Single sided SMD cmoy pcb - please comment

[balou]

Hi,
Just made my first pcb layout... well, honestly it's my third, the first was a complete failure, the second was enormously large... here is my third try.
It's a simple cmoy, with a tle2426 railsplitter, a single cap (10mm diameter), and 0806 resistors, with groundplane, and I managed to use just one side.

I plan to etch this myself (first etch, thats why I only used a single plane), and to learn a bit smd soldering while doing it


So here we go with some pictures of the board:

Does anybody spot an apparent flaw? What could be done better?

And a question about raster size: Sometimes I chose a 'creative' raster size to cram in all the traces. If I order a professional board, do the traces have to be in a specific raster? Or do only the holes/vias have to be in the raster?

edit: I forgot... the pot is an alps rk097, the jacks are lumberg 1503 08 or one of its chinese clones

 

[DaKi][er]

The traces from the resistors to the opamp are far too long, put them as close as you can

You need capacitors from the +/- rails to ground

This is just a personal thing, but I like to make all traces at 45 degree angle increments, you've got a lot of everything in there

 

[balou]

I thought with a TLE2426, caps from +/- to GND are no longer needed.

What is the drawback of having the resistors far away from the opamp? First, I had them right next to the opa, but cramming them under the jacks helps to save a lot of space

 

[digitalmind]

Quote:

Originally Posted by balou /img/forum/go_quote.gif I thought with a TLE2426, caps from +/- to GND are no longer needed. What is the drawback of having the resistors far away from the opamp? First, I had them right next to the opa, but cramming them under the jacks helps to save a lot of space

A 100nF cap between the power lines and ground is always a good idea when working with precision equipment that's easily influenced by noise. It filters it.

Which is also why you want all the lines as short as possible, open straigth lines from the opamp to the resistors are pretty much antenna's picking up noise and broadcasting it.

Note that these are my experiences with high frequency applications (>1MHz). I'm sure there will be less trouble with an audible frequency spectrum, but these two points are easy to follow and will help.

Good luck with making the PCB's!

 

[balou]

Ok, now I don't know what were exactly talking about - power supply caps or bypassing caps? Yes, with many opamps bypassing caps are needed, but I plan to use the good-natured OPA2134 on this board. About power supply caps... commercial pocket amps seem to use just one big cap, and as I understand it, two supply caps are really needed in a resistor divider config like in the basic cmoy, but as far as I know, with a tle2426 they aren't absolutely needed.

Quote:

open straigth lines from the opamp to the resistors are pretty much antenna's picking up noise and broadcasting it.

does it really make a difference if the resistors are at the jacks and then a long line, or if the resistors are at the opamp and then a long line to the jacks?

Quote:

Good luck with making the PCB's!

thanks. Btw I'm still fiddling around... for instance replacing the 10mm cap with a 8mm one. With that, I can move the cap between the pot and the jack. It's getting really tiny

 

[digitalmind]

Quote:

Originally Posted by balou /img/forum/go_quote.gif Ok, now I don't know what were exactly talking about - power supply caps or bypassing caps? Yes, with many opamps bypassing caps are needed, but I plan to use the good-natured OPA2134 on this board. About power supply caps... commercial pocket amps seem to use just one big cap, and as I understand it, two supply caps are really needed in a resistor divider config like in the basic cmoy, but as far as I know, with a tle2426 they aren't absolutely needed.

Ah, I was talking about bypassing caps. They might not be necesary, but they'll never hurt.

Quote:

Originally Posted by balou /img/forum/go_quote.gif does it really make a difference if the resistors are at the jacks and then a long line, or if the resistors are at the opamp and then a long line to the jacks?

I've always found it comon practise to group parts together. The resistors are essential to the opamp in order to work correctly, so place those as close to eachother as possible. It keeps things looking tidy and often makes troubleshooting easier. Not very essential in such a small schematic, but if you take on larger projects it's nice if it's comon practise for you.

Quote:

Originally Posted by balou /img/forum/go_quote.gif thanks. Btw I'm still fiddling around... for instance replacing the 10mm cap with a 8mm one. With that, I can move the cap between the pot and the jack. It's getting really tiny

Tiny is goooood! Imagine how small a two layered PCB could be.

 

[balou]

It really is getting the length and the height of just the alps pot, and the bare minimum width with which you are still able to put in two 12mm wide 3.5mm jacks in parallel.

Oh, maybe I try to cram in a LED, but thats not so important, you could always wire one directly parallel to the battery

 

[Pars]

I would think you would want to move the pot out (down) closer to the board edge so that the mounting hardware would be right up against the case.

In Eagle, red signifies top layer. Are you sure you didn't mean to put everything on the bottom (blue) layer? Your pot, jacks and electrolytic cap would be impossible to solder on a home etched board (doable on a commercial board IF it had plated-thru holes). Also, thru-hole components benefit from having the solder side on the opposite side of the board from the component... helps prevent trace lifting.

I agree with the comments about resistors. You are using alot of board space routing the switch leads... I would route signal and resistors first, placing the resistors close to the opamp pins. You are also negating any ground plane under the opamp, where it is probably the most important.

As far as one cap preceeding the TLE vs. two caps following, read Tangent's article on virtual grounds.

 

[colonelkernel8]

Those are some fun traces

 

[balou]

Quote:

I would think you would want to move the pot out (down) closer to the board edge so that the mounting hardware would be right up against the case.

