PCB layout help

Discussion in 'The Projects Forum' started by kiyoukan, Nov 4, 2010.

  1. kiyoukan

    Thread Starter Member

    Nov 17, 2009
    63
    0
    Hello i have been working on a project and gotten as far as i can with my skills.
    I have a schematic that and the pcb board done and laid out mostly.
    The only part left are doing traces on the PCB board. i orientated the components and set them but i am not good at all doing traces.
    I would be willing to compensate for help.
    Also note that i have removed the buttons as they are not needed.
    http://forum.allaboutcircuits.com/attachment.php?attachmentid=24255&d=1288917724
    [​IMG]
    [​IMG]
     
  2. kiyoukan

    Thread Starter Member

    Nov 17, 2009
    63
    0
    okay so i gave it a go. if any one here has expresspcb and a good eye you mind giving it a look over.
    I had a friend help me put down the traces and both went over it but i cant help feel there is still something off.
    the file is a .pcb but named .brd to get it to upload.
    again i omitted the switches.
     
  3. KMoffett

    AAC Fanatic!

    Dec 19, 2007
    2,577
    231
    "cant help feel there is still something off." Elaborate!
    Have you "linked" the schematic and pcb files to verify net connections?
    Post both the .sch and .pcb files.

    Ken
     
  4. John P

    AAC Fanatic!

    Oct 14, 2008
    1,634
    224
    Sorry to have let communication lapse earlier.

    I'm noticing a couple of things: you say "USB B" but I think that's a USB A footprint, and why are the pins not evenly spaced?

    There don't seem to be any resistors or capacitors on the board, but they're off to the side, so maybe you hadn't done that part yet.

    If that voltage regulator is in a TO-220 package, I wonder if the holes are big enough. Other parts, like the crystal and the USB connector, seem to have holes that are too big.

    I'm used to dealing with LCD's that have 14 pins, or 16 if there's an LED backlight. Does the LCD plug in directly here, or is there a cable?

    If this really does have to be "as small as possible" you could put components on the back. Maybe that's the plan with the R's and C's.
     
  5. kiyoukan

    Thread Starter Member

    Nov 17, 2009
    63
    0
    Yes is did switch from a usb type b connector to a type a the b was to tall so i decided to go with the other connector.
    Remember that brd file is a pcb but it wont let you upload a.pcb file so i changed it to a .brd os when you dl just change the name and it will work fine.
    Also i used a 78L05 for space.
    And that picture is just there for idea of component placement.
    [​IMG][​IMG][​IMG][​IMG][​IMG]
     
  6. KMoffett

    AAC Fanatic!

    Dec 19, 2007
    2,577
    231
    In ExpressPCB, to "link" the .sch file to the corresponding .pcb file, component designators (S1,R1,R2,C1,U1,J5....) on the pcb must have matching designators in the sch file. When linked, the pcb network function will show you if all the pins on the schematic are connect to the corresponding pins on the pcb layout. None of the components on either of your schematic or pcb files have unique designators.

    Ken
     
  7. kiyoukan

    Thread Starter Member

    Nov 17, 2009
    63
    0
    Okay i have updated them and linked them.
    So i think its right now, i just want some help before i go and etch out my trial version and test. i would hate to find a mistake.
     
  8. KMoffett

    AAC Fanatic!

    Dec 19, 2007
    2,577
    231
    I cant run a "Highlight net connections" check, because of too many wires that are not properly connected to pads.

    On the mounting hole pads...see the little dark red squares? Also to the lower mounting pin hole for USB. Same on the square pad next to "TEC". These are the ends of wires that are not terminated at the center of the pads. It would work for etching your own boards, but it does not give you a correct net list to work with. When you run a wire to a pad, you connect it to the center, not just anywhere. It prevents the linking for cross checking the layout with the schematic.

    Also it looks like you overlayed some of your thinner tracks with thicker ones, without deleting the thin ones.

    There are green tracks to the left and around the tops of P2 and R2 that don't go any where.

    Green surface mount pads below "R2" ???

    I'm trying to type one handed with my non dominate hand, because of surgery. (I hate capital letters!) It wears me out, so I'll stop for now, and let you clean things up a bit. So far it seems like a nice compact layout.

    Ken
     
  9. kiyoukan

    Thread Starter Member

    Nov 17, 2009
    63
    0
    okay so i cleaned it up a bit.
    And after talking it over 2 buttons have been added to aid in the programing.
    I also changed and corrected the pins on the usb as well as the headers.
    Every thing should check out.
    I also will be adding a ground plane on both sides of the board once i am done.
    I do not add it now because it makes it hard to see the traces.
    Thanks so much for the advice keep it coming!
     
