First PCB Design Suggestions?

[jacob84401]

Hello all,

I am a Mechanical Engineer but have recently got hooked on electronics.  I really don't have any formal training in electronics but I am willing to dig in and learn.

Attached are several pictures of a pcb I've designed.  The information used to design this board has come from a lot of reading and youtube watching.  I am quite certain that all the connections are correct but I would like to know if I have missed some rule or good practice that I don't know about (yet).  Do you have any suggestions?

I place a lot of vias around the outside to link my two ground pours together.  Is it enough, too much?  This board is a SIM900A module and connected to a atmega328P 28PDIP package.  I am planning on using maker studios http://makerstudio.cc/index.php?main_page=product_info&cPath=8&products_id=14 to make the board.

Thanks for your help in advance.
Please let me know if you would like more information I can post more if needed.

[ludzinc]

First tip - the SIM900 can be a hungry beast, and you need to improve power to it.  Lots of decoupling, fat tracks and all that.

Some lessons I learnt can be found here http://ludzinc.blogspot.com.au/2013/09/finishing-up.html.

[Leopoldo]

there are a few 90° bend...I'm not an expert but I think there shouldn't be any.

[katzohki]

Looks ok. I'm not a PCB expert, but it looks good as long as you're not running any high frequency data or analog signals. Couldn't hurt to add a schematic for us to look at.

Also do fatten up the power lines since you have the room. By the way, just to give you another option, I use Seed Studio: http://www.seeedstudio.com/service/index.php?r=pcb

What is the dotted red line going all the way around the PCB???

[Mr.B]

What is the dotted red line going all the way around the PCB???

Polygon pour.


As said above, you need to fatten up those power supply tracks.

[katzohki]

What is the dotted red line going all the way around the PCB???

Polygon pour.


As said above, you need to fatten up those power supply tracks.

It looks like the end result will be a jagged edge on the pour.

[eejake52]

When you connect a crystal - try to make both traces equal length. Turn Q2 by 90 degrees.

Capacitors C4 and C3 should probably connect to ground, but unless you have some vias that I can't see, they appear to be open on one side. Are you using Eagle? and if so, did you run the Electrical Rule Check? and the Design Rule Check?

Jake

[Mr.B]

It looks like the end result will be a jagged edge on the pour.

I am not sure if it is Eagle, but it looks like it.
It is just the way Eagle displays it in the editor.
The Gerbers don't come out like that.

Although... It does look a little like it may be a second polygon on layer 1 without a solid pour.
I just checked one of my designs and it doesn't look like that after the 'pour'.

[jacob84401]

Wow guys you all have given some great advice.

The red and blue dotted lines represent polygons on the first and second layers.  There are many components that are connected to ground through the two pours.  eejake52 C2 and C3 are connected to ground through the pour.  Also good call on rotating the crystal 90 degrees.  I read that somewhere but I forgot about it.

I got rid of all the 90 degree traces (I think).  Just because I am trying to learn, why not 90.  I'll stick with 45 because it looks nicer but why is it important.  I took all the power tracks and made them all 25mil.

Do you have any more suggestions?  Attached is the next iteration. 

Thanks Again

I know that the topic is off for this part but I have come to find I can't find an inductor (L1) that will work with my power supply.  I one that can take 3 amps.  (2amps peak supposedly)  Where might I find one, I have everything else.   See here for more info on my power setup

[ludzinc]

You need a *LOT* more decoupling on the SIM900 - see my comment above.

But to be specific, I found it needed 2700uF on the 4V rail.  That's a big cap...

Otherwise the 4V rail will dip, the SIM900 will reset and you will be wondering why the damn thing doesn't work.

[LukeW]

In theory you should be controlling the 50 ohm impedance of the line to the antenna, but if you keep the SMA connector as close as possible to the module and just keep the track straight then it will be probably be fine and you don't have to worry about learning microstrip impedance design.

[jacob84401]

You need a *LOT* more decoupling on the SIM900 - see my comment above.

But to be specific, I found it needed 2700uF on the 4V rail.  That's a big cap...

