How to Design Spark PCB Heat Sink for 3 pin SMD regulator. (SOT223)
Consider the 3 pin SMD regulator (say a LM1117) where the heat sink pin is not in the schematic, but the PCB needs to have a Cu area that connects to the heat sink pin and the heat sink pin and heat sink area are electrically isolated and floating.
Position the 3 pin regulator and run the tracks to the used pins (In, Gnd, Out) and prove the Design Rule Check is error clear.
Create the floating Cu shape, <Add> <Shape> <Rectangle> <Right Click> <Change Layer> <Top Cu> and position it away from the heat sink pin. The shape can be sized and positioned later. <Right Click> <Filled Space> if necessary.
Add the Cu shape into a new NET, <Right Click> the shape <Add to Net> Make a new suitable name, maybe call it <Heat Sink>.
The spare heat sink pin of the regulator needs to be on the same NET as the shape, <Right Click> the pin <Add to Net> <Heat Sink>. The Air Wire will appear and the error is now about the Gap In Net.
To avoid the single pin net error, the regulator heat sink pin needs a track to terminate into another pad. <Add> <Pad> and place the new pad anywhere in spare space on the board.
The new pad needs to be on the same net, <Right click> the pad <Add to Net> <Heat Sink>. The new Air Wire will appear.
The new pad is by default as a through hole. It needs to be SMD. <Right Click> the pad <Change Style> and select any SMD pad style, or the same style used for the SMD component. It will throw a warning about the though hole being removed. This is normal. But because it was a through hole, it now needs to be forced to the top layer only.<Right Click> the pad <Properties> <Layer> <Top Layer>.
Run the tracks to replace the Air Wires. Error check is clear.
Size and position the shape to cover the heat sink pin and the extra SMD pad. Error Check is clear.
Now I want a gap in the solder mask over the heat sink Cu top side to allow a heat sink riser blade to be soldered on later to improve the thermal capacity. <Add> <Shape> <Rectangle> <Right Click> <Change Layer> <Top Solder Mask> and draw the solder mask gap for the blade.
Now I want Cu on the under side layer with VIA to further improve the heat sink area.
<Add> <Shape> <Rectangle> <Right Click> <Change Layer> <Bottom Cu> and draw the Cu on the under side. Use <Ctrl> <1>, <2>, <3> to switch layers or tick off under the layers tab.
The under side Cu needs to be on the same net, <Right Click> the under side shape <Add to Net> <Heat Sink>. The Air Wire will appear showing a connection is required to the top layer.
The top and bottom heat sink shapes can now be peppered with VIA to thermally and electrically connect the two shapes. <Add> <Via> (may times). The new protected via (s) will not have thermal spokes.
The final result is a heat sink for the regulator on the top and bottom side connected thermally by many via through the board and a gap in the solder mask layer (topside) for a thermal bladed to be soldered on later. The heat sink Cu is electrically isolated. The error check is free. Cu pours top and bottom function correctly.
The reason for this post is education for others and myself and questioning if anyone has an easier idea to produce the same isolated heat sink (top and bottom). Please note that this was a lot easier before the implementation of the quick patch just issued in V12.0 (Feb 2024). I agree with the need for the quick patch. I use Explorer level.
Previous to the patch, it was simple matter of adding a shape and running a track to the shape to snap the shape onto the same net as the pin, but this applies only where the heat sink pin was used in the schematic. This discussion is intended where the heat sink pin is NOT used and does not exist in the schematic, but the heat sink pin is used in the PCB for the component (as per the foot print for the SOT 223 having 4 SMD pads). I am aware that the manufacturers of the LM1117 have connected the heat tab to the output pin, but this is not always the case for other manufactures that use the same SOT 223 foot print.
Comments