Yes, the schematic, trafo and regulator look good, the trafo should be able to handle all the LEDs fine.

 

Awesome! Here is what I have for the PCB. Included are two images, one with a ground plane and one without (to see routing better). In addition to the ground plane, is there anything else I should add? Perhaps a power plane for VLED and/or V+? I just don't want to overlap power planes, creating a small capacitor. To my knowledge, a ground plane is the most important.

 

Any thoughts?

 

Nice job.

Is this the look you have in your mind?

​

 

Nice job.

Is this the look you have in your mind?

​

I love you. I had no idea how clean it would look. Any chance I could get a peek at the underside?

Also, what program did you use? I primarily use SolidWorks and 3DSMAX for my 3D work and then render in Maxwell. Do you know of a way to export .brd or .sch to these programs?

 

Wait a minute - you're going to be supplying a lot of current from that 7805 regulator to drive all of those LEDs; if it's going to be powered from 12v, you'll wind up with up to 20 x 20mA x (12v-5v) Watts, or ~2.8 Watts of power dissipation in the regulator. The regulator will need a heat sink and air circulating around the heat sink, or it will get hot during loud music passages, which may cause the regulator to shut down. With no heat sink and the regulator tab exposed to 25°C/77°F ambient air temp, the regulator will overheat if power dissipation exceeds 2 Watts. If you put the project in an enclosure with no air circulation, your mileage will be worse.

The ground plane can serve as a heat sink, but I'm not certain how you are planning on mounting this thing. You could install the 7805 from the bottom of the board instead of the top so that the tab will be in full contact with the ground plane (this is fine, as the tab is connected to the ground terminal; not like the LM317 or LM337). If the board is mounted vertically with air circulating across the ground plane, that will probably provide enough cooling.

If you mirror the 7805, it should send it to the bottom of the board. You will only have to do minor re-routing (IN and OUT terminals), and the new routing will actually be cleaner than what you have now.

If you run a DRC in the board as shown now, it will likely complain about the tab of the regulator overlapping the trace running to the bar/dot switch. Moving the regulator to the bottom may help the "space crunch" a bit.

 

I love you. I had no idea how clean it would look. Any chance I could get a peek at the underside?

Of course you can.

Also, what program did you use? I primarily use SolidWorks and 3DSMAX for my 3D work and then render in Maxwell. Do you know of a way to export .brd or .sch to these programs?

I'm using eagle3d to make a script-file. This file I'm rendering with PovRay.

I find this very useful, because then I can see how the board will look like when its done.

 

I find this very useful, because then I can see how the board will look like when its done.

Like those two traces running through the holes

 

Like those two traces running through the holes

Excactly, and it looks like the LEDs are not connected with both legs...

 

Like those two traces running through the holes

Are you looking at the edges of the ground plane? Eagle3D/POVray doesn't fill in copper pour areas, so the outline can be somewhat confusing if you don't realize what it is.

The Eagle autorouter does some strange things. Reorienting some of the components would make the routing less quirky, like rotating R1, R2, and R5 90°. Placing C3 and C4 close to the IC power pins is preferred. C6 seems to be quite a ways from home.

You might think about using the bottom of the board for horizontal traces, and the top of the board for vertical traces. As it is now, the ground plane is nearly cut in two in the vicinity of IC1. Just reorienting some parts might help to clear that up.

One thing I really don't care for is that the autorouter runs traces right through pads, as in the anode supply traces for the LEDs. I like for pads to only have one trace coming in or going out, as otherwise it make it more difficult to solder to the pad without lifting it; the traces act like heat sinks, pulling the heat away from the pad, making you apply more heat for a longer period of time. I would run a nice wide trace a short distance away from the LED anodes, and run individual traces from each anode to the wide trace. It's more work initially, but less of a chance that you will have to do a messy re-work later; and it also provides more flexibility in case you need to make changes to the board.

Anyway, once I've reached a certain point with a schematic/board, I'll save it with a version number on the end, like V1, V2, etc. That way if a disaster happens (or you just don't like the way that version is going), you don't have to start over - just resume from an earlier version.

 

Excactly, and it looks like the LEDs are not connected with both legs...

This is a good catch, as the +V supply to the LEDs has been routed on the top of the board. That will not work well for a home-made board, but will be fine for a commercially-made PCB that has thru-plated pads and vias. Even so, if our OP decides that they need to make some changes on a board that's already been made, it would be easier to have the traces on the side of the board that is accessible.

 

Looking at the board again, I see that the LEDs are soldered on both sides. I think this will be hard to do. The same goes for all of the ICs.

 

Looking at the board again, I see that the LEDs are soldered on both sides. I think this will be hard to do. The same goes for all of the ICs.

DIP IC's won't be a problem whether the board is made at home or commercially; as you can solder the pins from the top and the bottom; you would only need to solder from the bottom on a commercial board.

The LEDs are a problem for home-made boards, but not so much for commercial boards.

 

I just remember the challenge I had, when I made Bills 25 LED Open Ended sequencer.

 

Would a layout like this be better? I tried to follow your suggestions for where to put the various components. To answer your question, I'll be using a heat sink on the 7805 and I'll have a small fan to move air away from it. I have lots of experience with computer case cooling, so I'll have no problem making sure it is quiet and cool.

 

Are you certain that you want the regulator on the top of the board? Routing might be easier if it were on the bottom. Using the mirror tool will and clicking on it will send it to the other side of the board.

Don't forget that resistors can be used as jumpers over traces that would otherwise be awkward to route; just put them in strategic locations. If something is not routing well, you can always add zero Ohm resistors and use actual jumper wires instead of resistors.

Your DOT/BAR switch could be rotated 180° to ease routing.
Move C8 and C7 nearer the 7805 terminals so that the air wires aren't crossing so much.
Looks like trimmer R10 would go better below the opamp.

You might want to start off by plunking down the ground plane using the polygon tool so that those air wires won't appear anymore. Don't forget that the polygon width should be 10 mils or more, or it'll take forever to fill the polygon.

And I'm fresh out of time for this evening.

 

Alright. I tried to follow your suggestions as much as possible. All my bottom wires are horizontal and my top ones are vertical. I moved things around according to how you thought would be best. I also mirrored the 7805. I'll still be providing lots of cooling for this piece, regardless of how well the ground plane will act as a heat sink. I notice that the ground plane is once again split in two, this time it's just lengthwise. Is this ok or will I need to fine a way to bridge the two halves closer together?

I did a DRC and nothing came up, even with my specs of 10mil spacing and 24mil trace width. Also, I won't upload new pictures, but I just mirrored the crew holes since I'll be screwing this in with the top facing the panel and the 7805 facing the open area in the case.

 

Are you going to make this board yourself, or are you planning to send it off some manufacturer?

Reason for asking this is that I think some of the traces are dangerously close to some of the pads.

 

Are you going to make this board yourself, or are you planning to send it off some manufacturer?

Reason for asking this is that I think some of the traces are dangerously close to some of the pads.

Definitely sending it off to a manufacturer. There's no way I'd be able to do this, especially with those traces so close as you mentioned. I have a small group of people who want to do a group buy, so the price shouldn't be too outrageous.

Specifically, though, where are you referring to about the traces being so close. Perhaps there's a way I can change it in Eagle.

 

I've added a yellow circle in the areas I think is a little bit close...