Hello,
I would like to know if it is possible to create a via mesh on ground located on each side of a PCB.
What I mean is how to automatically create vias, for example, every cm. * * * * * *
* * * * * * etc
cdt
Sure.
Just select the via tool from the right toolbar:
Then place a via somewhere, and adjust it’s properties to something you like:
Then Right click it and select the array tool:
Fill in some numbers and your PCB is covered:
If you do not want to cover everything, then it may be more effective to create a small array, and set your grid to the same distance as your array settings, and then make a copy of a section of that array and copy it (with help from the grid) to other sections of your PCB.
Ideally you do not want more then one via at any location. With being a bit careful it’s not so difficult to avoid those, but you can also use Pcbnew / Edit / Cleanup Tracks and Via’s and then remove the redundant via’s later.
But in a more general sense:
Why would you want to do such a thing?
Having a single continuous GND plane is a good thing to have for a PCB. Adding a grid of via’s to that is not going to help much. I’ts better to place far fewer via’s but in strategic positons, such as at places where things are actually connected to the GND plane.
For best decoupling, you put the decoupling capacitors closest to your IC’s, and then connect the GND of the decoupling capacitors to the GND plane. But ideally those three (GND pin of IC, GND of decoupling cap and Via) are within a few mm of each other and the order does not matter much.
What he’s looking for is Via stitching, in this case to join two ground planes using number of Vias. It’s a common technique, especially if the circuit goes RF.
I usually don’t use Arrays, but set a coarse grid and place Vias manually. It’s been much tougher with earlier KiCads (<5) where one had to route a GND trace between Vias.
Concering RF stuff…
There are also plugins / scripts for KiCad that place stitching via’s around contours. For example:
And there may be similar plugins in this fashion, but I have no experience with them myself. The link above was just one that popped up with
https://html.duckduckgo.com/html?q=kicad+python+rf+via+stitching
Hello,
Thank you for your very interesting answers.
But I was wondering if we should not further differentiate the planes of the ground.
For example name Ground1 the ground plane of the digital part, Ground2 the ground plane of the analog part and connect them together in a star just to the Ground connection of the arrival of the power supply. That’s what I read online.
cdt
All this depend on your design goals.
Analog/digital ground separation is widely used. In this case, “Net tie” will be your friend.
Hello,
I come back to you to ask you how to properly connect two planes of analog and digital ground.
I looked on the net, we recommend a very fine PCB trace (ex 0.35mm) between the 2 masses, or a connection with a self impact. Other solution?
Another question, where to connect the power (-) wire? Do you still need 2?
Thank you for your answers based on my model. (Please complete it for explanation)
cdt
I come back to you to ask you how to properly connect two planes of analog and digital ground.
Depends on your goal. Why did you split the grounds?
Do you want to create a dipole antenna that radiates at a hard to calculate / define frequency, somewhere between 50 MHz and 1 GHz and cause a EMC problems? Then you place a single track between both planes, place a component that has some ADC or DAC converters in it and uses a small rise and fall time (most “modern” ICs with CMOS will work) above this track.
If you don’t want this problems, don’t split the ground. Use a single ground plane for analog and digital signals. But place the analog signal tracks in one region and the digital signal tracks in a different one and keep some distance (maybe > 10 mm) between them.
1 Like
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.