PCB Design help

Discussion in 'The Projects Forum' started by Vanush, Sep 28, 2011.

  1. Vanush

    Thread Starter Active Member

    Apr 19, 2008
    46
    0
  2. nerdegutta

    Moderator

    Dec 15, 2009
    2,515
    785
  3. debjit625

    Well-Known Member

    Apr 17, 2010
    790
    186
    From Edit menu or Command Toolbar select "Change" command and select "Width" and use the width you want and then click over the trace.But in the pdf its not just a wide trace rather its a plane normally we do it for ground or power,in Eagle we do it using "Polygon command" ,check the help files.

    Good Luck
     
    Last edited: Sep 28, 2011
  4. SgtWookie

    Expert

    Jul 17, 2007
    22,182
    1,728
    The Polygon tool is very useful for creating such large fill areas. If you want to merge a polygon with a signal or power node, use the NAME tool and give it the same name.

    Use a line width no less than 10 mils. I usually set isolate and spacing to 16 mils.

    Once you place a complete polygon, you can fill the polygon using the Ratsnest command.
     
  5. Vanush

    Thread Starter Active Member

    Apr 19, 2008
    46
    0
    Hello

    Here is my first PCB Design. Some wires are still unrouted but does anyone have any tips...

    http://i.imgur.com/jgiyD.png

    It is a board for an OLED module. Battery (3.7 V) linearly regulated to 3.3 V provides VDD. Vdd for logic is then boosted to ~18 V using a boost converter (FAN5331SX) to provide Vcc. Vcc is then used by the OLED.

    I have tried to breakout the data pins of the OLED (note: no SPI) so they can be controlled by an AVR ATtiny24, whose pins I have also broken out. The reason I've done this is because I believe this will require a lot of debugging, and I intend to connect them with hook up wire. I have also included pins for the AVR ISP Programmer.

    The OLED has a FPC ribbon with contacts having a pitch of 0.75mm, which I created a package for in EAGLE with the smd pads.

    Things I dont get:

    -To get Vcc to the oled pads, I've had to use a via and route it from the bottom. I don't think this is elegant, but will it work?

    -When are you supposed to use via's? I basically just used them when I ran out of space on the top layer?

    -Why does the LM1117T get printed out on the silkscreen layer when it will be 'standing up'?


    - For the Ground plane. On a 2 layer board, are traces at the bottom still acceptable?
    - Can anyone recommend resources on PCB design ?
     
  6. SgtWookie

    Expert

    Jul 17, 2007
    22,182
    1,728
    Why don't you provide power to the FAN5331SX directly from the battery? It can accept voltage range from 2.2v to 5.5v. That way you eliminate a good portion of the loss of efficiency of the linear regulation, and you will also need less filtering on the output of the linear regulator.

    Your supply trace from the FAN5331SX to the OLED ribbon is very long. Any chance you can move the FAN5331 closer to the OLED ribbon? You're still going to need polygon pours for heat sinks.

    It looks like you have some pretty long traces from the OLED connector to the 24 pin dual header. Can you move them closer together to reduce their length?
    There's one trace that runs on the bottom layer from the lower right corner, all the way around between the pins on the 24-pin header, then back down to a cap on the bottom of the board, and finally on the top layer back to the ribbon connector. I'm sure you can route that more directly.

    Same thing with those three diodes; you have the common running from the right to the middle of the board, and then each diode seems to be oriented to maximize the length of the traces. Can't you move those diodes over to the right side of the board? Or, what's the deal with the whited-out rectangular area; is something mounting on there? If so, perhaps you can move the three diodes to the bottom of the board to keep them close to where they need to be.
    [eta]
    I don't know what kind of power you need to send through those diodes, but you can get SMT/SMD diodes that are quite compact; some are Schottky and have a very low Vf, which is good for low power dissipation. You might consider something like a BAT120C.
    A couple of other possibilities:
    http://search.digikey.com/scripts/DkSearch/dksus.dll?Detail&name=CRS01QCT-ND
    http://search.digikey.com/scripts/DkSearch/dksus.dll?Detail&name=MBRX120LF-TPMSCT-ND