Already did that, I did a print-out mockup and immediately saw it was way to high above the edge
Quote:

In Eagle, red signifies top layer. Are you sure you didn't mean to put everything on the bottom (blue) layer? Your pot, jacks and electrolytic cap would be impossible to solder on a home etched board (doable on a commercial board IF it had plated-thru holes). Also, thru-hole components benefit from having the solder side on the opposite side of the board from the component... helps prevent trace lifting.

No, this is meant to be that way

Yeah I messed that up. But you could just mount the through hole stuff on the underside of the board
Quote:

I agree with the comments about resistors. You are using alot of board space routing the switch leads... I would route signal and resistors first, placing the resistors close to the opamp pins. You are also negating any ground plane under the opamp, where it is probably the most important.

Fixed that. I moved the opamp between the two jacks, and there I had enough space to move the resistors right next to the chip. But R2R and R2L are still directly at the pot.
Quote:

As far as one cap preceeding the TLE vs. two caps following, read Tangent's article on virtual grounds.

Reading it, I think I should be safe with just a single opa2134 drawing power

Board is now 19x39mm, maximum height is now the alps pot (11m above board). Cap is a 8mm dia, 9mm height 470uF

Quote:

Those are some fun traces

Why? Me likes round traces

I'm thinking about abandoning the ground plane in my home-etch. No solder stop mask, meaning I WILL make a lot of accidental connections to the ground plane

Here's the current revision:

 

[axiom]

Quote:

As far as one cap preceeding the TLE vs. two caps following, read Tangent's article on virtual grounds. Quote: Reading it, I think I should be safe with just a single opa2134 drawing power

I think he was referring to your previous picture which had a single cap after the TLE from the + to - rail. I'm pretty sure this wouldn't work.
The current revision with the cap before the TLE from + to - should be fine (note that the opamp will be current limited to 20 mA by the output of the TLE which should be sufficient).

Also, you'll have to solder these as they appear because if you put the through hole components on the bottom of the board it will change the pinout (because they will be upside down).

In other words your grounds on the pot would be on the two rightmost pins. To see this look at the second to last picture here: http://tangentsoft.net/audio/cmoy-tutorial/assy.html

You could mirror the layer and then you can mount all of the through hole components to the nontrace side.

Nice looking board

BTW if you were wondering how small a pcb for a cmoy could be there is a thread where someone made a 2 sided pcb smaller than a dime!!

 

[balou]

Before, after... the electrons don't really care. They float around the pads of the tle2426 anyway. That's at first very confusing and then very revealing when you work with Eagle.... it sometimes shows you connections you think are completely wrong, but then you begin to understand that all of these variations are equivalent.

About the smallness... yeah, I saw that postage stamp board, but somehow it is much bigger than my board. This board has an alps pot and two jacks directly mounted on it. with the smaller board, you have to wire them up separately, which in the end makes the whole thing larger than this board. double sided also wouldn't help much here, the size of this board is limited by the minimum width with which you can still put two 3.5mm connectors in the jacks, and the size of the alps pot with the knob attached. edit: I made a mockup of the amp. Minimum distance between two jacks (measured from the middle of the jack) is 12mm so that you can still attach a lineout dock and a grado headphone plug to it. this is my current spacing... it might already be a very thight fit with larger lineout docks. And a small pot knob has about the same diameter as an grado plug

On my current revision (6mm cap, max 220uF), you could actually make the board 0.0125 inch smaller if you would use two layers - thats the size of one trace going around the alps pot. Not worth the hassle

About the wrong plane... yeah, looks like it doesn't work 100%, I have to check how I could fix it with the least new problems introduced. The TLE2426 might be harder to fix than the pot.

And one more thing about the tle2426... the RSA Tomahawk and the Xin amps only have one cap, too. Well, maybe some small smd caps after the tle2426. And the Mini^3 has a 1000uF main cap and two 100uF caps. Amb told me that this is how it worked for him, altough he wasn't very specific if they are really needed. But the mini^3 is another league anyway, compared to it the currents that flow here are minimal.

 

[balou]

Umm... does anybody know how I can move parts to the other plane?
Or, if we're at it, whole signal layers excluding through hole parts?

edit: NM found it

edit2: yeah, eagle is unlike every computer program I have used to date. It takes some time to get acquainted to it. But what I do find to be very practical is that you can type in your commands. As a lover of unix shells, I will use it quite often as soon as I learned the different commands

edit3: the pot is giving me headaches. One wire doesn't want to fit in anywhere...

edit4: Now I've got a ground plane segment that isn't connected to the rest of the ground plane. But else everything has worked out. Except....

 

[balou]

Yeah, it requires greenwiring, see upper left pin of the pot and upper left pin of the first jack. I will fix it tomorrow, now I just wanted you to show how tiny it is.

edit: 37x18mm

 

[Pars]

Actually, you could have left the pot, TLE, electrolytic cap and jacks alone. Use the layer command to switch all traces to the bottom layer. You would then use the mirror command to move the SMD stuff to the bottom. Your opamp traces would need to be redone, and resistors moved around some, but the pot and jacks would have stayed the same.

For the ground plane and clearance issues for home etching/solderability without a solder mask, use the isolate command and play around with the parameters, clicking on the ground plane, to increase the spacing between the ground plane and traces, etc. I've done double-sided boards at home with full groundplanes, and not had any real problems with solder bridging (and that was before I knew about the isolate command).