Pcb Tracks-Paths What Sizes And Thicknesses ?

Hello

Checking around , and of course "googled" too....
about right method to calculate Pcb Tracks-Paths right Sizes And Thicknesses ...
but not helps found  :-[

i know any "conductor" have impedance and absorption...
so I guess the tracks-Paths Sizes And Thicknesses have to be made in the " ideal " size,
to prevent excessive absorption of signal or power ,
and-or tracks that are interrupted because undersized ,

which " good " method of calculating
is required about?

thanks for all helps
peace
R2D2

The only time I have given this serious consideration is for audio power amps where traces can be carrying lots of amps, and in addition to using thicker copper (more expensive raw material), sometimes we would leave off the resist, so solder could build up and lower the resistance even more.

For general audio layouts this is not a big concern. Keep traces fat around power supply parts that will see peak charging currents (like between bottom of reservoir caps and central ground.

JR

Although the calculator returns extremely small width for a mains track carrying 0.2Amp, it's obvious that you must use much larger width, for at least two reasons:
manufacturing: most vendors will charge a premium for tracks smaller than 12 mil
reliability: tracks going to connectors, switches, pots are submitted to additional stress when connectors are engaged/disengaged or knobs manipulated

I use 12 mil for default width
16 mil for rails
24 mils for unregulated voltages (rectifiers, smoothing caps, low-voltage AC connections)
32 mils for mains
70 mil for ground and earth
YMMV

I run similar, but larger runs, based on cheap pcb vendor performance mostly.

This is based on thru hole, stuff sits on a .025" grid, and lots of room, meaning old style audio layouts.

20 mils for interconnects
30 for rails, i.e. decoupling networks
40-60 raw supply distribution, and mains
70 and up for supply returns, grounding.

minimum clearance to anything 0.012"

I like to use as large a pad as possible for component mounting, switching to oval shapes if necessary to
facilitate hand assembly and rework/repair. It helps when the pad has enough annular ring to get an iron tip or
desoldering tool on it.

Today I was doing an industrial control board with 8/8 rules, still 20th century, but a lot more involved than most audio.

thanks to all for post

normally power is
15v + / 15v -  like ssl

24v + like neve

48v + for phantom power

something other require 18v + / 18v -

and also 3,5v + / 3,5v -

or 5v + / 5v - 

for "logic / switching " controls

r2d2

abbey road d enfer said:

Although the calculator returns extremely small width for a mains track carrying 0.2Amp, it's obvious that you must use much larger width, for at least two reasons:
manufacturing: most vendors will charge a premium for tracks smaller than 12 mil
reliability: tracks going to connectors, switches, pots are submitted to additional stress when connectors are engaged/disengaged or knobs manipulated

I use 12 mil for default width
16 mil for rails
24 mils for unregulated voltages (rectifiers, smoothing caps, low-voltage AC connections)
32 mils for mains
70 mil for ground and earth
YMMV

Click to expand...

This is very helpful! I wonder if you wouldn't mind sharing your standards for clearance (spacing between traces) as well. -- I realize this is a voltage-related issue - so a little off-topic, but nonetheless important to consider when laying out a PCB.

Thanks!

16 mil is my default, except for mains at 150 mil. In tube design I also have 100 mil for B+ (<300V) and 50 mil for plate or screen.

Clearance or minimum spacing depends somewhat on process accuracy or resolution. In past lifetimes I've had to live with 20 and 20 mil traces and spaces, due to the limitations of screening traces across large panels. Modern PCB fab can deliver arbitrarily fine detail, if you are willing to pay for it.

If you a buying PCBs, check the vendor price list to determine your design rules, as they will typically charge premium pricing for fine lines and spaces.

JR

Usually it comes down to temperature rise above ambient conditions that the PCB is exposed to in addition (which of course could be considered parasitic resistance at audio frequencies)...

MIL-STD-275 had two charts that relate, copper weight, trace width, current carrying with temperature rise...

