PCB board thickness

[alank2]

Hi Everyone,

I noticed that itead gives a ton of options on pcb thickness.  0.4/0.6/0.8/1.0/1.2/1.6/2.0mm.  What is the benefit to all of these?  Why would they (the pcb manufacturer) want to stock and deal with all of the different sizes?

Thanks,

Alan

[Ribster]

Most commonly is the 1.6mm one. If you want to use your board as USB stick, you can use the 2.0mm thickness.
That way the pads of your pcb are the connections for USB.

[Sebastian]

If you are using a 2 layer board and you need transmission lines you probably have to use a thinner board to be able to achieve the characteristic impedance without unreasonably wide traces.

[mazurov]

Also, thinner boards conduct heat better - could be useful for integrated power supplies and other heat-producing circuits.

[tszaboo]

Such that Dave can make front panel from PCB. There are dozens of reasons to choose something other than 1.6mm. The 2mm one nicely fits into the 2mm standard slot hole. There are different PCB edge connectors. The 0.4mm is lighter than the others. Layers are closer to each other, so if you need a controlled impedance, than you don't need stupid wide traces.

[alank2]

Does the strength of a pcb come into play?  I have to wonder if a 0.4mm thick pcb is more prone to cracking, being weak, etc.

[mikeselectricstuff]

Normal : 1.6mm
Need more rigidity (e.g. for heavy parts) : 2.4 , 3.2 or 4.8mm
Need smaller size or  some flexibility : typically 0.8,0.6 or 0.4mm.
Other thicknesses are also available but less common

[DanielS]

Another reason for having multiple PCB thicknesses available is for composing multi-layer boards: PCB manufacturers already have 0.4/0.6/0.8mm boards in stock because you need two of those and an extra prepreg core in-between to make a four-layer board. Ex.: a 1.6mm four-layer board may have a pair of 0.4mm boards and a 0.6mm core or possibly a pair of 0.6mm boards with a 0.4mm core.

[German_EE]

2mm is nice for front panels.

1,6mm is the standard thickness.

Thinner than 1,6mm is handy if you are building something that has to be thin such as a PCMCIA card or a mobile phone.

[Neilm]

3.2mm thickness is often used if you are expecting high g shocks or vibrations. Quite often military stuff will be that sort of thickness. I saw a 1.2mm board going though a vibration trial - it bowed so much it snapped in half

[Precipice]

If you're solving vibration issues that bad by stiffening up the PCB, odds on you're doing it wrong...

Aside: You can put quite a bend into a 0.4mm PCB if you need a curve, and don't do it repeatedly (and take great care to avoid popping large components off the board). Gluing stiffeners where the chips are, and allowing flex elsewhere, is cheap and sometimes useful. Rather cheaper and less annoying than proper flex-PCBs, too.

[SirNick]

Thick PCBs are also used as daughter cards.  Take an enterprise router for example.  There will be a vertical backplane board made of thick PCB to provide rigidity during insertion and removal, and the modules will be thick to withstand the insertion force applied to the connector on the end.

[DanielS]

Thick PCBs are also used as daughter cards.  Take an enterprise router for example.  There will be a vertical backplane board made of thick PCB to provide rigidity during insertion and removal, and the modules will be thick to withstand the insertion force applied to the connector on the end.

The multiple ground and signal planes necessary for all those custom BGAs, FPGAs, high-speed IOs, etc. plays a significant role in the thickness too: it is not uncommon for those boards to have 10+ layers. In some cases, they have to add layers simply because surface-mount capacitors and their connecting traces/vias are too inductive to get the job done on their own.

[zapta]

I designed recently a few breakout boards (sub square inch) and with 1.6mm thickness they look overkill and disproportional. Next time I will order with thinner material.