Board Questions - Page 1
Forum section: electronics / general

author: ahnuts72
author_rank: Regular Contributor
timestamp: January 26, 2013, 03:43:21 am
content: Can you guys tell me what you think of my board layout and all.I've done a few small lm386 amp boards but this is a bit more crowded.It is a hf upconverter schematic by Paulino Sato i found on the net for my rtl-sdr receiver.Since i already had the TA7358 and the 50 Mhz crystal in my junk box i thought i would build it.Any obvious problems you see?

author: andersendr
author_rank: Regular Contributor
timestamp: January 26, 2013, 11:44:49 pm
content: Really the only suggestion I would have is to make the traces bigger. Especially if you are planning to home etch this. One thing you could look over is the component placement. For example, C14 could be moved above Y1 to cut down on trace length.

author: jeroen74
author_rank: Frequent Contributor
timestamp: January 26, 2013, 11:54:22 pm
content: It can be much more compact and and it needs a good tidy up; bigger traces as suggested and traces erminating neatly into the centre of a pad, not on the edge. Better component placement that makes routing easier. Align components neatly.

author: tinhead
author_rank: Super Contributor
timestamp: January 27, 2013, 12:03:45 am
content: C14, with how it's connected now, have no functionC6 and C7 are for reason, they now almost (especially C7) without any reason there.C2 should be near pin2, no 10km awayC9 have is useless as well (you have to think about why these caps need to be there)VHF_OUT is, almost ok (avoid these Y tracks)HF_IN is completly wrongAnd btw, your schematic, ehm, why not like?in -> amp -> outclock

author: free_electron
author_rank: Super Contributor
timestamp: January 27, 2013, 12:21:14 am
content: am i the only one that sees serious problems ?-this is an RF design. WHERE IS YOUR SLAB OF COPPER ?-in and out next to each other.-massively oversized components. ( caps are way smaller footprint than that ... and inductors dont look like resistors... )- you can easily get rid of the two traces that run inbetween the chip pins ...

author: ahnuts72
author_rank: Regular Contributor
timestamp: January 27, 2013, 01:24:35 am
content: I left the copper pour out in the picture but i plan on using it when i etch the board.For the other stuff i just followed his component layout best i could.Like i said first board with this many components I've done.I could spend 60-70 dollars and buy one but i had the stuff so thought i would try to build it.Most of the stuff I've built has been audio stuff like headphone amps,distortion boxes for my guitar.The inductor footprint is the one that shows up in diptrace the schematic symbol is right but that's the pattern it uses.The cap pattern was my fault but i have changed them to a smaller footprint.

author: marshallh
author_rank: Unknown
timestamp: January 27, 2013, 02:55:50 am
content: A ground fill is going to have some, but not much improvement over your existing maze of routes. It's no good if it's sliced up beyond recognition.Consider ditching your pcb entirely and dead bug all your components on a copper clad pcb. Use smallest components feasible to minimize parasitics, arrange connections in a logical manner, compact the size down as much as you can.http://www.qrp.pops.net/ugly.asp

author: ahnuts72
author_rank: Regular Contributor
timestamp: January 27, 2013, 05:15:51 am
content: I thought about doing it dead bug but this gives me a chance to brush up on making pcb's and practicing with Diptrace but if it comes down to it i may.Here's the revised sch and board I know its not perfect but I'm trying to learn something a little more complicated thanthe little batt powered amps i was building.And don't worry about hurting my feelings with your comments,a lot of you guy's know a lot more than me.I have no problemsaccepting constructive criticism.

author: marshallh
author_rank: Unknown
timestamp: January 27, 2013, 06:13:00 am
content: Build it, and see how it works... and then revise the design and try it again.Read these links to learn more about why board routing, part packages (specifically through hole versus even large smd), their associated parasitics and even things like part orientation will affect your circuit.http://advantage-dev.com/services/pcb-layout-examples.html#rfwirelesshttps://www.jlab.org/accel/eecad/pdf/050rfdesign.pdfhttp://www.semtech.com/images/datasheet/rf_design_guidelines_semtech.pdfhttp://www.eeweb.com/blog/circuit_projects/basic-concepts-of-designing-an-rf-pcb-boardhttp://www.maximintegrated.com/app-notes/index.mvp/id/4636If you can understand the principles behind these you will have a head start on even many digital pcb designers.Here's one that shows promise:http://3.bp.blogspot.com/-TY0KZIwLbD8/UFG0ZSLzjPI/AAAAAAAABx8/ht2exE6Tp88/s1600/UP100-coils.JPGThere is a reason for almost everything being a certain way on there, like the side-mounted SMA connectors (through-hole connectors with the signal coming out on the top layer will have a small stub formed by the rest of the connector pin poking through the pcb and acts like an antenna)

