I used to check complex commercial PCBs specially those of graphics cards to see how professional PCB designers do their layout and learn from their techniques.

When I checked the card shown below I noticed two things regarding the placement of vias:

(A higher resolution image is shown here).

  1. The PCB is surrounded by stitching vias all around the edges. What's the role of all of these? I think they're connected to ground to act as a shield, if that's true, I can't understand technically how by this placement they achieve this shield?

  2. By looking closer to the mounting holes, I noticed they added vias all around the pad, why?

enter image description here


3 Answers 3


Ground Ring

Surrounding the PCB, and sometimes areas within the PCB, is surrounded by a ring of traces that is connected to GND. That ring exists on all PCB layers and is connected together with a bunch of vias.

To explain what this does, I need to describe what happens when you don't have the ground ring. Let's say that on Layer 2 you have a ground plane. On layer 1 you have a signal trace that goes all the way to the edge of the ground plane, and runs for several inches along the edge. This signal trace is technically directly over the ground plane, but right at the edge. In this case that trace will radiate more EMI than other traces, also the trace impedance would not be as well controlled. Simply moving the trace in, so it is not at the edge of the ground plane, will fix the problem. The more "in" you move it the better, but most PCB designers will move it in at least 0.050 inches.

There are similar issues when you have a power plane. The power plane should be moved back from the edge of the GND plane.

Enforcing these rules, that traces can't be within 0.050" of the edge of a plane, is difficult in most PCB software packages. It's not impossible, but most PCB designers are lazy and don't want to set up these complicated rules. Plus, this means that there are areas of the PCB that are simply empty of useful traces.

A solution to this is to put in a ground ring and tie it all together with vias. This will automatically prevent other signals from going into that area of the PCB, but also provide better EMI prevention than simply moving the traces back. For the power plane, this also forces the power plane back from the edge (since you just put a GND trace there).

Mounting Holes

In most cases you want to connect your mounting holes to GND. This is for EMI and ESD reasons. However, the screws are really bad for PCB's. Let's say that you have a normal plated through hole that is connected to your ground plane. The screw itself can destroy the plating inside the hole. The screw head can destroy the pad on the surface of the PCB. And the crushing force can destroy the GND plane near the screw. The odds of any of this happening is rare, but many EE's have had enough problems with this to come up with fixes.

(I should note that destroying the plating and/or the pad usually results in metal flecks getting loose and shorting out something important.)

The fix is this: Add vias around the mounting hole to connect the pads to the GND plane. Multiple vias gives you some redundancy and reduces the inductance/impedance of the whole thing. Since the via is not under the screw-head it is less likely to get crushed. The mounting hole can then be unplated, reducing the chance of loose metal flakes shorting something out.

This technique is not foolproof, but does work better than a simple plated mounting hole. It seems like every PCB designer has a different method for doing this, but the basic thinking behind it is mostly the same.

  • 7
    \$\begingroup\$ ... the grounded stitching sort of forms a Faraday cage around the internal layers of the board (which are also sandwiched between ground planes) \$\endgroup\$
    – vicatcu
    Commented Jul 30, 2012 at 14:35
  • \$\begingroup\$ David and @vicatcu .. In a design i'm working on right now I want to apply this ring, but the specs about grounding tell that all mounting holes should be connected to a "Shielding GND" which is completely isolated from the main circuit ground. Can I make this ring and connect it to Shielding GND instead of circuit gnd? would I get same benefits? \$\endgroup\$
    – Abdella
    Commented Dec 20, 2012 at 15:35
  • 2
    \$\begingroup\$ @Abdella The GND ring should be connected to the same GND as your ground plane. If your plane is Chassis GND then connect the ring to chassis gnd, If your plane is Signal GND then connect the ring to signal gnd. Using a different GND will make thing worse. For your mounting holes, you can connect them to the local ground plane through a cap/resistor/bead and then not populate it to keep the hole isolated. This gives you the option of later adding a 0-ohm resistor or whatever when you fail your EMI test. If this is not acceptable according to your spec then you need to change the spec. \$\endgroup\$
    – user3624
    Commented Dec 20, 2012 at 16:01
  • \$\begingroup\$ @user3624 A bit late getting to the party here but... As far as the statement, "Since the via is not under the screw-head it is less likely to get crushed. The mounting hole can then be unplated, reducing the chance of loose metal flakes shorting something out." Isn't one of the prime reasons for the via to be in the annualar ring, other than impedance, so that it's intentionally under the screw head in order to add structural support against the force of the screw in effort to mitigate damage to the PCB? \$\endgroup\$
    – AJbotic
    Commented Oct 15, 2019 at 16:25

You always want to have as much solid ground plane as possible. Inner layers can have ground islands separated, so must be connected to all planes/islands together.

However, there are two most important things:

  1. avoid having a ground loop and
  2. avoid having a ground antenna.

That's why You add as much vias as possible and also "sew" the PCB around.


The VIAs in the mounting holes are there to reduce board assembly labor cost. If you look closely, you'll see that the mounting holes are not plated and there's a small gap between the holes and the inside of the pad.

To solder through hole components, the boards are going through a wavesolder machine. If the mounting holes are plated, they need to be masked on the bottom side with kapton tape for example. This will prevent solder from going up the mounting hole but increased the assembly labor cost.

Using the VIAs in the mounting hole pads, allow the mounting holes to be non-plated and still have the pads connected to the ground plane. On the bottom side, the mounting hole pads are covered with the soldermask. This way, there no need to mask them before going through the wavesolder machine. When the PCB is installed in an enclosure, the screw head will make the electrical contact with the mounting hole top pad and the enclosure.

  • \$\begingroup\$ Really well spotted! At first I didn't realise the mounting holes are not plated, but indeed they are. And then, there are some THT components (it seems the electrolytic caps are THT). And yes, you are right. Probably this was done to reduce the assembly costs with wave soldering. It would be great if we can see a bottom view of the PCB \$\endgroup\$ Commented Apr 27, 2017 at 13:46
  • \$\begingroup\$ @YvonHache This may be accurate, but only if you are assuming there aren't any (or are very few) SMT components on the other side of the board. In modern PCI/PCIe cards, there are significant SMT components on both sides and I'd wager the vast majority are assembled with reflow soldering. Then the few THTs are affixed by hand. \$\endgroup\$
    – AJbotic
    Commented Oct 15, 2019 at 17:36

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.