PDA

View Full Version : First Board Design



Sal Ammoniac
12-16-2009, 07:54 AM
I'm working on my first hardware design from scratch and have a first draft schematic and board layout completed. I'd appreciate any feedback on both the design and layout.

The design is basically a data logger that collects data from various weather sensors and transmits the data using an Xbee to another computer that processes and graphs the data. Most of the sensors are external to this board and connect to it via cables to screw terminal connectors.

Dr_Acula
12-16-2009, 08:10 AM
Wow, you are doing very well for a first design! Even have the power tracks thicker than the data tracks, and the four mounting holes. What program are you using?

If you want to be really fancy, in the settings for the autorouter you can set the minimum space from a via to a pad. If you increase that then the vias don't end up right next to IC pads and there is less likelihood of a solder bridge when you are soldering it up late at night after a glass of wine. Eg look at the reset switch with the two vias right next to that pad.

▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
www.smarthome.viviti.com/propeller (http://www.smarthome.viviti.com/propeller)

Sal Ammoniac
12-16-2009, 08:15 AM
I'm using Eagle. I'll take a look at the via-to-pad spacing and try to increase it (if the program lets me). Thanks for the advice.

One concession I made, because this is a first design for me, was to use DIP components rather than surface mount. I'll try SMT on a later board.

Erik Friesen
12-16-2009, 08:18 AM
You really ought to implement a ground plane.

mpark
12-16-2009, 08:19 AM
I've been compiling pcb design tips. Check out this page and let me know if it it helps:
propeller.wikispaces.com/pcbdesign (http://propeller.wikispaces.com/pcbdesign)

Dr_Acula
12-16-2009, 08:24 AM
Re vias, it took me a while to find the setting. In DRC which is the button at the bottom on the left or in the Edit menu 'design rules'. Click on the Clearance tab, then work out in that table the via to pad distance (middle bottom of that group of 6). Default is 8mil and you can try 40mil and then reroute.

▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
www.smarthome.viviti.com/propeller (http://www.smarthome.viviti.com/propeller)

Peter Jakacki
12-16-2009, 08:36 AM
Well Sal, placement is everything and you seemed to have thought of this as it shows. It's not at all unusual for layouts to have connectors all over the place and even in the middle of the board so you did well to place them logically around the edge. Another thing to keep in mind is making it fit an OTS box so that you can package your pcb easily when you need to. Your crystal is well placed as this is a sensitive connection and it should be kept as short as possible.

Big word of caution though is to strap the various VSS and VDD tightly together and not circuitously as uneven ground currents has killed more than one Prop on this forum. So make the signal tracks jump around if you have to but make sure the power and ground have top priority.

I see you have screw terminal connections so if you space them correctly you can have them joined in the case of the two 4-way connectors on the left could be butted up together and even replaced with an 8-way. Watch that you don't get too close to the mounting holes as you need room for the head of a screw and the screwdriver if you are going this way. Watch the IDC style pins and mark them well using an unmistakable pin 1 indicator. Much milk has been split by many connecting cables up to these back-to-front.

If Eagle allows you use larger bolder text for the connector labels and even place labels next to the connections. Does Eagle do ground planes? What you want to do is fill up the blank spots with copper connected to the ground (this should be taken into account when routing anyway and there are caveats as always).

Ok, that sums up my 2cents worth.

▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
*Peter*

Sal Ammoniac
12-16-2009, 09:08 AM
Thanks for all the advice.

Erik: I added a ground plane.

Peter: I cleaned up several of the connector labels and added pin 1 designations. I'm not sure if I have all of my VDD and VSS lines tight enough. I have no experience as to what this looks like on a board layout.

Here's an updated image of the layout.

Peter Jakacki
12-16-2009, 09:34 AM
Sal, the decoupling cap on the center left of the Prop has it's ground connection "loose". Route track to pin 15 of the Prop to the left of the cap and the ground plane should make it tight. Failure to do so will make the cap ineffective due to lead inductance. Are you able to pour a small "power-plane" for VDD or thicken up the tracks? Also any place where you don't have to run as close as you do to other pads etc you should give them a bit of extra room just to lessen the likelihood of pcb manufacturing problems.

▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
*Peter*

Nick Mueller
12-16-2009, 03:23 PM
You can get a better copper pour if you adjust some bents to allow the copper to "flow" between (increased) gaps.
Also try to place as much tracks on the non-ground-plane. So the tracks don't cut the ground plane to much. Like in the upper left corner, you could place the diagonal line from the "on off switch" on the top layer. Or from Prop pin #6 goint to the right up: Place more on the top layer, so it doesn't cut through the ground plane that much.
Or if you look at the supply line from the LT1790 to the LM358. If you move that a bit to the right (under the LM358) you'd gain some space.
One technique to improve routing is to click the "info"-icon and select a trace (the power trace for example). It highlights that trace and you can find better routing that way. So many traces are abit confusing. And its a good procedure how have a look at the board in overview (with a trace selected).

HTH,
Nick

▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
Never use force, just go for a bigger hammer!

