PCB Critique

Go To Last Post
22 posts / 0 new
Author
Message
#1
  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Hello Everyone,

My name is tkdcompdude and I am working with rwcjunglist on a project for school. We are developing PCB's for the project and I was wondering if anyone or would it be consider okay to have a critique of the PCB before we send it to out to be manufactured. Like I said since no one our team had prior experience in this field we are constantly learning how to use Eagle and also how to design a PCB. I should be able to have something up by tomorrow morning if this is okay. Thanks.

tkd

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

there was a thread recently by Alank asking the same thing. You might want to have a look at that for suggetions. His board started out crap and ended up near production quality.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Quote:
My name is tkdcompdude and I am working with rwcjunglist
WOW what were your parents thinking when they gave you those names. :shock:

John Samperi

Ampertronics Pty. Ltd.

www.ampertronics.com.au

* Electronic Design * Custom Products * Contract Assembly

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Off-topic:

js wrote:
Quote:
My name is tkdcompdude and I am working with rwcjunglist
WOW what were your parents thinking when they gave you those names. :shock:
There is a photo blog out there I sometimes visit to get a few giggles http://myparentswereawesome.tumb... After you've seen those parents you know where such names came from :-)

On-Topic, to the OP:

Just do us a favor. When you submit your homework, be honest and tell your teacher, teaching assistant, professor that you did get some external help and the amount you got. Your schools has probably more about how to do this in their academic conduct, academic dishonesty or similar rules.

Stealing Proteus doesn't make you an engineer.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

tkdcompdude wrote:
Hello Everyone,

My name is tkdcompdude and I am working with rwcjunglist on a project for school. We are developing PCB's for the project and I was wondering if anyone or would it be consider okay to have a critique of the PCB before we send it to out to be manufactured. Like I said since no one our team had prior experience in this field

Man, have you got a bad memory. Third sentence and already you think that you have told us that you have no pcb experience. How do you manage to remember the spelling of your name? :lol:

Ross McKenzie ValuSoft Melbourne Australia

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Hello everyone. As for the names posted those our handles on this website. As for academic integrity this is not a HW assignment; it is for our senior project. Since we had no experience and have no one to turn to right now I figured I'd try here. As for dealing with this situation the one's that assist in this process are referenced for their assistance in our final report. As for my last comment, I apologize for the misunderstanding and repetition of this. My sleep pattern this semester has been so varying that sometimes structuring a good sentence and avoiding repetition happens. Sorry about that everyone. I will be posting the stuff up later today. Thanks.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Welcome to the site.

If you post an image file then those who do not have Eagle software can also have a look.

Please add a brief description of what your project is all about.

Is this a working prototype? Have you wired it on a breadboard or development board yet, prior to committing to a PCB?

JC

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Sorry for the delay.

The project is for a tangible sequencer and this is for the blocks that the user can move around freely. Basically what you will see in the schematic is a micro controller, Zig-Bee Module, infrared LED's, and supporting capacitors and resistors. Let me know if you need a better description than this. To answer the last part of the question; yes it is.

tkd

Attachment(s): 

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Sounds like a fun project.

A few thoughts:

The voltage regulator needs capacitors on the input and output. See its data sheet.

It may be wise to put a diode in series with the power supply to the regulator. Then if someone hooks up the power backwards it won't fry your project.

The AVR should have a by-pass cap across each V+ & Gnd lead pair. Say a 0.1 uF.

Many would tie an external pull up resistor, ~10K, from the uC reset line to the V+.

Many would consider putting a normally open push button switch on the reset pin, to reset the uC when testing your code.

The XBee appears to be pretty close to the top left mounting hole. Do you have adequate clearance to mount it properly?

I would put a BIG #1, or ">" by the uC's pin #1, and by the ISP header pin #1, and by any other polarized connector.
At 2:00 AM, when I am tired, in a hurry, and behind a deadline, it is easy to hook something up backwards.

Put a name on the top of the PCB, in copper.

Put a version number and a date on the top of the PCB, in copper.

You have lots of room on this board, so I would make your traces wider.

You might want to have room surrounding the voltage regulator for a heat sink, or put a filled plane and an array of vias, under the 78xx as a heat sink.
You can put a filled pad on the top and bottom, extending a bit beyound the 78xx outline. Put in a bunch of vias to carry heat from the top to the bottom filled plane.

ERROR:
Your External Crystal is not hooked up properly.
Look at ATMEL Application Note 042. AVR042: AVR Hardware Design Considerations

The leads from the Xtal go to the Xtal pins on the uC. Each pin also has a cap to ground. The Xtal does NOT connect to the uC through the caps.

You would like the connections from the uC to the Xtal to be as short as possible.

Some would put a filled ground plane under the Xtal, and NOT run any lines under the Xtal.

You have plenty of spare uC I/O pins available.

You may want to consider using an I/O line to control the Reset of the XBee. This lets you have software control of it.

When debugging it is very useful to have an LED on the XBee RSSI, and perhaps on a few other pins.

Move the stuff away from the ISP header. The plastic head on the 6-Pin cable takes up a fair amount of room. You do not want it blocked by the LED or JP4.

++++++++++
What voltage are you running at?
++++++++++

Note that the XBee's are 3 V devices. You would like to run your uC at 3 V to make the connections simple.

LOOK VERY CLOSELY at the pin out for the 3-terminal regulators. The 5V and 3V units can have DIFFERENT PINOUTs.

I would add a spare Gnd pad for a scope probe. I would also put a spare I/O pin to a pad for a scope probe.

As I noted, it looks like a fun project. Hopefully a few of the above suggestions will be of benefit to you.

JC

Edited lots of typos...

