Microvia in OpenGL Canvas

Hi, I’m placing micro-vias and the shove router correctly blocks me routing a trace over other unlike nets on different layers, but other times it will let me route a trace directly over/under others. Also it will push some vias out of the way but let me walk all over others and I am not seeing any discernible pattern to it?

The reason I don’t expect this is because I have explicitly said “Do not allow blind/buried vias” in the design rules. So I’m a little confused how this is supposed to work.

All I am doing is setting the normal and micro via up in Net Classes Editor under default. Under Global Design Rules I have “Do not allow blind/buried vias” and “Allow micro vias”

pcbnew version : 4.0.2

First try updating to a more recent version. 4.0.2 has a lot more bugs than 4.0.7

If you still see the behavior you could try and help us understand you by adding screenshots. Ideally you mark the affected vias in the screenshot.

Thanks I upgraded to the latest same problem.

In the image below I run the blue trace to the center of the pad. Press Ctrl+V to place a micro via and click to end.

The DRC shows this pad is not net connected hence I am able to run the yellow trace on a different net directly under it.

Clearly I’m not placing the via-in-pad correctly??

What are the interactive router settings?

Micro vias can of course be placed on top of other traces as they only affect two neighboring layers.

I tested it in KiCad 4.0.6.
If i have micro vias disabled in the project settings (this is the default), i get an error message when i try to place a via with (crtl+v).

So if you have indeed disabled microvias but are still able to place them, then there is some bug hidden in there.

Um no, Micro vias should not ‘of course’ be placed on top of other traces if I have ‘Do not allow blind/buried vias’ option and I do, and even if I did my Yellow and Blue traces are on facing inner layers.

Below are my other settings.


The micro via goes from red to blue Layer. All other layers are not affected by the micro via.

A micro via that can go further than between two layers is called stacked micro via. This is even more expensive than a normal micro via.

I have made a quick sketch to explain your situation (with colors close to the once you used in pcb new)

And a image found via google that shows multiple different types of vias.


First and foremost I owe you [Rene_Poschl] an apology because in my ignorance I had a fundamental misunderstanding of what a uVia was and assumed they were just tiny vias that went all the way through the board connecting all layers and that buried or blind vias were the only ones that traversed layers less then the total number of layers…

So thanks. With that understanding the routing makes perfect sense.


A microvia (uvia) is indeed just a tiny via, usually less than 150um, and can be either a blind or buried via. However, like all vias a uvia has an aspect ratio constraint. Standard through hole and buried vias are constrained to a max aspect ratio (diameter to depth) of 1:10 to 1:12 depending on fab. Some fabs offer aspect ratios up to 1:6 as part of their standard service while higher aspect ratios may incur higher costs. However standard blind vias have an aspect ratio constraint of 1:1. Therefore a suitable diameter must be used if the blind via will connect more than two layers. A uvia has an aspect ratio constraint of 1:0.8 (most fabs offer 1:0.5 as standard) and therefore, due to their small diameter, are limited to the thickness of a single layer of prepreg.

Note: Aspect ratio is based on the pre-plated drill size. Always consult your fab for their capabilities.

1 Like

This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.