PCB Design: How to avoid tombstoning?  - Page 1
Forum section: electronics / general

author: LooseJunkHater
author_rank: Frequent Contributor
timestamp: December 15, 2023, 06:54:33 pm
content: I'm designing my first PCB using KiCad and I've been struggling to find very much information onlinehow to avoid tombstoning of small SMD componentslike resistors and capacitors when designing a PCB. Does anyone have any video references on this topic? I couldn't find anything made by Dave either. Thanks.

author: PeteH
author_rank: Unknown
timestamp: December 15, 2023, 08:01:38 pm
content: I haven't seen much tombstoning with advanced modern assembly houses, tuned processes.You can make it less likely to happen by just making sure both sides of these components have equal copper balance.I.e. thermal relief, or enter and exit the pads in the same way if it's not plane connected. (I.e. don't put a 2mm trace on one side and a 0.2mm trace on the other... Or a via in one pad to 10 copper planes vs a small trace on the other pad .. etc)Symmetry promotes equality during reflow.

author: ajb
author_rank: Super Contributor
timestamp: December 15, 2023, 08:35:42 pm
content: The important thing here is to make sure that both pads of each chip component reflow at about the same time. If one side liquefies before the other, the surface tension of the solder on the end cap will pull that end into the joint and lift the other end out of the solder, and voila: tombstone.In addition to copper balance as PeteH mentions, watch out for thermal 'shadow' effects from other components. The thermal mass of a big heavy inductors or something may suck heat away from one side of a chip component that is too close.Quote from: PeteH on December 15, 2023, 08:01:38 pmYeah, any half decent CM should be able to make any reasonable design work, and should tell you if they foresee an issue with your design. But as long as you haven't got a tiny track one one side and a massive copper plane on the other, most chip components > ~0402 shouldn't be much trouble.

author: jmelson
author_rank: Super Contributor
timestamp: December 16, 2023, 07:04:15 pm
content: Are you going to assemble the board yourself or have it assembled? I have done over 2000 boards in my own shop since 2007, and have had maybe 5 tombstone parts. Now, using GC10 solder paste, I have not seen even one in the last few years.It is all in the solder paste and the even-ness of the heating cycle of the oven. I actually use a "GE" toaster oven with a thermocouple controller.Jon

author: Infraviolet
author_rank: Super Contributor
timestamp: December 16, 2023, 08:56:32 pm
content: Can't speak for industrial scale systems, but when pasting by needle by hand, then putting through a reflow oven, I always found the key factor in whether tombstoning would happen was whether the amount of solder paste put on each side of the passives was equal. If it was unequal, then tombstoning might happen, although it was only for perhaps 1 passive in 40 very unequally pasted ones. It mostly affected 0603 resistors, but slightly bulkier and heavier 0603 capacitors would sometimes do it to. Never saw it happen with any bigger passives.

author: peter-h
author_rank: Super Contributor
timestamp: December 31, 2023, 03:13:34 pm
content: The solder quantity will be determined by the stencil, so the main thing is to- use equal size pads (obviously this is normally the case anyway)- use pads which are not excessively big (too much excess area -> too much "pull" on that component end)It can be a problem if e.g. you have a 1206 pad and you are placing an 0805 component there. But probably not if the pads are equal in size.

author: Feynman
author_rank: Regular Contributor
timestamp: December 31, 2023, 08:35:38 pm
content: For professional assembly shops the main reason for tomb-stoning usually is wrong footprint/stencil design. An assembly shop will probably optimize your stencil, but not your footprints. So just ask your assembly shop for a well-proven footprint for passive components. A common mistake are the pads being too big, because often times designers re-use footprints intended for manual soldering.Copper balance usually isn't a big concern in automated soldering processes since the entire board is heated up evenly.

author: free_electron
author_rank: Super Contributor
timestamp: December 31, 2023, 09:14:33 pm
content: as stated before : footprint design and copper breakout.The volume of solder needs to be the same on both pads. But there are other things to look out for :- soldermask : tighten that thing up. Board shops cando 0.05mm over copper these days.- routing : equal amount of copper leaving the pad. The little bit of copper wicks solder during reflow and can cause an imbalance. This is important with very fine pitch parts like 0402 and 0201 or 01005. The stencils are very thin and there isn't much solder to begin with. For things like 0201 and smaller you may want to switch to solder mask defined pads- thermal balancing. Both pads should heat the same. Be careful with planes under a part. They can wick lots of heat. Parts should not sit on plane boundaries or overhanging plane edges. 1206 and larger is ok but the little snot can be problematic.- pad design. The pad should NEVER extend beyond the electrode under the body of the part. ( for passives like 2 pin parts. ) having paste there (even when squashed duting the actual placement) there is a risk for balls to form. they may push the part off the board.

author: Malik Xiong
author_rank: Newbie
timestamp: January 08, 2024, 04:07:33 pm
content: 1. Control the Reflow Profile: Ensure the reflow profile is controlled correctly to avoid rapid heating or cooling which can result in unequal expansion and lead to tombstoning.2. Component Placement: Place the surface mount components precisely at the center. Even a small shift can cause an imbalance during the reflow process.3. Pad Geometry: The pad design and dimensions for the component should be according to the manufacturer's specifications. Different sizes can cause an imbalance in the heat and surface tension.4. Solder Paste Printing: Ensure the solder paste is printed uniformly across all pads. Unequal solder paste can exert unequal forces during reflow causing the component to lift.5. Quality of Components: Use good quality components that are free of defects. Defective components can have uneven weight distribution causing them to lift during reflow.6. Proper Storage: Keep the components properly stored to prevent moisture absorption which can lead to tombstoning.

author: coppice
author_rank: Super Contributor
timestamp: January 08, 2024, 04:16:39 pm
content: Don't avoid Tombstoning. If you are in Arizona visit Tombstone. Its a very interesting slice of the past.

author: Selectech
author_rank: Regular Contributor
timestamp: January 08, 2024, 04:38:20 pm
content: Tombstone was depressing & boring. Bisbee, AZ much more interesting.

author: coppice
author_rank: Super Contributor
timestamp: January 08, 2024, 04:45:06 pm
content: Quote from: Selectech on January 08, 2024, 04:38:20 pmIts depressing to realise that Arizona took so long to become a state, because they didn't want to end the enslaving of Chinese mine workers in places like Tombstone. However, things like the signs in the graveyard reminding you its a real graveyard, and not a movie set, amused me. Those signs are really needed when you read the bizarre inscriptions on some of the graves.