Edited #2:

Error:

I think you also need to look CLOSELY at the ISP 6-Pin Header layout. It is shown in the Application Note 042 I linked to above. Note that the application note shows a TOP DOWN view. I think your signals may not be in the correct location for a "Standard" AVR programmer.

Edit #3:
You mentioned using IR LEDs. You may want to put some visible LEDs on your PCB, also. You have plenty of spare pins to do so. It can be a great help when debugging code to turn on a visible led when you flash your IR LED, or have one blinking once a second by an ISR as a "Heart Beat" to show the circuit is up and running.

JC

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Currently that's a pretty poor layout. Be prepared to give it a fair few more goes before you will get much positive feedback.

This version has poor grounding, poor layout and has a serious lack of decoupling and bulk capacitors.

You should spend some time looking at other pcbs from computer parts and things like that to get some better ideas for layout style.

You should spend some time looking at other schematics in application notes to get some better ideas for the circuit requirements.

The tracking you have used is all way too small, especially given the amount of pcb space you have to work with.

On the schematic side of things, some notes about input voltages and things like that would help us understand the application more. Why is the '+' on the header tied to ground?

Sorry to sound so critical, just trying to give some tough love.

oddbudman

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Thanks guys for your assistance so help so far. I will work on getting those changes/suggestions in place in the coming days. I will not be able to touch this for a few days due to a midterm I have early next week and this will take most of my time. I will then report back here once that is done and I have completed the things you had talked about. Thanks again.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

In addition to what was mentioned, there are a few stylistic issues with the schematic:

- Don't skimp on power/gnd symbols. It would be easier to follow if you use additional gnd symbols, for example, rather than traces that all lead back to the single ground symbol you have.

- Don't have any 4-way connections, like the one at the regulator's ground pin. If you have them, an extra or missing connection dot will be hard to find.

- The trace from U5 pin 9 to u$4 pin 2 shouldn't be on top of the ground lead for JP8 (this is an example of the two issues above...)

- What's up with the refdes? Some are U5, others U$4

- The schematic symbol used for the phototransistor is an LED. The arrows should go the other way.

- Any way to turn off the '+' centroid marks? They cause confusion; see JP1 with the '+' on the ground pin

Also, you can't do 16 MHz on most Atmel processors on 3.3V; the Atmega324 maxes out at 10MHz for 3.3v. If you really need the higher speed, you will have to run it on 5v and level-shift the lines going to the xbee

/mike

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Hey guys,

David here, Paul (tkdcompdude)'s partner on this project. First, I'd like to thank everyone for their feedback. We over looked quite a few things. We looked at APP NOTE 042 for hooking up ISP lines but I didn't bother to read the rest of it, there was the first mistake. Anyhow, I have attached the new schematics, PCB soon to follow. If you want more details about our project check out the link below.

We got the idea here:
http://www.youtube.com/watch?v=F...

The difference with our project is that it works standalone, without the computer. What we have posted here is the slave block (the blocks with the buttons).

Attachment(s): 

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Much better!

Your capacitors are draw backwards, the straight bar is the + side of the caps.

As I mentioned earlier, debugging a XBee project will be much easier if you add LEDs for RSSI, (D10); and XBee Assoc, (D5).

Good Luck with your project!

JC

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

David/Paul,

You have C1 is series with the DC input. It will block DC ...

Cheers,

Ross

Ross McKenzie ValuSoft Melbourne Australia

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

The output from the voltage regulator is not connected to the positive rail and/or the capacitor - there's no blob and there should be.

And as Ross has pointed out, you need to take the power input to the other side of the 10u capacitor.

Neil

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Here are a few:

Add a capacitor to the AREF in the case you need to make analog measurements. Also consider a chip inductor or small resistor for improved filtering on AVCC, and a jumper to connect to AREF if desired. There is good information in Atmel application notes for this.

Consider the use of a different crystal value to achieve standard baud rates with less error. The cap values of 15pf and 16pf might be too small.

Perhaps consider a prototype area with a means to use unused pins, in future projects. Or consider a package with fewer pins.

It all starts with a mental vision.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Here are some things that I have found VERY useful when using Eagle:

    * Learn to use buses. Those make the schematic very easy to follow and it does not become lot worse if/when the schematic gets more complex.

    * Learn how to name wires and attach labels on them. This makes it easier to check Your schematic visually. One more countermeasure against human errors.

    * Learn how to use the Electrical rule check. Make the schematic so that it runs without errors and preferably also without warnings.

I attach a sample schematic I have made with Eagle. I am NOT telling that it is a perfect one. Some may get really sick by just looking my transistor symbols... I show it here to visualize what I mean by buses and labels. IMHO that is one of the greatest features in Eagle.

To put labels inside a bus just name it like:
BUSNAME:label1,label2,label3,...labeln

After that You can connect any of the labels by using the correct tool - at least try it out - it WILL save You from wire mixups and horrible errors.

Attachment(s): 

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Hello everyone,

I have finally been able to resume work on the PCB layout again and I had some questions. When you do ground planes where and what should I look for when making these provided you see what David did on the latest version of the schematic? You can either give me advice or a tutorial that explains this well would be greatly appreciated. Then from there I should be able to get another revision of the PCB layout up afterward. Thanks again for your help.

Paul

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

This is how I like mine... Tight, compact, and well ordered.

Attachment(s): 

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Here's our new schematic. PCB layout should follow next week. Thanks again to all. Everyone has been a great help!

David

edit: new version

Attachment(s): 

Last Edited: Mon. Oct 26, 2009 - 11:10 PM
  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

You still have a couple of capacitors drawn backward, on the crystal, and on AREF. The curved side should go to GND.

I can't quite figure out what you are doing with AREF. The capacitor which was mentioned before should simply go from AREF to GND. With the capacitor in place, the reference voltage can be selected in software.

Michael