Hello, I’m trying to connect the pad below as a thermal relief pad to the copper area surrounding it. Appreciate any guidance on this.
There are different ways to do it. The most common method is to edit the properties of the zone itself. It has a setting for thermal reliefs.
You can override the settings for the zone by either modifying the properties of a footprint, or the properties of a single pad. For example in the drop down menu when modifying pad properties.
And this is of course also mentioned in the manual, available in the menu via Help, or an online version on the KiCad website.
1 Like
I had already set the pad set to thermal relief like this
but it still doesn’t show a thermal relief connection and if I click on the component (so the copper bit, not the actual pad) is also set to thermal relief. I’m wondering if I should ‘hardwire’ the thermal relief in the library itself.
Here is a clearer picture
The pad needs to be on the same net as the zone.
1 Like
The zone is just a free fill area - I can’t see a way to connect it to the pad in the free fill zone dialog box.
Thanks
Go to the zone’s properties and set the Net . . .
When you created the fill zones you should have assigned them the same net as the pad. You can still edit that.
I cannot find the zone properties dialog box like you have. If I right click on the zone and select properties this is what I get
It’s the same, I’m on V8 are you on V7 ?
Meh, to me they look the same. I guess Bonsai is confused because you only made a screenshot of a part of the dialog instead of the whole window.
And this brings the question back to:
So, What is the net name of those tracks connecting to the heatsink pads?
I’ve checked, the central track between the two pads is GND, checked the top and bottom copper fill and they are also GND but I still cannot get a thermnal relief connection. I am at a bit of a loss here (I’m on V7 - not transitioned to V8 yet)
I doubt the Track on bottom layer that connects the heat-sink(?)-pins and the fill are the same net.
If they were the same net, the Fill wouldn’t make a coutout for the tracks.
Double check the actual net of the track. Then select the same net for your fill.
1 Like
Click the track then look at the details at the bottom of the KiCad window . . . just to be 100% sure its on the GND net
1 Like
If all else fails, then upload a simplified version of your project.
It should at least contain:
- All project files.
- Schematic with the voltage regulators, something to connect those voltage regulators too, and the heatsink.
- The PCB file with those parts.
You can delete most of the other parts from both the schematic and the PCB files if you don’t want to share the whole project.
Hello, I am back to trying to resolve my thermal relief pad problem. I’ve checked and the pads I want connected to the copper fill zone are labelled GND and the two copper fill zones are connected to GND (via the pull-down menu when right mouse clicking on the copper fill zone).
The copper fill zone is not being rendered in the 3D viewer and when looking at the PCB layout, the copper fill zone is not shown as a thermal relief pad.
I’ve got a thermal relief to a copper fill area on a different component working ok in another project - but this one refuses to cooperate.
I have updated the footprint to show the pads are thermal relieve in the footprint library and then updated the symbol on the schematic, and then from the schematic to the PCB.
I’ve attached the project file (nothing fancy, just a bog standard jelly bean linear PSU)
Appreciate it if someone can point me in the right direction.
Regards
A
Linear PSU Thermal Relief Issue.zip (3.8 MB)
Just pressing b to re-generate internal zone geometries shows the thermal reliefs. Both in the PCB editor and in the 3D viewer. (I disabled solder mask to make the copper more visible).
But also, In this application it is both useless and (probably) bad practice to use thermal reliefs here. It’s useless because these heatsinks have thick sturdy pins, and to solder them, you pretty much have to heat up the whole heatsink. It may be bad practice because during operation the extra copper on the PCB works as a heatsink too. Especially when it’s the only heatsink this effect is significant, but compared to a big chunk of aluminium it is negligible, especially when there is no airflow because it is also covered by the heatsink itself. For this reason, I would not bother at all with adding an extra zone under the heatsink.
Also, you can always safely release the fp-info-cache file, and you never have to back it up. This shrinks zip files significantly.
You also do not have to backup the backup directory, or intermediate gerber files. (I only archive gerber files if they are the actual files used to order PCB’s.
After removing the stale lock file too (It should not even exist when all KiCad instances are closed) your zipped project shrinks from 3.8MB, to 150kB
2024-07-13_Linear PSU Thermal Relief Issue.zip (150.4 KB)
Concerning the schematic:
Adding a connector to pin 3 of U2 makes it possible to use the outputs as two independent 15V supplies, or to parallel them for more current (probably with some balancing resistors (long PCB tracks?)) Do be careful with mouting the voltage regulators onto the heatsink. the GND (tab) of U2 is on a diferent voltage level, and the poor thing will be shorted out if it’s mounted withhout isolation pad and washer.
D3 and D4 are also (mostly) useless. They have some limited application when there is a possibility when the input (between the rectifier bridge and the voltage regulators) gets shorted. In that case they form a high current path for C6 and C7 to discharge quickly. That is the only use for those diodes. But even if you do not mount them, reserving a bit of space for them on your PCB is not bad either.
1 Like
Fantastic - I was unaware of the ‘b’ thing and disabling the solder mask to get a better view. Thanks for that.
The PSU will only ever be used in a split 15-0-15 mode, so FP1 is just there for debugging if ever needed.
Sure, but the cheap Chinese PCB factories sell about 10 PCB’s for the price of one, and with very small tweaks it’s a pretty universal dual power supply that you can also use in other projects (and other (different) voltages and such)
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.