author: free_electron
author_rank: Super Contributor
timestamp: January 27, 2013, 06:41:49 am
content: It looks from the way you do your layout that you don't understand the signal path in this circuit, nor how it works, nor what the function of the various elemnts is.Before making a board those things are key. Especially rf boards.Lets take a look at a section of your board. Bottom right L6 L7 L8 c17 c18 c19 c20 and c21 and the hf in connector.This is an incoming signal going through a filter. The signal path runs through the inductors. The capacitors to ground form the filter in combination with the inductors. Any additional stray capacitance you introduce is going to affect the frequency response of this filter. As you are dealing with capacitors in the pf range the influence of the board is going to be big here.So theres a couple of things you want to do :keep the copper as far away from the signal path as possible to reduce stray capacitance.Keep the flow of electricity logical. You do not want to 'contaminate' the signal that comes out of the filter by running it right next to another signal. Like the output of that oscillator module...You sort of got it right for my second point but you mess up big time on the first point.Look at c21 for example. Rotate that thing 90 degrees and do not run ground between its pins.Also rotate c19 c18 and c17 90 degrees and keep ground away from the nodes between inductors.Your pcb layout should be almost exactly like you have drawn those components in your schematic.Run a single ground ring around that block . And take a good look first at your actual components you will use. I doubt they will fit those footprints.Knowing this, let's take a look at the left section of the board. Another one of these filters. Apply the same technique. Arrange stuf logically.Look at c2 why coonecting to ground by going up.. You have ground immediately down...move c2 to the right of the chip and connect to ground there. Rotate y2 180 degrees so its output lays on top. Build its output filter logically working from the oscillator towards the ic.If i got 5 minutes tomorrow ill draw you a floorplan. But start by following the hints i give you here.This thing can be laid out without a single crossing or a single trace inbetween the ic pins

author: ahnuts72
author_rank: Regular Contributor
timestamp: January 27, 2013, 07:10:31 am
content: Thanks for the links marshallh I'll definitely check them out.Thank you free_electron for showing me some examples on the board to look at.I was just following the layout he had for the board.I kinda understand each part if i break it down into blocks like the low pass filter and the high pass filter.The oscillator and even the mixer I've read the datasheets for,but like free_electron said putting them togetherin a semi compact form so they don't effect each other and the best way to do the ground fill is where i fall on my face.I've just started getting back into this stuff after about 10 years maybe I'm getting ahead of myself.

author: ahnuts72
author_rank: Regular Contributor
timestamp: January 27, 2013, 12:39:09 pm
content: Here's the next version.Still having trouble with ic pin 3 to r1

author: ahnuts72
author_rank: Regular Contributor
timestamp: January 28, 2013, 09:06:35 am
content: A few more changesI'm still having trouble getting ic pin 3 to r1 and staying away from the highpass filterand getting rid of the last few crossings.Just wanna get some of your professional opinions if I'm going in the right directionor made it worse.

author: marshallh
author_rank: Unknown
timestamp: January 28, 2013, 11:10:05 pm
content: Here is my interpretation. Input from pros welcome.You can get this board made for super cheap at some batch service like oshpark or batchpcb. Everything is on the top layer.You don't have to order all SMD parts. You can use through hole parts just fine, but DO clip the leads short as physically possible, and just solder them on the top pads.Eagle files and gerbers are attached

author: ahnuts72
author_rank: Regular Contributor
timestamp: January 28, 2013, 11:35:44 pm
content: Must have been posting same time as you MarshallhI hate uploading photos to a file host takes me forever.That was my first thought when i found this sch till i found the mixer and crystal in my junk boxThought it might be a good way to get some practice with my layout and routing with a little help from the pros.Something a bit more complicated than my other circuits.I hate asking dumb questions that are prob obvious to alot of you guysand i know how aggravating it can get.Thank you for the eagle files i really appreciate that and I may end up using themi just figured for a one off board it would be cheaper and I would learn something in the process.Next attempt.This board was manual routing I auto routed the others.

author: c4757p
author_rank: Super Contributor
timestamp: January 29, 2013, 12:08:12 am
content: Forgive me if I'm wrong, marshallh - I have no RF experience whatsoever - but wouldn't you want to keep the ground pour out from directly around the filters? Those are some small capacitors, I think I would want to control the capacitance to ground more tightly in that area.

author: ahnuts72
author_rank: Regular Contributor
timestamp: January 30, 2013, 01:06:34 am
content: Ok not gonna post anymore pics.Whether I build this board,buy one already madeor use marshallh's eagle files which i really appreciate who knows.I mainly did this to work on my layout and i thought no better place than the eevblogto get some professional tips or advice.So for the minute lets forget this is about building the boardand ask if the layout has improved since the first post.