to enter it in to the refferal box.

also futurlec.com seems to have good prices on small runs of smaller boards, so they may work out to be a good option for some also.

 

[MisterX]

Quote:

if you do register with them my user name is "skyskraper" if you want to enter it in to the refferal box.

Only if I get a free Ipod.

 

[skyskraper]

hah doesnt bother me i aint giving you shz

 

[dsavitsk]

Whatever savings are to be had by using a different company, my guess is that needing to learn more difficult software will cost me more. I'll look into it, though.

Anyway, 45 degrees. I needed to use thinner traces to get this to fit. Is that a problem with a B+ that can get up to almost 300V?

 

[skyskraper]

well i can see the negative there. maybe you could play with the actual layout. my first few efforts were very random and i had a hard time conceptualising a layoutin terms of the nets and traces. i am not confessing to be good at this by any stretch, but using the same circuit and doing maybe half a dozen layouts for it have led me to a hugely routing scheme.

 

[nleahcim]

Quote:

Originally Posted by skyskraper one thing drilled in to me by AMB about pcb layout is to use 45 degree angles and not weird ones. it took a bit of thinking to get used to it but it's not too hard when you do get used to it and is way more aesthetically pleasing too

I've heard this advice from other people before - but I've never understood it. Whta's so special about 45 degree angles? Why not 30, 60, or 28.324125? I can't imagine it's electrically any better. In fact I expect it's worse as it causes traces to be longer. So - why 45?

 

[SnoopyRocks]

The second one looks better but still has room for improvement. Keep at it. Like most things, practice makes perfect. Symmetry, and simplicity are your friends.

If you aren't going to make the traces thicker, I would add teardrops at the mounting holes.

Also, filling the signal layer with a ground plane is a good idea. However, this can be a pain in the ass if the software doesn't support this feature. I've never used the software that you're using but can tell you that the demo version of Mentor Graphics PADS Layout does this, along with everything else that the full version does.

 

[tangent]

Quote:

Originally Posted by dsavitsk I needed to use thinner traces to get this to fit.

Some places where some rerouting would alleviate this problem:

1. From the tube pin at 11 o'clock, route that trace up and over the one at 10 o'clock instead of under it. That will allow more room for the trace coming from the pin at 5 o'clock.

2. To make #1 work, add a short vertical segment to the trace coming from 1 o'clock.

3. Move the resistor in the upper right corner down far enough that it can jump over the trace coming from the pin at 2 o'clock. Then take that trace over and then down instead of down and then over.

4. A similar thing can be done with the trace at 3 o'clock.

Quote:

Is that a problem with a B+ that can get up to almost 300V?

When it comes to voltage, what matters is separation. So on that score, the thinner traces are doing you a favor here. (Speaking thereof, there are several places where you're running signals closer to different conductors than is required.)

Thicker traces, on the other hand, give you lower resistance (hence lower induced voltage drops w.r.t. current) and lower parasitic inductance.

As with everything in engineering, you have a tradeoff here. You'll have to figure out where the balance point is.

Quote:

Whta's so special about 45 degree angles?

Couple of reasons:

1. When the traces get dense, it helps them to nest better.

2. A 90 degree corner gives you the worst practical case of the "inside track" issue: the edge of the trace containing the inner part of the elbow is a shorter path than the other edge. This matters at high frequency. Using a pair of 45's instead is the best compromise with straight lines. Better is to use a corner mitering feature, like EAGLE has, but ExpressPCB doesn't have this.

3. It looks neater. This isn't just a prettiness argument. Sloppy layouts often indicate sloppy thinking. There's a point in a good layout where it feels tight as a drum: moving anything even a little bit has widespread effects on the layout because everything is balanced carefully against everything else. This is a good thing: it means you have balanced the forces as well as you can given the constraints you have.

 

[guzzler]

Angles less than 45 degrees should be avoided completely, as they can act as "acid traps" in the etching process, meaning that etchant isn't removed in the washing stage and continues to eat into the copper. The only thing to add about it is not to compromise a crucial section of a design JUST to include the 45 degree turns. For example, a diagonal section might allow better routing of a tight and delicate trace (eg, a signal trace) through a dense section. Do, however, fit it all together with the 45 angles, and then examine it for any better routings if possible.

 

[Born2bwire]

Say Tangent, on a side note, what is your heuristic for choosing the amount of chamfer for a bend in the microstrip? My microwave handbooks suggest that the percentage to cut the corner is equal to 52+65*exp(-1.35*w/h) where w is the width of the line and h is the thickness of the substrate.

 

[Garbz]

sorry to skip ahead without reading, but wouldn't it be better to run B+ from a single fat trace and have the ground plane covering the underside of the tube as well? This may work better as a shield against noise.

 

[jcx]

http://www.vutrax.co.uk/trackwidth.htm

clearance calculations suggest you can't afford to put gnd fill/planes between pins in a tube pcb with any appreciable B+ V