Prop PCB

Cenlasoft · 2009-10-19 19:04

Hello,
I have just finished the PCB for my Eddy Current Analyzer and would like to ask if some of you would look at it and see if there are any problems with the PCB. I used the 40 pin prop. I hope I didn't make any big errors. I used ExpressPCB. I provided a bitmap as well.
Thank You,
Curtis

Sapieha · 2009-10-19 19:18

Hi Cenlasoft

If posible ... Not use any 90'' angles on traces

Only traces that conenct to other can have 90'' angles

▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
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

Phil Pilgrim (PhiPi) · 2009-10-19 19:39

I don't see any bypass caps. You need one 0.1uF ceramic bypass cap next to each Vdd/Vss pair. For the Prop chip itself, it wouldn't hurt to increase this to 0.22uF or 0.47uF. Also, the traces that provide power to the various ICs need to be thicker. With a ground plane, you still need to pay attention to how the ground currents get back to the supply. The ground connection to C3, for example is in a fairly isolated part of the ground plane, rendering it less effective for filtering. This could easily be remedied by using the other side of the board for your signal traces so they don't break up the ground plane as much. Is there any reason this has to be a single-sided board?

These are just my first impressions. I did not examine the board in enough detail to discover any other issues.

-Phil

Javalin · 2009-10-19 20:09

I'd make your prop plug via's (holes) 1.02 mm or so - the standard size is just too small for a standard header.

Ditto Phil's comments about bypass caps.

For neatness i'd line up the 3.3v and 5v regs, and use the same package cap for both - i.e you have one rectangular and one round.·· Just looks more professional.· I'd add more bypass caps to the regulator input/output too - just for good measure really.

Also - the circuit traces are not straight near C3.· Just looks more professional.

For ease of connection later - consider putting some writing on the board in trace.

Dunno what ADC you're using but otherwise looks ok.

J

WBA Consulting · 2009-10-19 20:13

Add a 6 pin header next to P1-6 and a 4 pin header next to P12-15; you have room. Depending on how you buy the board(s) this will give you easy access to additional I/O pins in case you need to do debugging or just want to make use of leftover fabs for other projects.

▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
Andrew Williams
WBA Consulting
WBA-TH1M Sensirion SHT11 Module
Special Olympics Polar Bear Plunge, Mar 20, 2010

Rayman · 2009-10-19 20:28

Why did you put all the traces on the bottom side? Normally, I like to keep the bottom side as a ground plane and run traces on the top surface, when possible...

Also make sure the tabs on your voltage regulators really are ground...

You do want caps near all the Vdd pins on the Prop chip... Probably need one beside your ADC chip and the EEPROM chip too...

▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
My Prop Info&Apps: ·http://www.rayslogic.com/propeller/propeller.htm

FredBlais · 2009-10-19 21:08

Sapieha said...
Hi Cenlasoft

If posible ... Not use any 90'' angles on traces

Only traces that conenct to other can have 90'' angles

I was reading something that maybe interesting to know.

a book said...
[noparse][[/noparse]...]A look through the references shows that when using high-end network analyzers and time
domain reflectometers to measure the reflection from a 90 degree·corner the effects are evident
(Bogatin, p. 318). However, the frequencies at which the reflections occur are high (into
the upper GHz for traces greater than 50 mils wide and THz for traces less than 10 mils),
and compared to other sources of impedance discontinuities (such as vias) the effects are

insignificant.

·

Cenlasoft · 2009-10-20 01:24

Thanks everyone,
Many great suggestions. The caps on the Vdd, where do you put them? From Vdd to ground? Also great idea in putting headers for extra pins for later. Where should cap go on the EPROM? I'll put the ground plate on bottom and the traces on top.
Thanks,
Curtis

Phil Pilgrim (PhiPi) · 2009-10-20 01:46

Bypass caps go from Vdd to ground. With a ground plane, the closer they are to the IC's Vdd pin the better.

-Phil

Nick McClick · 2009-10-20 02:59

Yeah, everyone always says something about 90 deg traces, but I've never had any problems with them, though it probably results in a cleaner looking design. One question - L1 is supposed to be an inductor?

▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
Gadget Gangster - Share your Electronic Projects

Cenlasoft · 2009-10-20 03:19

Yes L1 is a probe (coil). The coupling reduces or changes the voltage in the coil as it is scanned over a metal artifact. I wrote the software for analyzing the results in the 'Processing' language (processing.org).

Leon · 2009-10-20 09:45

The main reason for avoiding 90 degree track angles is that it makes etching harder - you are more likely to get shorts, especially with narrow tracks and spacing. Mitered tracks look neater, as well.

▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
Amateur radio callsign: G1HSM
Suzuki SV1000S motorcycle

Cenlasoft · 2009-10-20 13:24

Hello,
I have a question on the placement of parts if I have a two sided PCB. If I have the traces on the top and the ground plane on the bottom, do the parts go on the top layer? I hope this is not a stupid question.
Thanks,
Curtis

mctrivia · 2009-10-20 14:51

you can place parts on both sides if you like. but usually a best prictice to keep to 1 side when possible for easier assembly.

The only reason to possibly put parts on the side of the ground plane is if they are susceptible to em interference or would create em interference on the traces.

If using through hole like you are I would place the parts on the side of the ground plane.

▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
propmod_us and propmod_1x1 are in stock. Only $30. PCB available for $5

Want to make projects and have Gadget Gangster sell them for you? propmod-us_ps_sd and propmod-1x1 are now available for use in your Gadget Gangster Projects.

Need to upload large images or movies for use in the forum. you can do so at uploader.propmodule.com for free.

ElectricAye · 2009-10-20 15:02

This is really a question for the other forum members rather than a critical comment: but he's got his voltage regs laying flat. Is this really a good idea especially if he moves his ground plane to the other side? It seems to me that, by laying them flat, he's losing his ability to cool the regs as efficiently as they would be standing straight up. I don't know what his current requirements are, but in case they're high, could the regs over heat when screwed down like that?

Again, this is meant as a question, not an "answer".

thanks,
Mark

mctrivia · 2009-10-20 15:32

laying flat depends on lots of things.

1) What is current requirement and how much heat will be generated.
2) is he planning to use heat sinks. They are made for D2 Pack and press on for ics.
3) how big is coper trace under heat sink.

With surface mount parts my regulators are always layed down. I usually use switching regulators for any voltage drop greater then 3v so my heat is usually not that big. Also I make sure I have a large copper trace underneath the regulators heat sink tab usually on both sides of the pcb but not on inner layers.

▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
propmod_us and propmod_1x1 are in stock. Only $30. PCB available for $5

Want to make projects and have Gadget Gangster sell them for you? propmod-us_ps_sd and propmod-1x1 are now available for use in your Gadget Gangster Projects.

Need to upload large images or movies for use in the forum. you can do so at uploader.propmodule.com for free.

Phil Pilgrim (PhiPi) · 2009-10-20 15:43

If the ground plane is on the bottom, it's easy enough to add smaller ground planes on the top undrneath the Vregs with a grid of connecting vias to the bottom for heat transfer.

Which side to put the ground plane on is a toss up, I think, if you're having the board made with a solder mask. Without a solder mask, you have to consider where the potential for shorts is greatest and avoid that side. On top, there's the risk of parts shorting against a bare metal ground plane. On the bottom, there's a risk of creating shorts from solder bridges.

If you use SMDs atop a two-sided board, though, putting the ground plane on the bottom is the only sane choice.

-Phil

Cenlasoft · 2009-10-20 16:20

Thanks everyone,

I really learning from you experts. I have made a few changes. I put a header to have access to three pins in case I need them, I put a 2 pin header for 5V and one for 3.3 V, and I put a cap (C6) on Vdd of prop chip. Let me know if these changes are OK?

Curtis

mctrivia · 2009-10-20 18:24

There should be a cap for each vdd of every chip

▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔▔
propmod_us and propmod_1x1 are in stock. Only $30. PCB available for $5

Want to make projects and have Gadget Gangster sell them for you? propmod-us_ps_sd and propmod-1x1 are now available for use in your Gadget Gangster Projects.

Need to upload large images or movies for use in the forum. you can do so at uploader.propmodule.com for free.

Prop PCB

Comments