Otherwise the 4V rail will dip, the SIM900 will reset and you will be wondering why the damn thing doesn't work.

Oh yes, I will switch the output cap for a larger one.  I am having a hard time finding the footprints for electrolytic cap is there a standard for them?...  Say for something like http://www.taydaelectronics.com/capacitors/electrolytic-capacitors/2200uf-16v-105c-radial-electrolytic-capacitor-12x20mm.html

[jacob84401]

In theory you should be controlling the 50 ohm impedance of the line to the antenna, but if you keep the SMA connector as close as possible to the module and just keep the track straight then it will be probably be fine and you don't have to worry about learning microstrip impedance design.

That is what I am banking on.  From what I have found online I should be fine.

[Codemonkey]

As well as beefing up the power supply lines, I would also scatter more GND stitching vias around, especially near the RF module (not at the edge of the board, just randomly near and also under the module but generally all over the board). Also make sure that when you generate your gerbers that you opt for solder resist on the vias so that any vias under the module won't short with any exposed connections under the module since it appears to have some test points or something under there.

GCPrevue (free download) is a good gerber viewer that can be used to check everything is ok before you send them off.

[ConnorGames]

Looks like you've still got some airwires -- Might want to connect those up!
You might simplify routing by putting U6 above U5, or might not. I don't know hat U5 or U6 are, but it's probably not a big deal.
You have a lot of traces that are much smaller than they need to be, making them wider will reduce inductance and make the board more manufacturable at no cost.
I don't know too much about via stitching, but it seems like some vias under the AtMega might be a good idea. Also add a decoupling cap for the AtMega.
Most importantly, you NEED a big cap for that SIM900!

EDIT: just realized that U10 is an LM2596. I think this switcher layout probably needs work, but I'll leave that up to the switcher experts on this forum

[katzohki]

Footprints for through hole components aren't necessarily well defined, but if you look at the data sheet you should be able to figure it out based on the lead spacing of your part. Common practice is to put a square pad for positive terminal I think.

[jacob84401]

First tip - the SIM900 can be a hungry beast, and you need to improve power to it.  Lots of decoupling, fat tracks and all that.

Some lessons I learnt can be found here http://ludzinc.blogspot.com.au/2013/09/finishing-up.html.

Ludzinc,

I have read your blog on your sim900 alarm project and if I could I would love to learn from your frustrating problems with your power supply.

I am using the suggested LM2596-adj
I see the need for the large capicitor, I am planning on using a 3300uF cap just to be safe.  In your blog you mention using a small fast 100nF cap close to the power input to the sim900.  Do you still consider this to be a good idea?

I have been trying to find an inductor that will work.  You say that because your large cap is taking the brunt of the high current demand your inductor doesn't need to be so massive.  I have been trying to find a 3Amp capable inductor only to find that they are bulky, ugly, and relatively expensive.  If I could go smaller (or get rid of it? (Unlikely?)) I definitely want to.  What did you end up going with?

Edit:  I looked at the peak current timing the 2 amp peaks come in every 4615 uSec for a duration of 577uSec.  This gives a duty cycle of 12.5%.  So does that mean that I only need an inductor that can handle 0.125*2amps=250mA or to be safe say 370mA?

[ludzinc]

These:

http://www.aliexpress.com/item/Free-Shipping-20pcs-lot-Shielded-Inductor-SMD-Power-Inductors-cd127-33uh-330-marking-12-12-7MM/1983148094.html

Yes you need the smaller cap (as close to the SIM900) as possible.  The 100nF can respond to the voltage dip faster than the 3300uF.

[zapta]

1. For PCB price comparisons you may want to check here http://pcbshopper.com. Plastic stencils are available at oshstencils.com.

2. Add labeling for board name and version  (chances are this is not your last version ;-))

3. Many traces are skinny for no reason. Whenever possible, don't design for the PCB vendor minimal trace width. Same for silkscreen label size. This board has plenty of space.

4. Slight rounding of the corners removes the sharpness.