Provided that the PCB fabricator can provide a basic set of "design rules" for minimum trace width and spacing, then the charts can be used to determine temperature rise, usually if one is making copper artifacts that are larger than the design rule minimums...

There are probably many web based calculators out there that can give parasitic resistances and probably mimic MIL-STD-275 that are discrete numeric based calculators

but to see the curves in action....
Page 38 (printed as page 34 in the document) has the two charts... Both charts should typically be used in tandem...
http://www.everyspec.com/MIL-STD/MIL-STD+(0100+-+0299)/download.php?spec=MIL-STD-275E.026128.pdf

if you buy the UL book on electronics for helping you get stuff ready for certification, you will see a bunch of specs for traces,

maybe somebody has access to a bootleg copy as the original is about 5,000 smackers?

skip the wagon wheel ground plane traces, use a single trace, much easier to de-solder a single trace link to the ground plane, if it is kept small.

PCb Trace width Calculator:
http://saturnpcb.com/pcb_toolkit.htm
How IPC-2152 supercedes the older specs:
http://pcdandf.com/cms/component/content/article/171-current-issue/7710-current-carrying-capacity

Sorry to bring this post back to life but I didn't want to open a new thread.

I'm working on a PCB with +/- 28V power rails.

Now, since it's double sided and I have the room, I made all traces (both power and audio signal) 40mil.

Can this cause any undesirable effects, especially in the signal path?

FWIW, the PCB will be manufactured (ie. no etching).

Thanks
w.

In general thicker is better for power and ground traces. There may be subtle issues with audio traces if very high impedance  but I wouldn't lose sleep over it. Long high impedance traces should be avoided no matter how wide they are.

JR

I see, I've seen old PCBs where the signal traces are much thicker than today's standards but I guess that was due to different manufacturing requirements.

Once again, thanks for your help 

I recall hearing the owner and design chief of a small power amp company argue that he used narrow traces on his PCB as a form of QC on his PCB house, they had to have a good process to reproduce narrow traces back in the bad old days (I didn't buy his BS but his narrow traces for back then were not narrow by today's standards.  Fat traces are more forgiving of process flaws. These days the process is much better.  FWIW many PCB designs were done by technicians connecting the dots with little or no understanding of what the different traces were carrying, so I've seen entire PCBs using the same width traces for pretty much everything.

JR

Not at all relevant if one is getting boards made by a company, but I've found that for self-etch boards using the basic toner transfer method, traces wider than about 35 mil can cause problems due to uneven electrostatic attraction of the toner.  This causes pitting on thicker traces and ground planes.  I've been using Pulsar GreenTRF to solve this problem.

Again, not a consideration unless you're etching boards yourself.

For one more irrelevant comment. I recall the owner of the compnay actively lobbying for filling all empty spaces on PCB so it would deplete the etchant slower. 

JR

warpie said:

Sorry to bring this post back to life but I didn't want to open a new thread.

I'm working on a PCB with +/- 28V power rails.

Now, since it's double sided and I have the room, I made all traces (both power and audio signal) 40mil.

Can this cause any undesirable effects, especially in the signal path?

FWIW, the PCB will be manufactured (ie. no etching).

Click to expand...

I'm not sure whether you're using ICs or all discretes, but a 40 mil trace is pretty wide and you'll have clearance issues going into a 100-mil pin-pitch IC package. You'll have to neck-down the traces near the packages.

Any reasonable board house these days can do silly skinny traces. You can easily do 10-mil signal traces and maybe 20-mil power traces without any issues.

-a

Hi Andy,

The specific design is all discrete and although I can make the traces thinner I believe that (since I have the room)
wider traces = less resistance (right?). Unless, there's something obvious I'm missing...

It's a line level signal circuit so no high impedances are involved.

Thanks
Miek

The currents involved are small and the resistance of short traces are small.

Only for PS and grounds that you want to be very low impedance might it ever matter.

JR