How to short a net and a shape on layout using VIA

Hi

On your schematic you have three nets, VSS, AGND, PGND. Are you wanting to short VSS and AGND to the PGND Shape with vias on the board using the net_short property.

Perhaps I am reading this wrong but is that what you are trying to do ?

Thanks Paul.

Hello Paul,

The final goal is to short VSS and AGND to PGND. However, in the picture both VIA are connected to AGND.

I would expect that once net_short has been set on both they should be connected while the blue line seems to indicate that connection is still missing.

Thanks for your help

Francesco

Hello Paul,

The final goal is to short VSS and AGND to PGND. However, in the picture both VIA are connected to AGND.

I would expect that once net_short has been set on both they should be connected while the blue line seems to indicate that connection is still missing.

Thanks for your help

Francesco

Quite hard to tell exactly what is going on from just a screenshot but possible issues could be: Shapes are Dynamic and not up to date, check Shape>Global Dynamic Parameters or Design Status; the PGND shape is Static, rather than Dynamic and won't be updated to connect the Vias, change the Shape Type to Dynamic could help; you are using Negative Artwork and Dynamic Shapes and the Shapes need to be updated to reflect the connectivity change. Dynamic Shapes and positive artwork would be the recommended approach to Shapes, Shape updating of "Smooth", or "Rough", would ensure that Shape to object connectivity gets updated "as you go"

Hi oldmouldy and thanks for your reply.

PGND shape is dynamic. Indeed you can see that the vias are completely surrounded by it (because of the NET_SHORT property on the VIA)rather than having the clearence as if they were on different nets.

My question is why the two vias are not logically connected on the layout even if both have NET_SHORT set to AGND:PGND.

Francesco

Hello Francesco

Might I suggest that you do not use Net Short to fool the PCB nets. Doing this will mean that your netlist from the schematic does not actually
reflect what is on the board.

If you have multiple Ground Planes, such as VSS, AGND, PGND etc on the schematic and your intent is to have them joined on the board
then a good way to accomplish this is by using zero Ohm resistors between those nets at the schematic level. On your board you will then
have basically a component joining in the ground planes and your board will electrically match the schematic.

You could even make a Small copper ground plane part with two pins and a similar schematic Symbol to do the net joining. 

A good rule of thumb on any design is, If it does not exist on the schematic then it should not exist on the board.

Thanks Paul.