PCB ground plane not connecting to ground pins

Oh, it got worse. I suspected the package to be of some problem, so I changed it from analog-devices to atmel's LQFP-100 and reconnected all pins. Now it won't even airwire them, so I cant connect them manually. And if the two or more pins are next to each other they are connected properly, only the single ones are left unconnected.

hellow Michal, welcome to the community. have you tried changing the grid size to a smaller size and routing the GND pins of the ic to the usb GND pin in the scematic?

Yes, tried both of that - current PCB grid is 0.00625inch, and I've tried manually connecting all ground pins without the supply symbol and naming the net 'gnd' - the effect is still the same.

Also, I've put a genuine LQFP-100 part from atmel.lbr (AT91SAM7X128-AU) and connected random pins to GND - the effect is the same:

it does the same thing on mine so there has to be somthing wrong with the package.

I've checked this with QFP144 package and it's still the same so I guess thats more like a program problem than a packages one.

I've reduced the grid to "finest" setting, no help.

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

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.

A side note,

Your isolation seems to be really small. This is the gap between the GND flood and the other, non GND pins. Try setting it to around 10 or 12 mil, to prevent accidental shorts caused by manufacturing errors.

Thank you all, indeed it was the problem with polygon trace widh - had to set it to 0 to make it work.

Be aware that it is not good practice to use zero width  polygon wires.

That will make gerber files large. I tried your situation and could get it

working with 7 mil wires with 8 mil spacing in the DRC.

Warren

--

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