33 replies to this topic

[remotewizard]

First, thanks again to kenNET for posting his TDA7313 audio controller project in the Showcase. That's exactly what I was looking for for my ongoing radio project.

I also found this, by Tiktak, which is a variation of the manufacturer's test circuit (adding a regulated power supply). I downloaded his pcb pattern, but have had a bit of trouble constructing the circuit. My eyes aren't what they used to be, and the board is a little to crammed for my tastes. Besides, I'd rather use screw terminals than RCA jacks for the board.

So I created an Eagle project to design my own variation (wutrh the parts spread apart for easier soldering). I also added a header so I can plug in my si4703 FM radio breakout board and rount its audio output to Input 3 of the 7313.

Since I've never used Eagle before, I was hoping one of you nice folks could look at my schematic and board layout. I've also included the TDA7313 manufacturer's test circuit, and Tiktak's schematic and board (much more polished than mine).

Note that I haven't added the ground plane yet for my board, as I'm frankly not sure how to do that.

Thanks as always for any or all help and advice.

Attached Files

•  Eagle Attempt.zip   131.81KB   10 downloads

[hanzibal]

I took a quick look at your schematics and the first thing I noticed was that there are no I2C pull-ups. I haven't read the TDA7313 d/s but usually those are not integrated so you need to add them yourself (I normally user 4k7) or it won't work at all.

I also made an ERC in Eagle which indicated a few errors:
 erc.PNG   56.73KB   25 downloads

Some of them are probably not show-stoppers (and you can "approve" them) but the ones within the red ellipsis are pretty critical so you wanto to fix those.

Btw, the ERC (electrrical rule check) is available using this button in the Eagle toolbar:
 erc_button.PNG   4.51KB   21 downloads

I'm no expert in PCB-design but other than the above, I think it looks ok, but remember I haven't taken the time to study the datasheets.

Adding groundplanes is actually quite simple and generally, there are some really excellent tutorials over at SparkFun which I used lot when I made my first PCB in Eagle (there is a whole series of them, this is just one example):
http://www.sparkfun.com/tutorials/115

And I found this thread on how to create ground planes in particular:
https://forum.sparkf...opic.php?t=7500

Basically you use the polygon tool to draw your ground plane(s) and then you connect it to GND.

Hope this helps a bit. Good luck!

[remotewizard]

That's perfect! I'll go add the pullups, fix the errors, and add a socket for the antenna connector for the si4703 (somethins I forgot), and make another try. Thanks! I'll publish the revised board design and schematic in case anyone else would like to try out kenNET's library (it's pretty cool!). Thanks as always for your help!

[hanzibal]

Cool, please do publish the schematics to let someone other than me have a crack at it too before sending the Gerber files to any FAB-house.

As said, my experience is not very big nor long but I do know that the best way to figure what's wrong with a circuit is to send the Gerber's away. After falling a a sleep the same night, the perception of at least three mistakes will suddenly wake you up (cold-sweating and shivering) thinking darn, how could I miss that!

I would love to have an arbitrary fake FAB house that I could send my designs to in order for me to realize my design flaws prior to fabrication.The next morning I would get an email from the FAB house saying "fooled you, we're not for real". I could then correct my mistakes and re-send the design to a real FAB house. But then again, the fake FAB house would have to one pretty "non-fake" looking or else it obviously wouldn't work and so this fake FAB house would have to be constantly re-appearing under different names, different web sites and slightly different (but yet attractive) prices. However, the latter is not possible simply because reasonable pricing would be impossible given such terms of business and that's probably why you don't see many of these fake FAB houses

Maybe Secret Labs could start such an exact replica of a real FAB house for us all to use?

[remotewizard]

I think you're on to something. They'd have to keep changing the name and the URL to keep us fooled, but it's certainly doable. And it would have the added benefit of forcing the real FAB folks to offer good service at a reasonable price, lest someone think them as fake.

[hanzibal]

Good point!

[remotewizard]

I think I've fixed all the problems with the schematic, and added the pullup resistors (see attached updated schematic). Now I'll work on the routing and groundplane. Wish me luck!

[remotewizard]

It would have helped if I'd actually atached the schematic. Sigh.

