No. A “Hole” in the sense of a NPTH (= Non Plated Through Hole, which is a technical PCB term) is a separate entity from a via.
A via is a drilled hole (plated in the PCB factory) but it always needs a ring of copper around it, because of the tolerance with which drills are placed on the PCB. Look up “annular ring” in the specifications of PCB manufacturers.
Consider that, regardless of what item’s of interest are called by various sources (software, people and companies) what you do for design should consider ‘who’ is going to make it (or, Not make it).
You see that JCLPCB does not make Blind or Buried Vias.
They all look good in Kicad but, need go consider manufacturing…
And, specific details should come from who is going to make it…
The manufacturer for me is the Workshop in my university. And yes, I am always adjusting my design to fit there demands. And In my design only through hole is needed. Thanks 
Thanks, and here I have another question : according to the demands from the workshop the diameter of a minimum hole is 0,3mm and the minimum annular ring width is 0,25mm, which makes the diameter of a minimum vias 0,8mm, and this is so large that short circuit is caused in some part of my design. So the guys from the workshop gave me another suggestion : using vias with so called ‘’ long pads’’ instead of normal vias, so some vias with little diastance to each other would be possible, so how do I put a vias like this in Kicad ? I couldn’t find it in PCB editor.
Will the solution offered be of help?
You still need the annular ring width to cope with the hole tolerances, so the overall width of the via will remain unchanged. All you do is extend the length by using a long pad.
KiCad calls these “oval pads”. Via’s are always round in KiCad. But using them as you show in your picture is not a good design. On the right side, where the hole breaks out of the side of the pad you get loose slivers of copper that can easily peel the pad off the PCB. On the left side a very narrow piece of copper is left, or nothing at all if the drill vibrates a bit during entry.
The best option is to reroute the tracks to conform with the design rules, and that means just using the 0.8mm vias. I would much rather use 1mm via’s with a 0.5mm hole as 0.3mm drills are very fragile and break easily. I once broke one just by dropping it on the carpet floor. Footprint placement is a very important part of PCB design. A PCB with a good footprint placement may be easy to route, while with a bad footprint placement, the same project may be impossible to route. And what is a “proper” footprint placement is a combination of:
Your next best option is to use a few wire bridges. One way to do this is to set up KiCad for a 4 layer PCB and use big via’s. You can then use an internal layer as documentation for where you have to solder the wire bridges. (Also consider that via’s are normally covered with solder mask).
What is the goal of this part of the university coarse? Is it to make a PCB for another project (Then use some bodge wires), or is the making of the PCB the main goal? (Then start by revising the footprint placement).
Hello, it’s to design a PCB for a ultrasonic measurement circuit.
And if I want to apply this vias with oval pad, should I creat one by myself ?
There is not much you can do with via’s, but you can add a test point symbol to your schematic, and then attach a test point footprint to it. Then you can manipulate the pad in the test point footprint to the shape and size you like.
Can you tell me more details ? Or maybe there is a tutorial for this ? Thanks 
Modifying footprints is quite simple in KiCad. The simplest is to first put it on the PCB, hover the mouse cursor over it and press [Ctrl + E] to load it in the footprint editor. The footprint Editor works very similar to the PCB editor, except that it works with the footprints and their attributes themselves instead of the PCB and tracks.
You can read the manual that is included with the footprint Editor (Help in the main menu) or the online version.
There is also a short introduction in:
There is also this older tutorial (Written for KiCad V5), but most of it is probably still relevant.
But I do recommend to also put the footprint into a separate library, and this involves a few steps.
And if you prefer video’s, there are probably tutorials for footprint design and modification on youtube too, but I have not checked.
And overall, remember that the schematic is the source of everything. If you change something about the location or name of a footprint, then you have to update the footprint link in the schematic symbol manually to keep everything synchronized.
Hello, thanks for the reply, I creat a footprint for a through hole with an oval pad according to your instructions and some other videos on youtube. Now I can find them in the library and place it wherever I want in PCB editor, but I cannot connect them with other components or pads through wire, I guess that’s because the connection should be first ‘‘defined’’ in the schematic editor, which means I have to first connect them in the schema and then route in pcb editor. Is that right ? If yes, do I need also creat a corresponding symbol for the through with oval pad ?
Yes, you also need a schematic symbol to add your custom “via” to the netlist. You can create your own schematic symbol or modify an existing one, but TestPoint_Small already looks quite unobtrusive and fit for your purpose.
Hello, I have tried to add several testpoints in the schema, after that I am going to choose a footprint for them. What I need is round testpoints, so I go to testpoint_loop. For example :
here what is the meaning of the dimensions ‘‘D2.6mm and Drill1.6mm’’ ? Maybe it’s via diameter and hole diameters ? If so, then it’s to large for me, what I need is a hole with a diameter 0.3 mm. And the minimum one in the footprint library is 0.9mm. Maybe I can download some footprint for smaller testpoint somewhere ?
And by the way, what is the difference of normal testpoint and beaded testpoint ?
The dimensions are indeed very likely the pad diameter and the “drill” diameter. But normally the number is treated as the size of the finished hole after it has been plated by the factory. But you can both easily measure it yourself with PCB Editor / Inspect / Measure Tool. And it also just an example. You want oval pads, so you have to change the pad in the footprint editor anyway.
The “beaded” test points have another 3D model attached:
For the PCB, there is very little difference between a footprint for a 0805 sized resistor or a 0805 capacitor. It’s mostly the 3D model that shows the difference. And it is quite common for footprints to be similar to other footprints.
Thanks, now I have placed the testpoint in the schema and update it to the PCB editor, and I can set the shap and dimentions of hole and pad in the ‘‘properties’’:
But there are no options for adjustment for the parts belong to layers ‘‘F.Silkscreen’’ and ‘‘F.Fab’’ ,for example the yellow and grey circle outside, means that a larger distance is needed while placing them in PCB editor, which causes problem in this designing because they need to be much closer. One possible way I find out by myself is : double click the footprint > Edit Footpringt… to switch to Footprint Editor where I could adjust or even delete the parts belong to layers ‘‘F.Silkscreen’’ and ‘‘F.Fab’’. Is this the proper way to do the adjustment ? Can I just keep the pad and hole:
Because all I need is a vias with oval pad.
Yes, using the Footprint Editor is the normal method for editing footprints. In addition, you can add some library management to create your own library (-ies) of the footprints you modified.
You can also easily create new footprints, and there are built in generator scripts in the footprint editor that can help with getting a footprint with a lot of pads started quickly.
And also, you have deleted two of your posts to post similar post immediately after that. You can click on the pencil icon at the bottom of your post to edit it.
@LF666
Please note that the post editing tool Paul demonstrates is only available for 24 hours after each post for Basic (Level 1) users, after which the pencil will disappear.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.
