What are the advantages and disadvantages of thinner PCB thickness (<1.6 mm)?
My approach:
When do you use it?
Which are the technical limits for assembly thin PCBs (i.e. 0.5mm)? I know that It depends on the size of PCB. Could somebody tell about these limits?
To address the signal issue, closer to the plane is better (there is a critical height where inductance/resistance become equal, and lowering any more makes impedance higher, but it's a complex, lengthy and not well examined subject - see book below for details)
According to Henry Ott (Electromagnetic Compatibility Engineering - a truly excellent book), the main objectives for PCB stack up are:
1. A signal layer should always be adjacent to a plane.
2. Signal layers should be tightly coupled (close) to their adjacent planes.
3. Power and ground planes should be closely coupled together.*
4. High-speed signals should be routed on buried layers located between
planes. The planes can then act as shields and contain the radiation from
the high-speed traces.
5. Multiple-ground planes are very advantageous, because they will lower
the ground (reference plane) impedance of the board and reduce the
common-mode radiation.
6. When critical signals are routed on more than one layer, they should be
confined to two layers adjacent to the same plane. As discussed, this
objective has usually been ignored.
He goes on to say that, as usually all of these objectives cannot be achieved (due to cost of extra layers, etc) the most important two are the first two (note that the advantage of having the signal being closer to the plane outweighs the disadvantage of the lower power/ground coupling, as noted in objective 3) Minimising the trace height above the plane minimises the signal loop size, reducing inductance and also reducing the return current spread on the plane. The diagram below demonstrates the idea:
Assembly issues for thin boards
I'm not an expert on the assembly issues involved with board this thin, so I can only guess at potential issues. I've only ever worked with >0.8mm boards. I had a quick search though, and found a few links that actually seem to contradict the increased solder joint fatigue considered below in my comment. Up to 2x difference in the fatigue life for 0.8mm compared with 1.6mm is mentioned, but this is only for CSPs (Chip Scale Packages) so how this would compare to a through hole component would need investigation. Thinking about it, this makes some sense since if the PCB can flex slightly on movement which generates a force on the component it may relieve stress on the solder joint. Also things like pad size and warpage are discussed:
Link 1 (see section 2.3.4)
Link 2 (part 2 to the above link)
Link 3 (similar info to above two links)
Link 4 (0.4mm PCB assembly discussion)
As mentioned, whatever you discover elsewhere, make sure you talk with your PCB and assembly houses to see what their thoughts are, what they are capable of, and what you can do design wise to make sure the optimum yield is achieved.
If it happens that you can't find any satisfactory data, getting some prototypes made and doing your own stress tests on them would be a good idea (or getting an appropriate place to do it for you). In fact doing this regardless is essential IMO.
One advantage not mentioned so far is that you can do smaller holes in a thinner board. There is a max aspect ratio (the ratio between drill depth and drill diameter) for a mechanical drill (actually also for a laser drill, but that is another story).
So a thinner board can have smaller vias - which will have lower capacitance (all else equal).
And the obvious one : smaller end product! If you're making a digital watch, 1.6mm is huge! MP3 players, wearable electronics, possibly cameras, phones etc similar. At these board sizes, flimsiness is not a problem.
The biggest problem is flimsy-ness. In particular if you are running them through an assembly process, the pick-and-place machine will tend to flex the board when it pushes the components into their place and can cause a "bounce" that can jar previously placed components out of position. The boards might also be more likely to warp over time, but I'm not sure about that.
I'll address your ideas, but out of order:
- Problems with assembly process with heavy components
- Problems with PCB twist
These are definitely an issue. Having just made a design with 1 mm thickness, and dimensions maybe 3" x 6", the board is noticeably more flexible than a 1.6 mm board. I can imagine this leading to issues with damaged parts over time, especially if the board must be physically forced (like into an edge-card connector) in normal use.
My organization also makes much smaller boards (0.5" x 1.5") at 1 mm thickness in production volumes, and there is no problem at these dimensions.
- Better capacitance interplane and better power decoupling.
- Better track-plane coupling.
For these objectives, a multi-layer board is a better solution. With a multilayer board you can reduce the plane separation easily as low as 0.1 mm. For 2-layer boards, I don't think you'll want to go below maybe 0.8 mm, even for very small boards.
- Extra cost. No standard thickness.
I don't see this as a major issue. Board shops stock many different thickness of materials to be able to build multi-layer boards to whatever stackups their customers request. A request for a 2-layer board with a thickness different than 1.6 mm could easily be built from this material --- but do check with your vendor what thicknesses they have on hand, or can get quickly, before you commit to a particular design.
When talking about RF PCBs, the simplest transmission line is the microstrip line. For a given Characteristic impedance Z0, microstrip width decreases as the PCB thickness descreases. Example: if f=1GHz and the dieletric has Er=4.5, in order to make a 50 ohm microstrip would be necessary to the microstrip to have 2,97288mm width on a 1.6mm thick PCB while the same 50 ohms can be achieved with a 1,47403mm width microstip on a 0,8mm PCB (omitted other parameters).
