PCB ground plane not connecting to ground pins

Question

Hello,

I did some PCBs with Eagle, so I was quite sure I know it's basics, especially when it comes to ground and power planes.

I have a LQFP-100 device with some pins supposed to be connected to ground. I made a ground plane on the top layer, named it GND, same name as the gound net on schematics. Yet the plygon won't connect to the gound pins. I've put right next to the LQFP a different device (USB port) with ground pins as well - those are connected just fine.

Big pad on the bottom right is the GND pad of the USB connector, as you can see an airwire is led to the LQFP pin. There are some "blobs" or whatever on both sides of the unconnected pin.

I think I've clicked just about everything in Eagle, still no-go.

Eagle 6.2.0 Light.

Regards

Former Member · Accepted Answer

On Sun, 06 Jan 2013 13:08:22 +0000, Michal Lesiak wrote: Hello, I did some PCBs with Eagle, so I was quite sure I know it's basics, especially when it comes to ground and power planes. I have a LQFP-100 device with some pins supposed to be connected to ground. I made a ground plane on the top layer, named it GND, same name as the gound net on schematics. Yet the plygon won't connect to the gound pins. I've put right next to the LQFP a different device (USB port) with ground pins as well - those are connected just fine. Image:pcb-gndplane.PNG Big pad on the bottom right is the GND pad of the USB connector, as you can see an airwire is led to the LQFP pin. There are some "blobs" or whatever on both sides of the unconnected pin. I think I've clicked just about everything in Eagle, still no-go. Eagle 6.2.0 Light. Regards Check the trace size of the polygon that you're using to define the ground plane. It may be that the polygon trace size is too large to make the connection to the package. -- Tim Wescott Control system and signal processing consulting www.wescottdesign.com

Former Member · Answer

You can see the problem in the image with adjacent pins connected.

Note the distance the polygon is keeping away from the other pins(signals)

Now imagine that distance must be clear from a pin either side of a GND

pin. That does not leave room for a very wide trace.

So you need to balance.

(1) The polygon wire width. This will be the width of the trace attempting

to connect to the pin if it can without braking the required clearances

rules.

(2) The DRC and Class clearance rules governing how far signals must be

away from other signals

(3) A grid that is fine enough so that the above clearances can still be

satisfied if the pin/grid alignment is less than optimal

(4) For Autorouting a routing grid that satisfies similarly to point (3)

HTH

Warren

--

Web access to CadSoft support forums at www.eaglecentral.ca. Where the CadSoft EAGLE community meets.