Ground Planes

Making PCB Layouts, Manual routing, Auto-routing, Copper pouring, Updating from Schematic, Manufacturing Output
Post Reply
Message
Author
tom42107
Posts: 1
Joined: 04 Apr 2013, 22:10

Ground Planes

#1 Post by tom42107 » 15 Sep 2019, 19:46

What is the correct way to connect a component pad to a ground plane? Would you make a ground plane, make a trace between all the components that go to ground and tell the ground plane to connect to that net or use the thermal settings for each pad and tell it to connect directly to the pad. When I try that, I get a lot of errors when I run verification. When I connect all the pads with a trace and connect that net to the GP no errors.

Tomg
Expert
Posts: 1404
Joined: 20 Jun 2015, 14:39

Re: Ground Planes

#2 Post by Tomg » 16 Sep 2019, 08:45

When connecting a pad to a copper pour, a trace is not necessary. Just make sure the copper pour belongs to the same net as the pad and confirm that the pour has been updated. If you are not driving your design with a schematic, you will need to find all of the pads that are destined for the ground net and tie them together using the Place Ratline tool. This will create a new net which can be renamed "GND" (if desired) without having to lay down a trace. Once the "GND" net exists, it will be available for connection to the copper pour in the Copper Pour Properties dialog window under the [Connectivity] tab.
Tom

d1wang
Posts: 46
Joined: 13 Nov 2018, 02:19

Re: Ground Planes

#3 Post by d1wang » 20 Sep 2019, 07:47

Possible reasons of DRC error:
  • The net class of your GND has a clearance set to a value smaller than what's in your DRC
  • You have multiple net classes, each with a different clearance value. One of these net classes has "Use Clearance in DRC" checked.
  • On your copper pour, you set the clearance to a small value and do not have "Use Net Clearance" checked.

Newtham
Posts: 6
Joined: 03 Sep 2019, 20:31

Re: Ground Planes

#4 Post by Newtham » 24 Sep 2019, 13:31

Is it possible to simply tell the pour algorithm to not violate DRC?

In other words, set the design rules as higher priority than the pour rules, so that when it is pouring, it will not pour in an area that violates the rules. It seems odd to have it otherwise... :|

For the record, I am creating a board with MW frequency traces. I want the spoke width to be large when connecting to SMT capacitors, but when I do that, it shorts (or fills too close to) the small SMT ICs pins. As far as I can tell, I have set all the constraints properly, but it's very possible I missed something. I tried 45 degree spokes, which sorta-fixes this issue, but creates other, similar issues on other pins. I know I can create special rules for each IC (which is, I think, what I will have to do) but this could be really time consuming, when a simple "follow DRC in pours" option would solve it.

Am I missing something? Thanks!!

Tomg
Expert
Posts: 1404
Joined: 20 Jun 2015, 14:39

Re: Ground Planes

#5 Post by Tomg » 25 Sep 2019, 11:06

The real problem lies in the way spokes are generated in DipTrace. They seem to consist of a single copper line terminated with a half-circle rounded end having a diameter equal to the line width. When the spoke width is increased (the width of the single line), the size of the rounded-end is enlarged to match; increasing the length of the spoke. Apparently, the spoke "length" ends at the intended contact point, but the rounded end adds to the line's length. The larger the width, the longer the rounded-end termination becomes; increasing the possibility for it to overlap a nearby clearance gap.

Ideally, the spoke-generating algorithm should not rely on a single line with a rounded/half-circle termination. Each of the thermal relief's spokes would need to be created independently and each spoke should consist of multiple thin lines. Each line making up a spoke would likely have a different length depending on its targeted contact point. Processing time would increase, but I think that shouldn't overly-tax any system built within the last 10 years.
Tom

Newtham
Posts: 6
Joined: 03 Sep 2019, 20:31

Re: Ground Planes

#6 Post by Newtham » 25 Sep 2019, 14:34

Yes, I agree. I learned layout using KiCad, which is very diligent about following rules while it pours copper planes. Just neck down the spoke when it will otherwise violate the DRC, like it can do when you are wiring a trace.

Tomg
Expert
Posts: 1404
Joined: 20 Jun 2015, 14:39

Re: Ground Planes

#7 Post by Tomg » 25 Sep 2019, 16:11

Here are examples for anyone desiring further clarification on the spoke width problem...
spoke width.gif
You do not have the required permissions to view the files attached to this post.
Tom

Post Reply