Does anyone know how to create a heat dissipation pad around the pins of an IC as in the picture?
I already saw Chris’s tutorial on youtube however I don’t get it. Does anyone have an explanation for absolute beginners?
I think that is just a copper pour/zone.
What Part Number is this device?
ADuM6000
I am skeptical about just a copper pour/zone. Is it supposed to be covered in solder mask?
Didn’t you read the text in the datasheet?
Implement multiple vias from the pad to the ground plane to significantly reduce the temperature inside the chip. The dimensions of the expanded pads are at the discretion of the designer and depend on the available board space.
1 Like
In my design both the top and bottom layers are ground with vias to connect them.
What I am asking is not if the pad should be connected to ground. I am asking if I want to make such a pad (which I don’t know if it’s a part of the top ground fill or separate so for example it won’t have solder mask? But then again I don’t know if it needs solder mask or not? Will solder mask ruin heat dissipation and therefor should be avoided?) How is this technically done in KiCad?
I need a simple tutorial on how to make such a pad in KiCad. Even if you say it is part of the copper pour I challenge you further: Is it going to have solder mask over it? If not how can I make this possible?
I thought that the text explained it. The solder mask is irrelevant if there are vias in the pad which dissipate the heat to the other side of the board which then has a larger copper area. Almost never the copper is exposed for thermal conduction in normal designs. If better conduction is needed then other means are used, like heat sinks. But you can make the “pad” bigger on the top side, too, if it fits for your design geometrically and electrically.
I have made such pads or other comparable larger copper pours with zones. If you really want to expose copper you can create a zone in the mask layer, too, which makes a hole in the physical solder mask.
3 Likes
Thank you however I tried “just making a filled area” AND changing the two pads’ nets to ground but what happens is that after filling/refilling they look like this with no full fill:
Additionally, take into consideration the fact Chris chose to make this tutorial for a reason:
I want to know how to just make a square fill around those two pads exactly like the datasheets recommend.
open the pad properties and set them to “solid” currently it has thermal spokes to make soldering easier,
You can also reduce the “clearance” setting on the zone to make it paint closer to the other pads,
To put it short I have 3 questions:
1: Do you put solder mask over the area that is supposed to be a heat sink or not, judging by the above datasheet screenshot?
2: How do I make a pad and have it fill up?
3: If no solder mask should be over the pad how is this achieved?
- if your using a corrosion resistant plating, e.g. “enig” then you can leave off the solder mask, doing so will decrease the thermal resistance to the air it is in contact with, however the area you need can be calculated based on the amount of heat you expect it to produce (how much wattage),
I would expect the datasheet to reflect with soldermask on, however sometimes they set crazy conditions in order to work with the listed size, e.g. fixed 25C ambient temp.
-
I assume you mean a solid zone connection to a pad, right click the pad, open pad properties, and set the pad to “solid” this will make it join zones with a solid connection, without spokes,
-
If you wanted no solder mask over the zone, you would draw a zone on the soldermask layer, this remove soldermask for that area.
How do I know what plating I am using? I am using Osh Park just in case that helps? If I leave the solder-mask on will be sinking heat properly or does that effect it greatly?
OHS use purple boards with an ENIG plating (gold plating), not having solder mask on helps a few % in still air, more in forced airflow,
The issue with removing the mask is it creates a risk of something conducting across the isolation barrier as it increases the area dust or other detritus can build up while in contact with a pad.
Looking as the datasheet, Its maximum dissipation is about 0.9W at 5V 80mA, The chips temperature raises by 45C/W, so about 40C above ambient with no zones or anything,
Reading below where you have screenshot is the majority of what they are recommending, to have a copper area above and below the chip, stitched with vias to reduce that temperature rise,
If your not operating it anywhere near that maximum power output, it will be fine with minimal zone filling and I doubt you would need soldermask removed to gain anything significant.
2 Likes
Thanx!
If my project uses top and bottom layers are ground fills, and top is anyways going to be ground will I still need the pads? Or do I just rely on the fact that the top layer is ground fill anyways?
What about filling with solid connection for this part of the board and thermal connections for the rest of the board? Will having a pad in addition to the ground plane (and somehow connecting both) help?
This is what I have so far:
Because you have the capacitors on the opposite side, I would recommend you have ground vias to connect to them right near the converters ground pads, This is primarily to close the loop for the capacitor currents, but If you fit multiples grouped near the pins it would sink a fair bit of heat to the other side aswell
If you are running ground fills on both side, you will get significant heatsinking through the planes it connects to, but fibreglass is an insulator so without vias between, the heat will stay on 1 side,
Equally if you need it isolated to a certain voltage, dont forget to draw a “keep out zone” between the 2 planes to ensure a suitable gap,
Thanx again.
I still have a question: If I understand correctly, when I am in the copper fill menu I can choose if the connection to certain pads will be full or not (for soldering purposes so it will heat up and will be solder-able). I want that the ground plane should be fully connected to the pins on the ADuM6000 (as the datasheets suggest) but only partially connected to other pads. Will the fact that I have a ground pad around the ADuM6000 pins and in addition a general ground copper fill achieve this? Will I be able to ask for a partial connection of pads to ground while at the same time a full connection of the thermal relief pad to the pins?
The zone filling follows the pad mode first, e.g. your ADu’s “solid” pins, then by the zone properties, so if you have the chips pins set to solid and leave the zone as thermal, only the ADu pins will be solid.
1 Like
To have those caps on the other side will be like not having them at all.
1 Like
Care to elaborate? Why won’t the same caps connected to the same net not do their jobs?
The via adds to the serial impedance. For such caps you want that impedance as low as possible.
Where is the connection of 3v3 to the rest of the board?
Make sure the pin connects first to the capacitor and then to the rest of the board. (again impedance control)
All of the mentioned things are important if you care about electromagnetic compatibility. (If you want your device not to send out EM waves or be influenced by such waves received.)
There is enough space on the top side so why not put the caps there and have a board that is better in that regard?
Also you capacitor footprints look like they are the old bad handsolder footprints from the oficial library. Their pads are way too large. (Sadly the normal version is too small) There is a reason we replaced these footprints in the new version 5 lib.
My suggestion would be you download the capacitor footprints you need from the new lib and place them into a personal lib. (We will publish a kicad 4 backport of the whole lib within a week or two from now. Until then you can not simply use the new lib in kicad 4 as it does not work if any footprint in a lib has a unsupported feature within it.)
To download them head over to the https://kicad.org/libraries/download/ site and download the capacitor_smd lib as a zip archive. Use a file manager (of your operating system.) to copy the cap sizes you need from this to a .pretty directory somewhere in your personal folders. And add that .pretty folder as a library to kicad using the library wizard found in pcb_new -> preferences
1 Like