1. Welcome to our site! Electro Tech is an online community (with over 100,000 members) who enjoy talking about and building electronic circuits, projects and gadgets. To participate you need to register. Registration is free. Click here to register now.

Double sided PCBs in Eagle

Discussion in 'General Electronics Chat' started by Electronics4you, Dec 16, 2006.

  1. Electronics4you

    Electronics4you Member

    Joined:
    May 20, 2005
    Messages:
    341
    Likes:
    1
    Location:
    Denmark
    Hi there,

    Doing double sided PCBs in CAD software like Eagle or Electronicsworkbench makes som problems for the hobbyist with no access to through hole plating machinery. When autorouting a double sided PCB the software make holes for components into vias. It means that you either have to make through hole plating to get the proper connection between the layers or solder the components on both sides. The first technique is quite expensive (and time-consuming) and the other a very bad idea.

    Is it possible to set-up the software so that it doesn't use holes as vias, so the connections between the layers can be done with a piece of wire?

    If that's not possible, could anyone then tell me how to make my own via on a PCB trace and make my own PCB traces manually, so I can manually solve the problem after autorouting?
     
  2. justDIY

    justDIY Active Member

    Joined:
    Mar 1, 2005
    Messages:
    1,723
    Likes:
    12
    Location:
    Michigan, USA
    why is it 'very bad' to solder components on both sides?

    I've never used the autorouter, even on complex double sided boards ... there's a certain sense of accomplishment to doing it yourself, not to mention the micromanager in me loves the fiddley work.

    use the ROUTE command to draw your own traces, it looks like two green dots connected with a red line
     
  3. mramos1

    mramos1 Active Member

    Joined:
    Sep 15, 2005
    Messages:
    2,398
    Likes:
    9
    Location:
    Boynton Beach, Florida USA
    If you close the schematic and leave the board open, you can do anything you like to the board (Eagle stops trying to go back to the schematic).

    Sometime you have to use the group tool to move things though. You just can not annotate back to the schematic at that point (so your schematic better be done at that point). I friend of mine goes in, makes an empty schematic, click PCB, closes the schematic and does the whole thing in PCB mode.

    Me, I do schematic and then PCB and then leave pleny of space, LET Eagle route it, and shrink it all up. I am not a PCB guy and normally in a hurry. And I have learned enough to do it by hand, but time is short for me :)
     
  4. Electronics4you

    Electronics4you Member

    Joined:
    May 20, 2005
    Messages:
    341
    Likes:
    1
    Location:
    Denmark

    Soldering components on both sides is hard to do without buring som components especially on close component boards. The un-soldering proces is even harder to accomplish.

    I'm always in a hurry, and don't have the time (even if I want to do PCB routing all day) to do it, because the development and analysis of the circuit afterwards is a heavy job.

    Can you just make a via where you want and then move the "left-over trace" to the next layer?
     
  5. mramos1

    mramos1 Active Member

    Joined:
    Sep 15, 2005
    Messages:
    2,398
    Likes:
    9
    Location:
    Boynton Beach, Florida USA
    If you close the schematic windows you can alter the PCB in any way you like. I do boards all the time where I close the schematic and drop larger pads over the old small ones all the time, because I (am lazy) did not search the forum here to see how to set and save the defaults ;)
     
  6. kchriste

    kchriste New Member Forum Supporter

    Joined:
    Jul 23, 2006
    Messages:
    3,677
    Likes:
    45
    Location:
    Victoria BC, Canada
    You can tell eagle how many vias it's allowed to use to minimize it going nuts with the autorouter (Tools/Auto). Then you can "tear up" any traces you don't like and route them yourself.
    You can also just tell eagle to do a single sided board only (Tools/Auto) by setting N/A as the top layer. Then you can just add pads for the unrouted traces for topside jumper wires.
     
  7. justDIY

    justDIY Active Member

    Joined:
    Mar 1, 2005
    Messages:
    1,723
    Likes:
    12
    Location:
    Michigan, USA
    when you're using the ROUTE command, you can change layers on the fly, and eagle will automatically generate a via at that location. When I'm in a rush, I use this method, instead of specifying jumpers in the schematic.
     
  8. john blue

    john blue Member

    Joined:
    Oct 27, 2006
    Messages:
    67
    Likes:
    2
    • Like Like x 1
  9. tvtech

    tvtech Well-Known Member Most Helpful Member

    Joined:
    Mar 27, 2010
    Messages:
    2,461
    Likes:
    257
    Location:
    South Africa
  10. Boncuk

    Boncuk New Member

    Joined:
    Nov 10, 2007
    Messages:
    5,382
    Likes:
    87
    Location:
    Phetchabun,Thailand
    You can route manually using jumps.

    Before routing you should determine via shape, diameter and drill size.

    For easiest vias to solder wire use shape octagon, diameter 1.6002mm (standard pad diameter for DIL-packages) and drill size 0.8128mm.

    Start routing on the solder side (bottom layer) until you reach a position where the jump should start. Click 'Change' -> 'layer' and select top. Continue routing until getting to the final position of the jump. Change layer back to bottom and finish the trace.

    There is no need to use vias in the schematic.

    If you rip up a trace consisting of bottom and top layer the vias will also be erased.

    Plan to draw the top layer trace as a straight line always using a straight wire for the jump.

    Here is an example of jumps.

    Boncuk
     

    Attached Files:

  11. DirtyLude

    DirtyLude Well-Known Member

    Joined:
    Aug 5, 2003
    Messages:
    1,787
    Likes:
    31
    Location:
    Toronto, Canada
    I know this is an old thread that has been bumped, but I've tried several methods. I tried the wire though method that's shown in the link and used it for a while, but it was never that easy or quick. The method I use now requires a hot air rework station unfortunately, but I just use a cheap Chinese one.

    I drill the holes for the vias and lay the board flat on a piece of wood. I use a long piece of bare wire and insert it in a hole and snip it off flush. I skip through each hole doing this. The board is flush with the wood it's sitting on, so there's a small bit of loose wire in each hole. I put a dab of solder paste on each via and then just heat the board and the solder beads. Flip the board over, dab paste on the other side and repeat. It's super quick.

    This was the first board I tried it on. I put a little too little paste on some of the holes so they don't look perfect, but it works well.

    20091020-pcb-vias-002.jpg
    20091020-pcb-vias-001.jpg
     

Share This Page