Vias to the groundplane in the autorouter

On 15/08/2012 21:58, Robin Szemeti wrote:

Hi,

 

I'm trying to autoroute an audio circuit.

 

I have a groundplane and would prefer Eagle to wherever possible simply take a via from one end of the SMD direct to the groundplane.

 

When I run the autorouter, it seems to go to extreme lengths to avoid vias where possible, running long tracks that eventually work there way to pick up a groundplane via. Even if I manually place vias on all the components with an gnd connection, it still seesm to try and run additional tracks around the place.

 

Is there a pre-made recipie for the autorouter that will efficiently pick up groundplane vias close to the end of SMD components, making good use of the nice groundplane I have provided for the purpose.

 

I second this wholeheartedly. I attempted to remove some ground tracks

on the front of an auto-routed board between points which were already

directly connected to the same ground plane on an internal layer. I

couldn't do it because I am told to do it in the schematic !

       Andrew

On 8/16/2012 9:51 AM, Andrew Forrest wrote:

On 15/08/2012 21:58, Robin Szemeti wrote:

>> Hi,

>>

>> Is there a pre-made recipie for the autorouter that will efficiently

>> pick up groundplane vias close to the end of SMD components, making

>> good use of the nice groundplane I have provided for the purpose.

>>

The trick for this is to disable all of the optimize runs in the

autorouter and set the Max number of vias in the route and bus tabs to

9999. The job of the optimize runs is to minimize the number of vias(not

what you want in this situation). Setting the MAX number of vias to 9999

tells EAGLE to use as many vias as necessary.

Additionally you would want the autorouter to only route your power

signals so before doing the above type AUTO net1 net2 etc, and press

enter then go ahead and perform the settings above.

 

I second this wholeheartedly. I attempted to remove some ground tracks

on the front of an auto-routed board between points which were already

directly connected to the same ground plane on an internal layer. I

couldn't do it because I am told to do it in the schematic !

To delete a via implies the destruction of a net hence EAGLE tells you

to remove it from the schematic. What you want to do is RIPUP the via

convert it back to an airwire.

hth,

Jorge Garcia

 

       Andrew

I am fairly new to Eagle, so please I hope someone will correct me if I am not stating something correctly here, but below is what I do for ground vias.

I place ground vias on my boards and name them Net Class "Ground" in the Properties Dialog Box. Then when I create a ground pour with the Polygon tool, I name that polygon Netclass "Ground" also. I use the DRC to specify "Generate Thermals" for vias in the Supply Tab. When I do a "ratsnest" by the Toolbar command all my ground vias are connected to ground via the ground pour polygon, with thermals. You mention you have a ground plane, use that to connect your vias to instead of the ground pour I use. Be sure your "ground plane is Net Class "ground" or the program won't know to connect your vias to ground.

Bob Moreno

I am fairly new to Eagle, so please I hope someone will correct me if I am not stating something correctly here, but below is what I do for ground vias.

I place ground vias on my boards and name them Net Class "Ground" in the Properties Dialog Box. Then when I create a ground pour with the Polygon tool, I name that polygon Netclass "Ground" also. I use the DRC to specify "Generate Thermals" for vias in the Supply Tab. When I do a "ratsnest" by the Toolbar command all my ground vias are connected to ground via the ground pour polygon, with thermals. You mention you have a ground plane, use that to connect your vias to instead of the ground pour I use. Be sure your "ground plane is Net Class "ground" or the program won't know to connect your vias to that ground.

FYI, you can undo the filled-in ground pour by "ripup @ ;" command. Meaning the filled-in pour will not show but is still there in the layout showing by the original outline of the polygon.