The DIY Digital-Readout for mills, lathes etc.:
YADRO (http://www.yadro.de)

Ale
12-16-2009, 04:14 PM
I'd add something: If the traces do not have to be .254 mm (.01") for space reasons make them thicker, for example .4 mm (0.16"). Power traces can be even wider, 1mm. The decoupling caps can be even nearer the power pins of the ICs and try to use thicker traces thus reducing the inductance.
Are you sure you need 2 layers ?. Maybe with a few bridges you can get away using 1 layer... and when you are 100 % sure it works you can jump to 2 layers for production.
The middle pin of the regulators is connected to ground, especially if you use the version without a middle pin!
Be sure to have the spaces for your fab right: pad to pad distance, track to track, via diameter.

▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
Visit some of my articles at Propeller Wiki:
MATH on the propeller propeller.wikispaces.com/MATH (http://propeller.wikispaces.com/MATH)
pPropQL: propeller.wikispaces.com/pPropQL (http://propeller.wikispaces.com/pPropQL)
pPropQL020: propeller.wikispaces.com/pPropQL020 (http://propeller.wikispaces.com/pPropQL020)
OMU for the pPropQL/020 propeller.wikispaces.com/OMU (http://propeller.wikispaces.com/OMU)

CassLan
12-16-2009, 09:06 PM
mpark said...
I've been compiling pcb design tips. Check out this page and let me know if it it helps:
propeller.wikispaces.com/pcbdesign (http://propeller.wikispaces.com/pcbdesign)
Thats nice work!

▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔


NYC Area Prop Club (http://www.gothampropclub.com)

Prop Forum Search (Via Google) (http://search.parallax.com/search?site=parallax&client=parallax&output=xml_no_dtd&proxystylesheet=parallax&proxycustom=<HOME/>&ie=&oe=&lr=)

·

Sal Ammoniac
12-17-2009, 02:24 AM
Nick: What are "bents" and how do I adjust them? I have zero prior experience with PCB layout and some of the terms I'm seeing in this thread, such as bents, are way beyond my current experience level.

Sapieha
12-17-2009, 03:33 AM
Hi Sal Ammoniac..

Some TIPS.

Can You have Ground Plane on both sides of PCB around XTal.
That build guard area around XTal pins and XI/XO pins on Propeller.

That give You better stablity on XTall

Regards

▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
Nothing is impossible, there are only different degrees of difficulty.
For every stupid question there is at least one intelligent answer.
Don't guess - ask instead.
If you don't ask you won't know.
If your gonna construct something, make it·as simple as·possible yet as versatile as posible.


Sapieha

Sal Ammoniac
12-17-2009, 08:19 AM
I incorporated most of the suggestions from this thread (wider power and signal tracks, ground plane, and better coupling of the bypass caps to each chip's power and ground) Here's the new version of the layout.

As before, I appreciate any feedback.

wjsteele
12-17-2009, 09:29 AM
The only thing I see that might be a problem is on your LM2940, your VDD has a via that is right next to your Ground pin.· I'd at least move that via to the other side of that pin.

If someone had to hand solder that, they might short out the ground with that via.· Moving it just makes it a little less likely.

Are you, by chance, going to have these printed with a solder mask?

Bill

Peter Jakacki
12-17-2009, 09:35 AM
If it makes the layout any easier then you don't need resistors from the Prop to the inputs of the MCP3204, that's 3 resistors that are redundant and that you can completely do away with.

Some notes about the schematic:
1) Usually the BOE pin is tied low to enable brown-out detect.
2) Include a large input cap on the input supply, around 200uf to 470uf as the regulator is only as good as the input. It's usually a good idea to include a protection diode here as well.
3) Couldn't see it but don't forget to include a 10uf tant on the 3.3V supply somewhere.
4) Include a pullup on P31 in case your software activates a serial port and the input is disconnected.
5) Technically you don't need it but the reset line can pick up glitches via the prop plug so keep this in mind (cutout switch maybe).

Don't worry about getting it perfect either as you could spend a long time getting it just right when you could already have learnt a lot and be onto revision 1,2 etc. Besides even when you get it perfect there is still something you want to change later on.

▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
*Peter*

Sal Ammoniac
01-16-2010, 05:51 AM
Thanks again to everyone offering advice. I got the boards made over the Christmas holidays and finished assembling them today.

Amazingly, everything worked the first time without me having to make any changes to the board. I don't know if this is an indication of my prowess as a board designer, or sheer dumb luck.

CassLan
01-16-2010, 10:33 AM
They look very nice, glad you had a successful first run. Do you mind sharing where they were made and maybe a rough estimate of cost?

▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔


NYC Area Prop Club (http://www.gothampropclub.com)

Prop Forum Search (Via Google) (http://search.parallax.com/search?site=parallax&client=parallax&output=xml_no_dtd&proxystylesheet=parallax&proxycustom=<HOME/>&ie=&oe=&lr=)

·

Sal Ammoniac
01-16-2010, 12:41 PM
I got them done by Imagineering (www.pcbnet.com/default.asp (http://www.pcbnet.com/default.asp)). They have a new customer introductory offer of $25 for a 2-layer board (up to 60 sq. in.), so I got two boards for $50 (plus about $8 for shipping)