[rembrant]

I'm sure most of you can tell what this is.

This Is the first time I have tried to design a PCB. I have only done it really as a learning tool. I would appreciate some critique on this one. Who knows, maybe once we get something satisfactory I might order a few.

I used ExpessPCB for this because it seamed the easiest. The software comes up with 8 Pieces for just under $100 with no solder mask or silkscreen.

Things I didn't consider.
Size. Currently it is 1.3"x3.2" Thats Probably not mint tin size but there is room to work with.

Trace width. Those are .01" traces except for the V-ground which is .02"

No place for a Pot. Woops. I wasn't thinking about it honestly. I will work it in there some where.

Edit
Updated layout. see post #32

 

[rembrant]

LMAO... Well that wouldn't work very well with the inputs and output switched around like that. Yep I'm tard. I have updated the Image.

 

[tangent]

1. The wider your traces, the less resistive loss you will get, and the less parasitic inductance there will be. For such a..."fluffy" board layout, there's no reason to skimp. I would use 50 mils for most traces, and 100 mils or so for the ground bus. Or, better, use a ground plane for ground, if EPCB will let you do that with a 2-layer board.

2. Use 45 degree bends to round off those sharp corners on the traces. It looks nicer, and shortens the paths.

3. The green trace from the bottom vground resistor could come up at a 45 through the lower 1K resistor, greatly shortening its path.

4. Since you won't have silkscreen, consider labeling the parts on the copper layer. It restricts your choices when it comes to trace paths, but you've got all kinds of space to play with.

5. Your caps should be much, much bigger. The rail caps can aren't as big a problem as the input caps...you're going to be seriously restricting the quality of the amp with the type of caps you'll have to force into these positions.

6. In DIY PCB design, I find that you usually don't want to put wire pads off at the end of traces. Collecting together several related wire pads is one thing, but collecting almost all of them at one end of the board is too extreme. Remember, with a project like this, you have a third dimension to play with: a hookup wire comes up out of the board and can then take any 3D path from there to its panel component. Also, hookup wire is going to be thicker than any trace, again due to the 3D nature of the thing. (PCB traces aren't exactly 2D, but you see the point.) So, more hookup wire, less PCB trace.

 

[rembrant]

Awesome advice! Thank you very much. I have continued to work on it and it has become much smaller. The only reason I have the wire connections going to the end of the board like that was because I wanted to use those board mount connectors. Your right though, I could just as easily leave them off and air wire would be better.

I was also thinking about changing the rail splitter to the TLE chip. That should free up some room in the power cap area. I could easily stand the resistors up and save even more space but I wanted to use some sockets so that the values can be changed anytime you like.

The software will allow me to plane both sides of the board if I wish. I did some experimenting with that feature this morning and it's gonna take some practice to get what I want.

I have increase the trace size on all the traces. I will see how much Bigger I can go.

 

[tangent]

Quote:

Originally Posted by rembrant /img/forum/go_quote.gif I wanted to use those board mount connectors.

In that case, design an EPCB part for them, with a correct outline. Even if you don't have a silk layer, it prevents you from trying to stack two connectors atop each other, and communicates to anyone looking at the board who doesn't yet understand it -- like me -- more of the intent.

Beware, however, that when using board-mount connectors, you greatly increase the difficulty of doing the panels, because now all of the holes have to be in the right place relative to each other. You can fake it by making all the holes extra-large, and covering up the slop with large washers, but then you lose out on the prettiness factor that a precision board-mount-everything design can give.

 

[rembrant]

Ok, I have made some changes. The board is now 2.3"x1.3" and all traces are now .05". I have added a gratuitous ground plane. I have moved most of the silkscreen into copper.
I haven't added more room for the input caps for two reasons.
1. From what I have seen, most people here jumper them anyway.
2. If you want them and need more room you should be able to fit quite large ones in now and tie to any part of said gratuitous ground plane

 

[rembrant]

Quote:

Originally Posted by tangent /img/forum/go_quote.gif In that case, design an EPCB part for them, with a correct outline. Even if you don't have a silk layer, it prevents you from trying to stack two connectors atop each other, and communicates to anyone looking at the board who doesn't yet understand it -- like me -- more of the intent. Beware, however, that when using board-mount connectors, you greatly increase the difficulty of doing the panels, because now all of the holes have to be in the right place relative to each other. You can fake it by making all the holes extra-large, and covering up the slop with large washers, but then you lose out on the prettiness factor that a precision board-mount-everything design can give.

Ahh that is true. I had assumed that the holes would be staggered in the pattern that they are now and that they would be at .1" of separation. I also didn't really take into account the size of the body of the connector. I guess it's really better for everyone if I just forgo that for now. At least until I read the data sheet.

