# What are the advantages and disadvantages of thinner PCB thickness (<1.6 mm or 0.063'')?

What are the advantages and disadvantages of thinner PCB thickness (<1.6 mm)?

My approach:

• Better capacitance interplane and better power decoupling.
• Better track-plane coupling.
• Problems with assembly process with heavy components
• Problems with PCB twist
• Extra cost. No standard thickness.

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?

• Also I'd wonder how the increased capacitance affects high-speed signals. – Phil Frost Jan 30 '13 at 16:33
• @PhilFrost - I was answering your question but it got deleted, so I added it here instead, since it's relevant to both. You would find the book mentioned a great read, it's the only book I know that goes into such detail on issues like this. – Oli Glaser Jan 30 '13 at 16:54
• @OliGlaser yeah, I was convinced it was better to not split the discussion. Thanks for the answer, good information. – Phil Frost Jan 30 '13 at 16:55
• The first two points are related to dielectric/prepreg thickness - not PCB thickness. Example: In a 24 layer board even with 0.1mm layer-to-layer thickness the board will be 2.5mm total or more. – Rolf Ostergaard Jun 5 '13 at 12:10
• @RolfOstergaard I suppose that prepeg thickness increase when PCB increase if the number of layer doesn't change. – Jesus Castane Jun 5 '13 at 13:07

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
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 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.

• According these issues about signal integrity it seems that always a thinner PCB is better, but what's happened with manufacturing/assembling issues? Would I be able to assembly a THT capacitor in a 0.5mm thickness PCB? – Jesus Castane Jan 30 '13 at 18:19
• @JesúsCastañé - I'm sorry I only focused on the one issue (see comments above, it was started as an answer to the related but now deleted question) As far as the assembly of through hole capacitors on a board with a total thickness of e.g. 0.5mm, I am not an expert - I'm pretty sure it's possible for less than certain size, but you would have to discuss details with your assembly house. I have never had this particular issue - I have used the bottom stackup as shown above, but the total thickness being the same makes assembly the same as normal. – Oli Glaser Jan 30 '13 at 18:27
• I think that as well as assembly issues, the board being less rigid as mentioned by @vicatcu would be the biggest potential issue (e.g. weight of components flex board on movement and solder joints work loose over time) – Oli Glaser Jan 30 '13 at 18:30
• Thanks for your reply. It's obviuos that a thinner PCB is less rigid but I'm looking for any rule of thumb about that. Any guideline for work with these thickness? – Jesus Castane Jan 31 '13 at 8:03
• I added a small section on the issues for thinner boards based on a brief search. Sorry I can't give any personal experience in this area. – Oli Glaser Jan 31 '13 at 9:54

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).

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.

• Also I bet there are regulatory requirements for the board to be a minimum thickness for circuits that carry mains power. – Phil Frost Jan 30 '13 at 16:30
• @PhilFrost, remember that breakdown voltage through air is lower than through typical dielectric materials, so the minimum thickness for carrying mains won't be nearly as high as the minimum copper spacing (which I don't recall off the top of my head) that we run into more often. That said, there should be some limit. – The Photon Jan 30 '13 at 17:18
• @vicatcu I would like to know about the technical limits in this way. Is a 0.5mm thickness PCB really troublemaker for assembly? How large could it be? – Jesus Castane Jan 31 '13 at 7:48

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.

• You have to also think about weight, although this isn't a big problem in most applications. Why do they make different thicknesses of plastic? So you can make something more sturdy, cheaper, smaller, lighter, etc. – Anonymous Penguin Jan 30 '13 at 21:44
• Weight would be a problem in a toy helicopter though! – Brian Drummond Jan 31 '13 at 4:31

• 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.

• Could give us any rule of thumb for the assembly process of thinners PCBs? What is the biggest component that I can assembly in a 1mm PCB? – Jesus Castane Jan 31 '13 at 8:08
• The biggest component doesn't just depend on the thickness of the board. It also depends how the board is supported and what other heavy components are on the board. If there's just one heavy component, you could simply use that component to support the board --- if there's no other forces acting on the board, then there's no problem as long as the board is at least thick enough to support its own weight. – The Photon Jan 31 '13 at 16:54
• If you want to experiment, you can just buy a sheet of "G10" (basically the same as FR4) fiberglass at whatever thickness you want and glue your components on to see how much they stress the board. I see G10 available online in thicknesses down to 0.005". You can buy one big sheet of thin material and laminate up different thicknesses to see how thick you need for your situation. – The Photon Jan 31 '13 at 16:59

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).