Ground plane a problem when wave soldering? - Page 1
Forum section: electronics / projects

author: Circlotron
author_rank: Super Contributor
timestamp: June 11, 2015, 04:41:20 am
content: Whenever I draw up a board I always put a ground plane on both sides. That way I don't have to worry so much about the routing of an earth track in and out of all the bits and pieces. Just pour a plane and make sure it can get to every nook and cranny and sprinkle vias around the place to join both sides where necessary to help things along. Have had great success with this approach over the years, especially where you have to watch out for large earth currents and the consequent voltage drop causing unexpected behaviour.Now it occurred to me that when a board with a large plane goes over a solder wave it would absorb more heat than usual because it is basically a large sheet of copper. Is this likely to cause a problem? I have seen some planes divided up into criss-crossed lines rather than a contiguous sheet. What is the purpose of this?

author: T3sl4co1l
author_rank: Super Contributor
timestamp: June 11, 2015, 05:02:29 am
content: I've seen hatching as well, but I think it's mainly for a copper density thing. You'll also see unconnected diamonds or other shapes strewn about (thieving), for the same reason.Obviously, such an approach would be murder to a multilayer board with high speed signals on it.I've never worried about soldering. The preheat and wave process should always be sufficient to heat the entire board to soldering temperature. The added mass of a little copper has very little effect, and the wave being a huge friggin' wave, there's little heatsinking action to worry about, unlike with hand soldering.Selective solder may have some issues, but I expect it's also good enough. Probably controllable/customizable enough to deal with special cases, too?If nothing else, you can ask a real assembler what they think -- it's their job to stick things on there! Of course, it's your part to see they can do it easily, otherwise you'll bear the added costs.Tim

author: IconicPCB
author_rank: Super Contributor
timestamp: June 11, 2015, 05:32:22 am
content: Not so much of a problem with wave soldering but a headache with reflow oven.

author: calexanian
author_rank: Super Contributor
timestamp: June 11, 2015, 05:59:11 am
content: Quote from: IconicPCB on June 11, 2015, 05:32:22 amAgreed. Wave soldering involves so much thermal mass, selective included, that it is typically not a concern. Reflow is an entirely different situation though. Especially with a hot air system. The cross hatching sometimes is don't for high frequency purposes. As a matter of fact last weeks Amp Hour show goes into it a little.

author: coppice
author_rank: Super Contributor
timestamp: June 11, 2015, 06:04:40 am
content: It is up to the PCB designer to sort out thermal management for manufacturability. Suitable use of thermal lands can overcome the great majority of heat conduction issues that arise from having large ground plane areas.

author: Circlotron
author_rank: Super Contributor
timestamp: June 11, 2015, 07:00:14 am
content: Okay. This is an 0805 footprint I have been using, showing it connected to a plane through thermal reliefs. No complaints from board loader either.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: June 11, 2015, 11:19:21 am
content: The only alert I get for stuff like that is if the tracks or spokes connecting to the pads are unbalanced between the two. Which is the case in the above example (one thin trace vs. four spokes). It could be equalized by using a thicker connecting trace, or restricting the number or orientation of spokes on the poly connect. The connections should also be mirror symmetric if possible, so that routing the trace to the end side of the pad (or in the inner gap, space allowing) would be preferred.But, it's not a big deal for 0805s and up, which are relatively unlikely to shift and twist or tombstone during reflow soldering, due to their size. It's a concern for 0603s, and even more so for smaller parts.Tim

author: matseng
author_rank: Frequent Contributor
timestamp: June 11, 2015, 12:44:04 pm
content: I've seen some wave-soldered old boards with a solid fill that got "crinkled". I thought that the main reason for doing a hatched fill was to avoid that effect. But I guess it make sense for balancing the amount of copper on the top/bottom side of the PCB as well. Does high end design software have build-in calculations for amount of copper for each plane?

author: IconicPCB
author_rank: Super Contributor
timestamp: June 11, 2015, 09:45:50 pm
content: Yes but it is the CAM software which tends to have a broader range of tools under the design-for-manufacturability flag as it is the PCB shop which knows its processes.

author: Circlotron
author_rank: Super Contributor
timestamp: June 11, 2015, 11:00:18 pm
content: Quote from: matseng on June 11, 2015, 12:44:04 pmI have seen that may times too but mostly on old style boards that had very wide tracks and large features. Not only on planes but also on tracks. I think it is the solder getting under the resist layer. Maybe there is maximum feature size below which the effect does not occur, so cut the plane up with hatching using a particular stripe width?

author: T3sl4co1l
author_rank: Super Contributor
timestamp: June 11, 2015, 11:44:25 pm
content: Wrinkled soldermask was due to SMOTC (soldermask over tinned copper). Probably using a film type mask as well. Modern process is SMOBC (bare copper), so there's no room for solder to float up along it.The bond is also better (liquid photoimagable, LPI, as opposed to a film stretched over the uneven etched surface), and usually of a compatible material (epoxy resin something or other?). Though the thickness is less (which however might be an advantage around SMT), and more uneven (being a liquid, it draws thin over edges and corners, and builds up slightly between and around traces).It's possible to get multiple solder mask processes applied, if you don't mind paying for custom processing. This includes multiple coats (improve insulation, plug vias?) or colors (yay, art?).Tim

author: Alphatronique
author_rank: Regular Contributor
timestamp: June 12, 2015, 01:09:02 pm
content: HIwave was less and less used today since vast majority of PCB was SMT ,as contract manufacturer i not start my since last 2 yearnow we try to use "past in hole" ,then for part that not support oven temperature we use selective solderingand whit the thermal mass of the solder pot , thermal plane was not a issue as long pad have proper pad thermal relief as IPC 2222as for re-flow issue ,if you use good True hot air convection re-flow that well profiled and whit proper thermal relief pad all will go goodproblem come that chiness relfow sold on ebay was IR type that not able to keep PCB whit good thermal spreadIR was absorb better by Black IC package so it hear more and reflected by shinny solder that act like mirror so not heat ,so it do invert of what need ...and most of time reflow belt was to short for have good profileas for hatched copper pour that was remain of 70-80 era when it have difficultly to etch fine trace whit big copper island ,but for long it no longer a issuesame for solder-mask opening bigger that pad ,that was require in past since registration problem , now need to put mask and pad 1:1 since registration was today really goodp.s. remember that in a wave you have a solder pot that contain 600 - 1200Lbs of melted solder ,so whit that kind of thermal mass PCB have no luck it will solder ;-)the plane or copper fill mass was very tiny in comparisonBest regardMarc

author: JuKu
author_rank: Frequent Contributor
timestamp: June 13, 2015, 09:22:39 am
content: Thermal masses play a big role in results, but the temperature profile the board goes through is equally important. With proper profile control reflow or wave pose no problem, with poor methods you'll get poor results either way.Thermal reliefs on pads solve most issues and make manufacturing much more reliable.On SMD passives, it is important to have equal solder tension on both pads. The smaller the part, the more risk of faults. The SMD image in this thread is a risk for tombstoning for 0603s and down: the side with one track will reflow first and the surface tension of the melted solder tries to lift the part vertically. The right way to do is to have a single track exit on both ends. Also, a pattern of bq will try to twist the part and might lead to short circuit between the pads.The criss-cross pattern is to make copper load equal on both sides of the board. A solid ground plane on one side and only tracks on the other tend to result to warped boards.