PCB routing - Polygons and thermal reliefs - Page 1
Forum section: electronics / projects

author: Nikos A.
author_rank: Regular Contributor
timestamp: May 03, 2021, 07:39:48 am
content: Hi everyone,I design a PCB and I have placed a polygon for thermal dissipation across with a couple of vias. Do I have to include thermal reliefs?Design with thermal reliefsDesign without thermal reliefsIn my opinion I believe that I have to include thermal reliefs if I will solder by hand but in case of a professional assembler is it really required?Nick

author: Evan.Cornell
author_rank: Regular Contributor
timestamp: May 03, 2021, 12:26:16 pm
content: Option #2 looks better to me.

author: mjkuwp
author_rank: Unknown
timestamp: May 03, 2021, 01:01:10 pm
content: This is a great question.Is it practical to extend the copper beyond pin 8 and put some vias to the bottom layer on the other side of the chip?Of course *after* assembly you will get the best heat dissipation the more copper you have. However you also have to consider the process. Consider the possibility of rework that may be required. With no thermal relief rework may be very difficult.You mention professional manufacturing so one option would be to ask the assembler.my humble opinion is to split the difference. Use thermal relief but add a trace about 2x as wide as what you have (just pads 7 andand also bring the connection out the other side if you can.Do you know how the part and package are built? Is there an expectation that the pads in the corner can carry energy from the chip package? I wonder if the pads 7 and 8 are specifically placed for transferring energy/heat and so there wouldn't be a need to connect the corner pads so robustly to the copper.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: May 03, 2021, 01:55:12 pm
content: I would rather leave the spokes in, place vias in the middle pads, and connect to both sides of the package.Tim

author: Nikos A.
author_rank: Regular Contributor
timestamp: May 03, 2021, 02:46:48 pm
content: Quote from: mjkuwp on May 03, 2021, 01:01:10 pmI will assembly the prototype by hand and then if everything goes fine I will assign the job to a manufacturer. So, probably it is a good idea for now to proceed with thermal reliefs and just increase the track width to double as you advised.Quote from: mjkuwp on May 03, 2021, 01:01:10 pmNo I do not have such information, this is the datasheethttps://www.ti.com/lit/ds/symlink/csd85301q2.pdf?ts=1620050248631&ref_url=https%253A%252F%252Fwww.google.com%252FProbably I overdid it with the vias and the polygon pour size and I have to reconsider.

author: Nikos A.
author_rank: Regular Contributor
timestamp: May 03, 2021, 02:59:49 pm
content: Thanks for your post TimQuote from: T3sl4co1l on May 03, 2021, 01:55:12 pmYou mean something like this?

author: T3sl4co1l
author_rank: Super Contributor
timestamp: May 03, 2021, 03:15:55 pm
content: Yes, although probably just one via per inner pad.Tim

author: phil from seattle
author_rank: Super Contributor
timestamp: May 04, 2021, 01:16:41 am
content: Thermal reliefs work to contain the heat to the pad itself so you can solder easily. But that is exactly what you don't want for a high power device. I just hand assembled several boards that have no thermal reliefs on the voltage regulator tab. While it took extra heating, I was able to solder it just fine. I wanted to test the power subsystem so needed to not have thermal reliefs.You can use a hot plate to heat up the board if it causes problems.

author: Doctorandus_P
author_rank: Super Contributor
timestamp: May 04, 2021, 01:53:15 pm
content: I fully agree with Phil.If you want to use copper fill as a heatsink then never use thermal via's, as they defeat the purpose.For normal SMD reflow, the whole PCB is heated to soldering temperatures anyway, so thermal via's are mostly for hand-soldering and for easier repair.Another use of thermal via's for automated PCB manufacturing is to improve manufacturing yield and reduce rework. If you have for example SMT resistors, and one is connected to a plane, and the other to a narrow track, then one pad will heat slower then the other, and this increases the tendency of "tombstoning"

author: T3sl4co1l
author_rank: Super Contributor
timestamp: May 04, 2021, 05:47:14 pm
content: Quote from: Doctorandus_P on May 04, 2021, 01:53:15 pmThink that was a typo, meant thermal relief?I somewhat prefer spokes / thermal relief, as it defines the pad shape. With solid pour, the pads become solder mask defined (SMD). Soldermask is by default expanded relative to the intended pad dimension, and has lower precision. This worsens soldering quality.The soldermask opening can be reduced to match the pad properly, and LDI (laser direct imaging) can be chosen at the fab for greater precision -- but also greater cost as this will be a custom option.There is still some value in leaving spokes for SMTs: the pads are heated through the component and flux, while the PCB core can actually remain somewhat cooler. Exactly how much of this happens, depends on the process; with IR reflow this would be especially significant I think, while for vapor phase or convection it shouldn't be as significant.I have seen cold solder joints / head-on-pillow failures on devices with large, direct connected pours.And yes, as mentioned, you want copper balance on small chip parts. (It shouldn't be an issue for multi-lead or DFN style parts, but spokes are still a good idea for even melting, and hand soldering should it be necessary.)Tim