Thermal reliefs - Page 1
Forum section: electronics / general

author: Simon
author_rank: Unknown
timestamp: October 19, 2020, 01:40:11 pm
content: In the past I did a PCB with a ground plane and no thermal reliefs and passive parts tombstoned (0805/1206). Is a thermal relief the only way to stop this? At the time the footprints i had used were my own design taken from the part datasheets which often had 3 options with few details and they were quite spaced out.Does the pad centre compared to the part centre affect/control this?I am using kicad with the standard footprints for passives.

author: SMTech
author_rank: Frequent Contributor
timestamp: October 19, 2020, 02:59:21 pm
content: I have no idea what a Kicad standard footprint looks like, but the first place to look is always thermal balancing. If one pad is essentially just a gap in your solder mask straight onto a massive plane of copper and the other is a pad with a little trace on it, you're asking for it. That said, bad footprint dimensions can also cause this issue, we used to have an 1812 fuse that tombstoned all the time, the pads were quite a long way under the device, switching the package to the same size but with a tiny semicircular notch in the end of the pads stopped the tombstoning in its tracks but I would have said the footprint itself was probably wrong. How does the Kicad pad compare to the IPC spec? IIRC there are two standards, the older one often has less solder/pad 'outside' the device and more underneath and I think was more suited to SnPb pastes.

author: tszaboo
author_rank: Super Contributor
timestamp: October 19, 2020, 03:08:48 pm
content: One way to control it is to send it back to the PCBA fab, and tell them to learn how to setup their reflow oven. Tell them nicely that you are not paying for the dog turd that they sent you until they fix it.There shouldn't be tombstoning on a 1206, even if you had 4 layer board (indeed, if your footprints are good) The most optimal layouts for power supplies, RF, high power stuff, etc calls for direct connection, and it is a problem for the assembly house, and not you.

author: Simon
author_rank: Unknown
timestamp: October 19, 2020, 03:40:38 pm
content: Quote from: NANDBlog on October 19, 2020, 03:08:48 pmIn this case I am the assembly house but I also do not want to make life hard and therefore expensive in production.When i had the issue before I don't thing the entire component pad sat on the PCB pad. Sounds crazy but I followed the datasheet of a resistor and capacitor. These datasteets did have 2 or 3 versions of footprint with no further explanation.So It looked like as the ground plane absorbed heat faster that solder melted and as the part pads were not fully on the PCB pads the ground pad won and pulled the part to it sometimes tipping it up. It may have been the other way around as the ground heated up more slowly but same process.So I redid PCB pad's with them closer so that the component pads sat fully on.But i am trying to play safe on this design which um yes needs to pass stringent EMC so i would rather not have thermal reliefs.Looking at my last KiCad design I have no thermal reliefs and it worked fine so maybe I am just panicking over nothing.

author: kylehunter
author_rank: Regular Contributor
timestamp: October 19, 2020, 04:58:35 pm
content: Quote from: NANDBlog on October 19, 2020, 03:08:48 pmWith all due respect, that just isn't right, there's so much wrong in your post...Yes, 100% 1206's/0805's shouldnottombstone, regardless of what is going on with the layout/oven.We are a design shop and assembly house. We do the assembly for both our designs and outside designs. There is just as likely going to be a tombstoning issue from a design issue as there is a reflow oven issue. Unless you were only referring to the 1206's in your post, to put the blame of tombstoning defects 100% on the assembly process is more often than not going to be wrong.If I take an 0402, I canmucheasier force it to tombstone by using a solid plane on one pad and an 8 mil trace on the other than I can by doing a super fast ramp profile in our oven."for power supplies, RF, high power stuff, etc call for direct connection, and it is a problem for the assembly house, and not you."That is true, but again, it's all about thermal balancing on the pads. Your super fancy and important high power resistor wouldnothave a solid pour on one trace, and a 8/10 mil on the other. If it did,youare responsible for the tombstoning issue,notthe assembly house.

author: SMTech
author_rank: Frequent Contributor
timestamp: October 19, 2020, 08:38:54 pm
content: Yeah you can maybe, maybe reduce tombstones caused by other factors by adjusting profile but you won't solve the problem and that's assuming the other factors that set your profile allow changes (large parts, sensitive parts, the paste, the board density, the targeted throughput). Most CEMs probably work with a small handful of generic profiles they have developed for certain sizes of board, in the real world its not realistic to create bespoke profiles for every product.However in a lab/DIY setup an tabletop IR oven or similar could well have very uneven heating anyway which would make matters worse, as would excessive paste, poor pad design or poor aperture design. You might even be able to keep the layout and work on those other areas and make the problem almost vanish. Also if your placement process has just dropped the parts on the paste that can contribute (e.g a wrong component height in your pick and place setup).The board I was building today broke several rules to no ill effect, pads too small for parts, poorly finished chinese stencil, copper fill on the bottom and just traces on top, could easily have resulted in mid chip solder balls, tombstones and warped boards but were in fact fine bar the odd short on QFPs, there's a lot going in the whole process that can contribute to a problem.

author: tszaboo
author_rank: Super Contributor
timestamp: October 19, 2020, 10:13:29 pm
content: Quote from: kylehunter on October 19, 2020, 04:58:35 pmIf you search for " tombstoning study" , you will find several papers, where they investigate 0201 and smaller compoents, with intentionally bad designs, where they have a few ppm errors. Those are components that are 100 times smaller than a 1206. BTW it is not "just as likely". That's like saying it is just as likely to die in a lightning strike than anything else. Biggest error sources:Component is not placed where they supposed to be.Wrong soldering profile.There is no excuse for this. If you get parts like this, you send them back for repair, because:1) It shouldn't happen in the first place.2) AOI should've found it.3) You defined that you wanted working boards, with all the components soldered to it. IPC-610 and all.Yes, and there will be a bunch of blog posts online, saying that "bad thermal design causes it". And it did, in 1990, with vapor phase soldering. Or in 2020, when they rush your order, and dont let it preheat properly.

author: Simon
author_rank: Unknown
timestamp: October 20, 2020, 06:53:51 am
content: You seem to be missing the fact that I did this myself. Can't remember the parts probably 0805 maybe I was using 0603 by then. So I managed by bad design to get them to tombstone.

author: tszaboo
author_rank: Super Contributor
timestamp: October 20, 2020, 01:26:07 pm
content: Quote from: Simon on October 20, 2020, 06:53:51 amYes, I was. Sorry, rant over.Preheat the board for longer, that should help.

author: wraper
author_rank: Unknown
timestamp: October 20, 2020, 01:32:19 pm
content: Ways to control tombstoning are thermal reliefs, footprint (matters a lot), amount of solder paste/type of solder paste and reflow temperature profile. Unless it's for connector mounting pads or, things needing heat transfer to copper or heavy (in regards to pad area, say sot-23) things which simply cannot tombstone, just use thermal reliefs. 0805 capacitors with square cross section are really hard to tombstone, resistors and other things which are thin on the other hand are not.