    Last edited: Nov 6, 2010
  10. KMoffett

    AAC Fanatic!

    Dec 19, 2007
    2,577
    231
    no connection (via) between top and bottom layer at X=0.775 Y=0.675
    no connection (pad) between top and bottom layer at X=0.675 Y=1.250
    un-designated, un-grouped component with lower right corner at X=0.675 Y=1.250
    SC1 has more pins and connections on the pcb than on the schematic.

    Ken
     
  11. kiyoukan

    Thread Starter Member

    Nov 17, 2009
    63
    0
    okay i understood what you posted before but i am a bit confused about this last one.
    i go to those coordinates and i do see what you mean.
    made some minor changes in the pcb and opamp is now all recognized.
    missed a connection to ground on pin 19, corrected.
    but other than that i keep going over it with a fine tooth comb and don't see any problems.
     
    Last edited: Nov 6, 2010
  12. KMoffett

    AAC Fanatic!

    Dec 19, 2007
    2,577
    231
    In ExpressPCB components, even non polarized ones, have unique designated pin numbers. A resistor has a pin 1 and a pin 2 in the schematic. The PCB resistor also has a pin 1 and a pin 2. Connections to pin 1 in the schematic should be to pin 1 on the PCB. In order for the net list to be checked on the PCB, you sort of treat them as polarized. The easy correction is to ctrl-x the offending component, ctrl-v it, rotate it 180°, and move it back into position

    I think I missed your switch in download subdirectories. Project 3

    Check the routing from the pic's pins 17 and 18 to R5 and R4 to SW1 and SW2. I think R4 and R5 are swapped.

    C3, C4, C7, C8, R, Reversed

    Trimmer P end connections reversed

    C5 and C6 reversed and swapped

    TEC pin connections reversed.

    I'm going to stop there for now...left hand is tired. :0

    Ken
    __________________
    "To invent, you need a good imagination and a pile of junk."
    Thomas A. Edison (1847 - 1931)
    Edit/Delete Message
     
  13. kiyoukan

    Thread Starter Member

    Nov 17, 2009
    63
    0
    Okay thanks going to go and check and make those corrections.
    Also how do you do that check? all i can do is click a component and it tells me if theres a problem.
     
  14. KMoffett

    AAC Fanatic!

    Dec 19, 2007
    2,577
    231
    In the PCB window, select the bottom icon button (picture of pads and wires) on the left side. This is "Highlight net connections". After selecting it, when you click the cursor on a pad, all the pads that are connected to it in the schematic will be highlighted in blue. In the upper right of the window are four (we used to call them) VCR buttons. The left one highlights the first connections in the net list. The right one highlights the last connections. The third button from the left steps forward one set of connections at a time. The second from the left steps backward one set of connections at a time.
    It really helps find missed or wrong connections. Once you highlight a group, visually go through and see if all the blue pads are connected, and that there aren't tracks in it that go to un-highlighted pads.
    It really helps verifying missed or incorrect connections.
    Because you have lots of vias, and a mix of surface mount pads on both sides of the board, you may periodically have to turn the layers (three buttons on lower left) on and off and on to see where your traces go.

    Ken
     
  15. kiyoukan

    Thread Starter Member

    Nov 17, 2009
    63
    0
    okay made the changes.
    We are getting their it looks like.
    a quick question tho, the resistors and caps being the wrong way does not matter much right? once the bard is made it make no difference just for schematic checking correct?
     
  16. KMoffett

    AAC Fanatic!

    Dec 19, 2007
    2,577
    231
    Yes, orientation of the non-polarized components in the real world, makes no difference. Only in the development program.

    Ken
     
  17. KMoffett

    AAC Fanatic!

    Dec 19, 2007
    2,577
    231
    For net list link consistency:
    rotate C8 180
    rotate SW2 180
    rotate SW1 180
    rotate C4 180
    rotate TEC 180
    rotate C2 180

    Very tight track/pad spacing at:
    Red X=0.525 Y=1.275
    Red X=0.350 Y=0.175
    Red X=1.025 Y=0.400

    It's a good practice to turn on one layer at a time to look for tight track spacing issues.

    Ken
     
    Last edited: Nov 8, 2010
  18. KMoffett

    AAC Fanatic!

    Dec 19, 2007
    2,577
    231
    C8's pads are shorting USB'S pin 2 to +5 and 3 to ground.

    Ken
     
  19. kiyoukan

    Thread Starter Member

    Nov 17, 2009
    63
    0
    updated traces have yet to rotate pads will do shortly
     
  20. KMoffett

    AAC Fanatic!

    Dec 19, 2007
    2,577
    231
    I"ll wait. :)

    ken
     
Loading...