PCB Thickness

[fsleeman]

Is there any advantage or disadvantage in using 1/16" or 1/32" double sided PCBs? If the board will not be under a lot of mechanical stress is the 1/32" board just as good (assuming the same copper thickness).

[Simon]

It should be but it is all about the mechanics of the design, if the board is not stressed it should not be a problem electrically

[redek]

Here is a link to a pdf discussing pcb thickness.  The larger pcb was developed for many layers.  But since you only want a double sided pcb you should be fine with a 1/16"
http://www.speedingedge.com/PDF-Files/Is%20063%20a%20standard%20PCB%20thickness.pdf

[fsleeman]

I actually found that today and its glad that somebody else can vouch for it.

What about the thickness? When does the differences between 1/2 oz. and 1 oz. matter?

[tecman]

I actually found that today and its glad that somebody else can vouch for it.

What about the thickness? When does the differences between 1/2 oz. and 1 oz. matter?

Thickness is important for mechanical strength (size of board, heavy components, etc) and voltage standoff.  High voltages may require greater thickness.

The copper weight rating, 1/2 or 1 or 2 oz primarily determine the current carrying capacity of a given run width.  Also in HF the inductance of the run can be a factor as well.  Also thicker copper stands up better to abuse (soldering heat, etc) and is a better heat dissipater.

paul

[migsantiago]

The copper weight rating, 1/2 or 1 or 2 oz primarily determine the current carrying capacity of a given run width.  Also in HF the inductance of the run can be a factor as well.  Also thicker copper stands up better to abuse (soldering heat, etc) and is a better heat dissipater.

paul

I have a PC motherboard which features a 2oz copper thickness. It's offered as a better board because of its good heat dissipation and ultra durable capacitors.

http://www.gigabyte.us/Products/Motherboard/Products_Overview.aspx?ProductID=3150

[EEVblog]

There are many variables such as rigidity, vibration modes, electrical strength, pre-trimmed PTH component lead lengths etc that may need to be taken into account.
But generally speaking, no, the thickness makes no inherent difference. It's the same material and copper, just thinner.

Dave.

[alm]

It will also change parasitic capacitance between layers (and via inductance), so if you're doing high-frequency stuff (eg. controlled impedance traces), you may have to adjust your design. You may also depend on parasitic capacitance without knowing it, but probably not for low-frequency stuff with plenty of margins.

[EEVblog]

It will also change parasitic capacitance between layers (and via inductance), so if you're doing high-frequency stuff (eg. controlled impedance traces), you may have to adjust your design. You may also depend on parasitic capacitance without knowing it, but probably not for low-frequency stuff with plenty of margins.

Yes, that's always a given. Controlled impedance and parasitic plane capacitance are directly calculated from the dielectric thickness and other parameters.

But I figure if anyone is asking the question of whether or not the PCB thickness matters, then they almost certainly aren't involved in controlled impedance or anything else that matters much!

Dave.

[Simon]

is the original poser asking about board or track thickness ? as other has said essentially use 2oz board for stuff that carries large currents or needs extra mechanical strength

[alm]

Yes, that's always a given. Controlled impedance and parasitic plane capacitance are directly calculated from the dielectric thickness and other parameters.

I figured it should me mentioned for completeness sake since this thread did talk about the relation between extra copper and inductance, and suggested that the only electrical difference was isolation rating. If not for this poster, than for future readers.

But I figure if anyone is asking the question of whether or not the PCB thickness matters, then they almost certainly aren't involved in controlled impedance or anything else that matters much!

Agreed, at least not intentionally . I believe Bob Pease told a story about a Philbrick operational amplifier (when op-amp meant a potted module with some tubes), all attempts at cloning the circuit failed, and nobody at Philbrick really knew why it worked, until somebody analyzed it, and figured out that parasitics were what made this circuit work. Using a thicker substrate (less capacitance), however, is more likely to cause trouble than a thinner substrate.

[EEVblog]

is the original poser asking about board or track thickness ? as other has said essentially use 2oz board for stuff that carries large currents or needs extra mechanical strength

Board thickness obviously, as 1.6mm and 0.8mm were mentioned, and they are the two standard board thicknesses.
It's quite surprising how flexible 0.8mm board is in larger sizes, and 0.5mm is really quite flexible!
I've actually done (potted) flex boards using standard thin 0.8mm and lower FR4.
On the other end of the scale, a 4mm board is like a brick!
Actually, you start getting thermal problems on very thick boards like that, and the board loader really has to get their process right.

Dave.

[jahonen]

Thinner PCB might be actually more favorable from signal integrity and EMC perspective, if one must work with two layers only.

That makes it possible to make thinner traces over ground plane (microstrips) to get decent impedance. Also, stray fields from traces come down as the distance between ground plane under the trace and trace itself becomes smaller. As a rule of thumb, trace width equal to dielectric thickness corresponds about 75 ohms microstrip trace and twice the trace thickness to the dielectric thickness is about 50 ohms. From that, it is easy to see that it is quite difficult to achieve reasonable impedance on 1.6 mm boards (or, 0.8 mm for that matter). You just can't fit the traces in, unless you are working with RF, where signal count is usually low.

For typical 4-layer buildup, the dielectric thickness between ground plane and signal (layers 1-2 or 3-4) is in the order of 0.2 mm, and it is easy to do those 75 ohm traces. 50 ohm ones are still quite thick.

In some cases, it might be necessary to make thicker PCB's just because your impedance would drop too low for reasonable trace widths in inner layers (striplines) otherwise. This becomes an issue when you have something like 16 layers (of which about half are power and ground planes).

Regards,
Janne

[mikeselectricstuff]

One practical difference is you can cut 0.8mm with a good pair of scissors.
Re. copper weight, apart from higher current handling at thicker weights, you can get finer linewidths at thinner weights, but you have to get down to pretty small dimensions for this to be an issue.