1) Select a net.
2) Right click and select 'Add via'.
It is also possible to add a via shield when a net or Pin-pair is selected.
It is also possible to add a via shield when selecting a flooded copper area.
Thanks for the feedback Klaus. The complication here is that
these are just copper geometries as imported from the DXF. There are no nets.
The vias as generated in AWR are just copper circles on their own layer
(and I assigned the layer at DXF import). I thought that maybe I could
select one of these circles, RMB, add net, and then do the process you
described. That didn't seem to work either. I thought maybe it was because the
vias were on their own layer, so I drew a copper pad on the top layer and followed
the same process - still no luck. Can you think of any other ways I might go
about this? If there is a way to assign all of the copper pads the same net
that was also tied to the bottom plane such that PADS would automatically add
the vias, that would be really slick, but I’ll settle for just being able to
manually place vias. I appreciate any additional feedback you might have.
First you need to define your nets. Ideally import the netlist from your schematic, or you can use the ECO tool to manually add nets (after you manually place components so you have something to connect with nets; these components could be as simple as surface mount test points).
Once you have the nets, assign the nets to the copper shapes (I'm assuming you've already converted your 2D-lines to copper shapes). Then you are ready to follow Klaus' suggestion.
Thanks John. I tried to do something very similar. What I've got is basically a bunch of copper pours that I imported from my DXF. Unfortunately, there is no way to bring in nets from AWR. I was able to right click the copper pours and assign nets to them. I ended up assigning my back copper to a net I called ground and assigned a couple of the copper pours on my top plane to ground as well. I wasn't able to add a connection between the top and bottom copper pours using the eco toolbar for some reason. I was hoping that if I could add a connection, I might even be able to take this a step farther and automatically add stitching vias.
I did find a workaround. I found a SMT resister (could have used anything with two or more connection points), placed it on the board, and connected the two pins. I then right clicked the connection and added a via. Then a copy-pasted this via everywhere I needed it. The Gerber/Drill file previews look good now. This works for what I'm doing right now, but it seems like the need for this arises every few months, and it would be nice to have a better way. These are all very simple RF boards used for test and we're really just using PADS as a way to generate drill files and Gerbers. My needs for the moment are met by this workaround (assuming my board house doesn't return any concerns), but I am certainly open to any suggestions that might make this process better in the future.
2 of 2 people found this helpful
PADS :Layout will only make connections between pins. Even though the copper shapes were already on the proper net, Layout didn't see anything to connect on that net until you added the resistor pins.
I suggest you build a simple schematic in PADS Logic to define the GND net and use SMD test points components to define the other nets (or you could do it with an ASCII editor). You can import this to Layout, place your test points where they will be hidden in the pours and then make your connections. You can probably even use the automatic via placement for perimeter or plane via placement; the last time I worked with RF shapes I had to place the CWG vias manually.
That's exactly what I'm dealing with, coplanar waveguide. In this case, my frequency is low enough that via placement isn't critical. This is on the right track. I really only grabbed the SMD resister because it was convenient. Is the SMD test point in one of the default libraries?
1 of 1 people found this helpful
Standard libraries... yuck, never use them. Here is a 5 mil square test point that I defined. It is easy to hide in almost any pour.
Import these three files into the Library Manager in Layout (.p into Part, .d into Decal, and .c into Logic) and you'll have a part that can be used in Layout and Logic. It can be imported into a Central Library if you use DxD.
Thanks John! That's very helpful. I suspect this will make things much less painful next time around.