 

[deltaydeltax]

Post your schematic. Something looks funny.

You also don't want high impedance traces running next to low impedance traces. Doing so will cause the amp to oscillate at higher gain settings.

Ground fill can help to keep low impedance traces and high ones from interacting. It can also cause problems if done incorrectly.

 

[tangent]

Quote:

Originally Posted by rembrant /img/forum/go_quote.gif I have moved most of the silkscreen into copper.

Okay, but leave the silk outlines so you don't overlap parts, and so people can see which pads belong to which parts. If they're still there, turn the layer on before saving out the graphic.

Also, use PNG for line art like this. JPEG blurs the sharp outlines, making it hard to read. To save some space, reduce it to 16 colors in a graphics editor. (You probably got a 24-bit PNG from EPCB, or a screen grab.) The resulting file should be a lot smaller.

Quote:

I have added a gratuitous ground plane.

Can you knock holes in EPCB ground planes? If so, do so under and immediately around the op-amp. Op-amp input pins don't like the parasitic capacitance this adds.

Quote:

From what I have seen, most people here jumper them anyway.

I'd decide this for yourself before you burn boards. Since you're doing this for yourself, you don't have to make anyone else happy: add the pads, or not, as you choose.

Quote:

If you want them and need more room you should be able to fit quite large ones in now and tie to any part of said gratuitous ground plane.

You're confusing the supply caps with the input caps. The input caps don't connect to virtual ground.

However, it's true that you can add the input caps off-board, if you don't use board-mount jacks. They just splice into the input wires.

Getting back to the board:

1. The V- line is probably shorting out on those two square pads it passes. Remember, pads are on both sides of the board. You'll have to jink a little around them.

2. Still a lot of 90's in there... And that oblique angle in the upper right...ick. Stick to 45s.

3. That 100K R in the lower right...I'd make the trace an L instead of a U

4. You can swap some trace layers in the upper center and get less ground plane interruption.

5. The upper 10K R can probably move left to jump over those traces so you don't need the via.

 

[rembrant]

OK, I have worked on this for a while now. I did my best to take most of the information into consideration. It has shrunk again as well. Now it's 2.1"x1.325".

Like I said before, I forgot about trying to use the board mount connectors even though I did model them. They just took up more space than I was comfortable with. I removed the plane area under the Opamp and added much more room for the rail caps.

 

[cobaltmute]

Try the following:

-Move the traces from the op-amp to R5 to the ground plane side. You may have to open the void up a little bit in the plane for this
-Move all the other traces to the non-ground plane side.

This will make less cuts in the ground plane.

 

[tangent]

Regarding the sharing of a hole between R3 and R4... Don't do that. You've got the space to give them their own pads.

Getting back to the question of the TLE, with the current design, I'd add it, nestled in the valley between the caps. You've got the space, so why not? Make it an option, so you can play with both that and the resistors.

 

[rembrant]

I thank everyone for their input on this. Especially you Tangent. I feel like I just took the crash course.

Changes this time around:
I opened up the ground plane some and switched the traces as per Cobalt.
Added more room for the R3-R4 so they both have a through hole.
Added through holes for the TLE2426 + a single capacitor and added traces for it. All one has to do is add the single cap and TLE to use the rail splitter. If I wish to use the resistor divider all I have to do is add the caps and resistors and jumper across J1 and J2.

It's not great, but it sure is a whole lot better than what I started with.

I give you the latest monstrosity! Rev00006A

Edit:
Ya know I'm not real sure that will work right in it's current configuration so I added a place to jumper across if I want to use the rail splitter. J3 and J4

 

[tangent]

I don't see the need for the jumpers, unless you're going to have both options soldered to the board and then switch between them. Otherwise, it should just be a matter of populating only one of the two options.

You're going to tweak the position of the TLE so it doesn't overlap the caps, right? If the default grid size doesn't do what you want, use a smaller grid for this. Remember to return to the default grid when you're done, so you don't end up with too much weird stuff off-grid.

You still have a lot of ugly bends to clean up. The electrons don't care, but we don't make PCBs just to make electrons happy.

 

[rembrant]

It wont overlap the caps. There will only be one farther back if I use the rail splitter. The other two caps will only be there if I use the resistor divider. I had hoped to use those little socket strips so that I can change parts out whenever I want. Then I can make a permanent one once I find what suits me.

I suppose your talking about the 90's that are still there. I really am a novice at this but I don't see what harm they can do. I'll look at it again tomorrow when I have fresh eyes and a belly full of turkey.