    It will work, but that trace seems to be quite long, and rather thin. I don't know how much current you're planning on it conducting. You should run your numbers through PCBtemp to find out how much thermal rise you're going to get with the trace widths you're using. Roman Black is hosting PCBTemp, as UltraCad has dropped support for it:
    http://www.romanblack.com/pcbtemp.htm

    Whenever you need to route a signal from one layer to another.
    You will also find it useful to conduct heat from one layer to another. For example, your FAN5331SX has an internal switch that will cause some heat when power flows through it. You can use vias to conduct that heat between the top and bottom layers, so you wind up with more surface area to radiate the heat from.

    You used the horizontal package. Use the vertical package.
    I don't know what you used for the LM1117T device, but in v-reg.lbr, there is:
    LM317TL - this uses the horizontal TO-220 package
    LM317TS - this uses the vertical TO-220 package
    So, have a look at those to see what they're using; or just use the LM317TS and reVALUE it to LM1117T.

    Sure.
    Have a look at this page:
    http://www.smps.us/pcb-design.html
    There are some links on the bottom left of the page.
     
    Last edited: Sep 30, 2011
  7. John P

    AAC Fanatic!

    Oct 14, 2008
    1,634
    224
    If the LM117 is like the more common LM317, it can't regulate 3.7V to 3.3V. It has a minimum voltage drop of about 1.3V. Also it looks as if it's not wired up right: am I seeing the ADJ terminal connected to Gnd, and two resistors going from Vdd to Gnd and never touching the ADJ pin?

    There should be a filter capacitor as near as possible to the power supply terminals of the processor.

    There should be an electrolytic capacitor between Vbat and Gnd.

    How about part numbers on the silkscreen?

    Is that long row of pads in the bottom right intended as a connector? You'll need to have a gap in the solder mask to expose them, and it seems as if some of them are shorted. Those are very small pads, if that's what they are!

    Please don't say you designed this on the fly and never drew a circuit diagram!
     
  8. SgtWookie

    Expert

    Jul 17, 2007
    22,182
    1,728
    Good catches, John_P - obviously my coffee hadn't kicked in quite yet. ;)
    The LM1117 has a minimum dropout of 1V with no current output!
    You would need at least 4.3v in to get 3.3v out with no load.

    The LM1117T-3.3 is sort of like a low-dropout 78xx series 3.3v fixed regulator.
    There is a LM1117T-ADJ that's similar to the LM317. Still, I think the term "low dropout" is being stretched a bit with this regulator.

    I didn't notice the shorted pads for the ribbon connector, either.

    Since the 24-pin dual row header is 0.1"/100 mil spacing and the ribbon connector is metric, it's easiest to route the traces neatly from the non-grid-spacing dimension object (in this case, the ribbon connector) to the object that has the same spacing (or multiple of) the grid spacing, and making at least 1 angle (corner) between the objects. That way, the traces will start and end in the center of the pads, and you will have less problems with overlaps/shorts.

    It looks like a number of the traces were drawn without the benefit of having 45° angle bends selected, such as those in the lower right corner. You really want to avoid having angles that are not even multiples of 45° where possible.
     
  9. Vanush

    Thread Starter Active Member

    Apr 19, 2008
    46
    0

    Hello. It's an LM1117T linear regulator, the pinouts are GND, VOUT, VIN.
    Since I was prototyping before with 5V I didn't realize that it wouldn't work with my final battery voltage of 3.7V. So I will have to find a lower drop out..

    The pads are for a display module like http://media.digikey.com/photos/Newhaven%20Display%20Photos/NHD-1.8-128160YF-CTXI%23.JPG

    The pitch is 0.75mm. No connectors exist, so I will have to solder directly. (Going to be hard)
    I did have a problem trying to reconcile metric with the 0.1" grid. I will try that technique in my next iteration.

    Thanks for the tips.
     
Loading...