net label invisible in Eagle PCB layout

Discussion in 'General Electronics Chat' started by vinodquilon, Mar 27, 2010.

  1. vinodquilon

    Thread Starter Member

    Dec 24, 2009
    234
    0
    How can I view net labels on Eagle PCB layout ? Thereby I can easily identify supply & ground nets on the PCB Layout without cross-comparing with its schematic.

    I turn-on all the layers in PCB layout, but except net labels all others are visible !!!
     
  2. R!f@@

    AAC Fanatic!

    Apr 2, 2009
    8,754
    760
  3. SgtWookie

    Expert

    Jul 17, 2007
    22,182
    1,728
    If you are creating a one or two-layer board, you can use the Polygon tool to create a copper fill for a power and/or ground plane(s).

    The polygon tool is below the Arc tool. Click the polygon tool, select a width greater than zero, and spacing/isolate greater than zero. I generally use 0.010" or greater for each.

    Then complete a polygon on your board by left-clicking and moving to the next point. Right-clicking at any time will close the polygon.

    Clicking the "Ratsnest" afterwards will cause the polygon to fill.

    You can rename the polygon using the NAME tool (resistor with R2 highlighted) Left-click on the polygon's edge and give it the name of the power or ground that you want it to be; eg "GND". When you click Ratsnest, everything inside the polygon that has a terminal with that same signal name will be connected to the polygon - if there is a path for it to flow to.

    You could use the bottom for GND and the top for Vcc (or other supply name). That way you will have very little routing of power nets to do.

    With multilayer boards, you can dedicate entire layers for various power rails. Make certain that you use bypass capacitors between the various layers.

    If you just want to see what is connected to a net, click the Show tool (eye) and left-click a trace or air wire. Everything that belongs to the net will be highlighted. The signal name and class will show on the bottom left.
     
    Last edited: Mar 27, 2010
  4. jpanhalt

    AAC Fanatic!

    Jan 18, 2008
    5,699
    907
    I don't know if you can make a net label appear on the PCB. But here is what I do. Maybe it will help:

    Under Option, go to Assign, then assign/reassign a function key to the net(s) you want to highlight. I have F9=GND; F10= +5V; F10=+12V; and F12= -5V for standard settings. Then I have a couple of keys for special nets, like a signal. When I hit a function key, that entire net lights up. It helps in manual routing.

    You can use whatever net names make sense in your specific application.

    John
     
  5. vinodquilon

    Thread Starter Member

    Dec 24, 2009
    234
    0
    Actually in my layout layer list $VCC ,$GND layers are not listed.
     
  6. vinodquilon

    Thread Starter Member

    Dec 24, 2009
    234
    0
    There is one more doubt, How we can cross-reference one relay across different sheets. My aim is that, relay is energized by
    the circuit in first sheet but its coils act on a different section in another circuit.
     
  7. SgtWookie

    Expert

    Jul 17, 2007
    22,182
    1,728
    Those are just example supply node names. You might be using +5v, +V/-V, AGND, or whatever.

    The freeware version of Cadsoft Eagle is limited to either two or four layers (I can't remember now, it's been awhile) - the registered version supports up to 16 layers.

    The layers are numbered. They also have default text names assigned. "Top" is layer 1, "Bottom" is layer 16, and the intervening layers have text names of "Routen", where "n" is the layer number.

    They are layer names, not net names. Big difference.

    You need to experiment with the polygon tool. It's very powerful. Just make sure that the Width is higher than zero, and that Isolate gives sufficient clearance. If the Width is zero or really small, your CAM output files will be *huge* - if it even manages to finish.
     
  8. vinodquilon

    Thread Starter Member

    Dec 24, 2009
    234
    0
    When I auto route, half of the nets comes in the top layer(Component Side) and others in bottom layer(Solder Side).
    But I want only components to be placed on top layer. How it is possible ?
    Does there any difficulties at PCB manufacturing time due to placing all nets on bottom side ?
     
  9. SgtWookie

    Expert

    Jul 17, 2007
    22,182
    1,728
    I do not have the Autoroute feature in my registered version of Eagle.

    If you do not wish for the component side of the board to have traces on it, then you will need to change the options in the Autoroute module, which I can't look at.

    However, change the directions allowed to None for the top layer, and to * for the bottom layer. Rip up all of your existing traces, and re-route.

    You may wind up with some signals that cannot be routed. You will then need to insert appropriate length jumpers in those net(s) on the schematic. Look in jumper.lbr.
     
  10. kubeek

    AAC Fanatic!

    Sep 20, 2005
    4,670
    804
    You have to disable the layer in the routing options. As for the nets, use the Eye tool from the toolbar.
     
  11. cloudsky823

    New Member

    Jun 12, 2012
    1
    0
    I've found it: go to Options -> Set -> Display pad names, then you should see the pads name in layout editor:
    upload_2014-11-25_15-44-35.png
     
Loading...