Attached Files

•  TDA7313_Schematic.zip   38.15KB   0 downloads

[remotewizard]

A modestly updated attempt, with a ground plane and everything. It's a mess. But it's a start. Perhaps I don't even need a ground plane for a project like this? I'd certainly prefer to keep it single-sided.

Attached Files

•  TDA7313-TestBoard2.jpg   692.69KB   33 downloads
•  TDA7313.zip   51.74KB   1 downloads

[hanzibal]

If I'm not mistaken, your groundplane is broken on quite a few places, meaning you got isolated pieces of groundplane not actually connected to ground. See the red markings in this picture:  broken_gp.png   482.21KB   26 downloads If you run the ERC on the layout, you should get alerts of where the islands are located so don't just go by my markings above since I could have missed places. Easyiest way to fix this is probably to add a second grounplane on the back which you then connect to each top island respectively using one or more vias. Vias are small copper coated holes in the pcb that make a connection between the top and back. Naturally, you could also skip grounplanes all together and just run a big fat ground trace around the board to each spot you need ground. EDIT: Btw, you can acutally see unrouted (disconnected bits and pieces) as tiny yellowish "air traces" in the layout. They can be quite hard to spot at times since, sadly Eagle doesn't really highlight them which is a something of mystery to me.

[Geancarlo2]

You should also make wider power traces and if you are making it 2-layer, make a Vcc plane/pour to make routing easier and reduce noise.

[remotewizard]

I was hoping to keep it on one layer so I could etch it myself. But one way or the other, it's obviously going to end up with two, so I might as well do it right. Thanks to both of you for the feedback.

[CW2]

IMHO it should be possible to make it on single layer, you can always add a jumper wire where necessary. For example, you can avoid all vias from U1 pins 16 - 21 by routing the trace that goes to pin 26 from inside, i.e. under the IC package between pins 15 and 16 and then back between pins 21 and 22, or better yet connect it directly to the other trace that goes from the connector to pin 26. Also, sometimes it helps to rearrange connector pins, if they are not fixed by any specification or so.

[hanzibal]

If you can fit your components on 50x50 mm you get 10 x boards (2-layer) for a total of only 10 USD over at iTead Studios:
http://imall.iteadst...rototyping.html
If you need 100x100 mm you get 10 x boards for a total of 25 USD. Huge value for money and you won't have to do the etching.

[remotewizard]

CW2: That's a good idea about the jumper wire. I'll give it a try hanzibal: For that price, I might just try. I'm pretty sure I could get it down to 100x100 and still leave enough spave for my sloppy soldering. If I do, I'd be glad to give away 7 or 8 of the boards for the cost of postage, if anyone would like to play with the TDA7313 at home. Speaking of which: the TDA7313 is a DIP-28 package (easy to solder), but it's wide. Do you know of a socket that would fit the TDA7313? I only have one working chip for the moment, and don't want to fry it when assembling the board.

Attached Files

•  DIP28-1.gif   19.26KB   9 downloads
•  DIP28-2.gif   11.16KB   11 downloads

[CW2]

The DIP 28 socket (600 mils) should be available at popular electronics websites, a quick search returns for example Jameco, Digikey, Mouser etc. You should be able to get them in a local electronics store too...or eBay...

[remotewizard]

Didn't see it at Jameco (where I usually buy pieces and parts) - I'll look again. Thanks!

[remotewizard]

Anothert attempt, somewhat less horrible than the last. I also reduced the size of the board to meet the specs for iTead. It seems to pass all the rule checks and such; I guess we'll see.

Attached Files

•  Route2.png   25.25KB   32 downloads
•  Eagle Attempt.zip   50.36KB   5 downloads

[remotewizard]

BTW: does anyone know which end is the 'front' on the SparkFun screw terminals?

[hanzibal]

I think it's starting to look real good.

About power line thickness mentioned by Geancarlo2, I don't know what current your board'll be pulling from the power supply but there's this calculator for trace thickness based on current and heat dissipation that you might want to check out:
http://circuitcalcul...dth-calculator/

About the screw-terminals, according the the d/s, I believe you got them turned the wrong way facing inwards. If you look at the d/s, there's a little slope on the long side that faces the screws but you got these slopes directed inwards instead of towards the outer perimeter of the board:
http://www.sparkfun....minal-3.5mm.pdf

EDIT: I first misread the d/s and corrected the post accordingly.