can i set the via connector?
Thermal reliefs or direct etc/…
Without modifying the Footprint,
Is there any other way to fix it?
I’m guessing that English isn’t your first language (your avatar looks like Korean to me, but I could be wrong). Welcome to to the forums. 
If any of the terms or phrases that I use below don’t translate well (either to your language, or even just to your understanding), please don’t hesitate to ask for clarification.
I want to gently let you know that the term “via” is a very specific board feature, and not what I expect you mean since you ask about modifying footprints. The holes in footprints for component legs are usually called through-holes, often abbreviated as THT (this means “Through Hole Technology”). Vias are only the holes through the board for carrying a signal, not intended for soldering components or wires to. Most vias are unrelated to footprints.
That said, you may be asking about what look like vias in a footprint, used to stitch a ground or thermal pad to both (or several) copper layers in the board. But because they are part of a footprint, KiCad still considers them through-holes not vias.
Now, to your question:
Short answer:
Look in the copper zone settings. This will apply to ALL the pads in the copper zone. See below for more details…
(very) Long answer with pictures and everything:
The connection of a through-hole in a footprint to filled copper area has multiple settings, each with priority over the other. For this explanation I’m looking at the provided “LFCSP-8-1EP_3x3mm_P0.5mm_EP1.6x2.34mm_ThermalVias” footprint in the “Package_CSP” library, and this is what it looks like in the footprint editor:
Note the multiple through-holes numbered 9 that are all in the front copper surface mount pad also numbered 9. Because they all have the same pin number and overlap each other, KiCad knows that they are all electrically the same connection in the netlist. If I select one of the through-holes numbered 9 and go into the pad properties, and then select the middle tab I see this:
The bottom section labeled “Connection to Copper Zones” is used to control the thermal reliefs and will override any other setting for this specific hole. The “Pad connection” has 4 settings in the drop-down:
As you can see, this footprint was designed to allow the footprint definition to control the copper zone connection, but it can be changed for this pad, and this pad only. This setting will not affect the other pads in the footprint, even if they have the same number.
Going up one level to the footprint settings, we need to be editing the footprint properties. This can be done in the footprint editor by either selecting the menu item “File/Footprint Properties…” or by clicking this button in the tool bar:
In the footprint properties window you will want to, again, select the middle tab. And you should see this:
Like in the pad properties window, the bottom section labeled “Connection to Copper Zones” is used to control the thermal reliefs and will be valid for all pads (THT and SMT) in the footprint and will override any settings in the zone, but will not override any pads that have a setting other than “From parent footprint”. The “Pad connection to zones” has 4 settings in the drop-down:
Note, if you select “Thermal relief” here, I’m not sure where to define the spoke width and thermal clearance for all the pads in the footprint. This might need a separate discussion since based on your question I don’t think you care about this at this point.
Going up one more level, brings us to the Zone properties mentioned in the short answer. Here I have the zone properties that opened up when I started drawing a copper zone while in the PCB editor:
The lower middle section called “Pad connections” is where you would configure how all pads that are in the copper zone with the same net as the zone will connect if there are no other settings overriding this one. This drop-down has 4 settings, but they are different than the settings in the footprint editor:
I hope this helps you decide which setting that you need to use for your application. Note, once a footprint is loaded into the PCB editor, it is copied into the PCB file and changes that you make to the footprint in your library won’t automatically propagate to your PCB. You have to manually update the footprint from the library. This also means that if you edit the footprint in your PCB then the changes you make there will not propagate to your libraries.
This can be useful for making custom one-off edits to a specific footprint in the PCB (like in your case changing the zone connection properties). Even if multiple components use the same footprint (let’s say for example’s sake, U2, U5, and U6 all have the same footprint). If you edit the footprint for U5, the changes you make are only for U5. U2 and U6 will not be affected by the changes you make. But there are a couple ways to update all footprints from the libraries which might wipeout the changes you made to U5 if you aren’t careful. This is why many people (myself included) would suggest copying the footprint that you want to change to a project library, make the edits to the footprint in the project library, and map the footprint for that component to the edited footprint in the project library in the schematic.
2 Likes
GNDREF is a thermal pad,
VBAT, UART-RX is VIA.
VBAT and UART-RX are normal pads(Direct pad).
Can VIA be changed to a thermal pad?
No. The upper VBAT and UART_RX are not normal pads, they are not pads at all, they are only vias. A pad is something which is used for soldering. If you need a pad, you have to create a footprint with a pad. Vias are used only as tracks which happen to go through the board, therefore it doesn’t make sense to have thermal connections for them. Either they are connected to tracks in which case thermal connection isn’t possible in any case, or they are connected to zones (planes, copper areas) in which case they connect to the zone as efficiently as possible, without thermal reliefs. Thermal reliefs are used in pads only because they make hand soldering easier. Otherwise solid connection would be better even for component pads.
I think he may have mis-typed. I took the second line you typed to mean “VBAT and UART_HAWK are normal pads(Direct pad).” Though I’m not sure what he meant by direct pad. Looks like a single pin footprint.
@seungyeon.won
Looks like GNDREF is part of a footprint because it has a pin number, something vias don’t have. Further GNDREF looks to me to be a SMT (surface mount) pad, not a THT (through-hole).
If you drop a via using the tool you highlighted into your copper fill anywhere there isn’t another trace on the opposite side, for example between the GNDREF pad and the UART_RX horizontal trace but not touching either, you will get a via that will automatically connect to the net of the zone. This is often used for via stitching. This via won’t have thermal reliefs.
I’m confused what your end-goal is. It may not be a via, so knowing your intent can help figure out the proper technique. You ask:
So you want thermal reliefs on a via? Why? Thermal reliefs are primarily intended to provide some thermal resistance between a pad that you are trying to solder to and to the copper zone which acts like a heatsink. Since vias aren’t intended to be places that you should solder to (usually), KiCad doesn’t put thermal reliefs on vias.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.