PCB track size and spacing - diyAudio
Go Back   Home > Forums > Amplifiers > Solid State

Solid State Talk all about solid state amplification.

Please consider donating to help us continue to serve you.

Ads on/off / Custom Title / More PMs / More album space / Advanced printing & mass image saving
Reply
 
Thread Tools Search this Thread
Old 27th April 2013, 09:09 PM   #1
diyAudio Member
 
Dan Moos's Avatar
 
Join Date: Mar 2013
Location: Lynden, WA USA
Default PCB track size and spacing

What is a good default PC track spacing/width for all the small signal portions of a poweramp. I will be using the toner transfer method, and would rather have my boards be a little big if it means getting better results.

Also, I have heard many different answers concerning the use of a ground plane.

What I would like to do is use a ground plane for the low current portions of the amp, a single star for the PS ground nodes, and have the 2 join at a single point just before (maybe even right at?) the chassis ground.

I have also heard that running the main rails close together is good. Can anyone elaborate? I only ask because it seems that it would be easier layout-wise to have them placed in a manner similar to how they are usually place on schematics. Maybe I am having trouble switching gears in my head from schematic layout to good PCB layout.

Thoughts?
  Reply With Quote
Old 28th April 2013, 03:37 AM   #2
diyAudio Member
 
dchisholm's Avatar
 
Join Date: Mar 2011
Location: St Louis, Mo
Check with the Yahoo "Homebrew_PCBs" group at http://tech.groups.yahoo.com/group/Homebrew_PCBs/ . Depending on your printer model and details of your toner-transfer process they may suggest 0.012" to 0.015" as the minimum trace width, and 0.010" or a bit more as minimum trace spacing. With some combinations of equipment and materials, and a little experimentation, I think a home constructor can get down to 0.010" width and spacing or maybe a little tighter.

A common suggestion is to start with a standard trace width of 0.010" (sometimes called "ten mils", or "ten thou") for 1-ounce copper and adjust as necessary. I believe this is supposed to be adequate for carrying currents up to 1 amp in non-critical circuits. They say the same 10 mils should be used as the minimum spacing between any two unconnected copper features: trace-to-trace, trace-to-pads, pads-to-ground-planes, etc. This guideline is often called a "ten-ten design rule" (or "10/10").

For comparison, if I recall correctly, a place where I worked a few incarnations ago had a "house rule" that PWB traces would be 0.008" (8 mils) on one-ounce copper for circuits up to 500 mA, and scaled appropriately for higher currents. I don't recall their standard spacing but it may have been wider than 10 mils since some of their products went to environments that were occasionally challenging. Currently (2013), commercial PWB fab houses can do 8/8 and even 6/6 design rules as a "standard" product, and down to 4/4 or less at extra charge.

This appears to be a straightforward question but the answer actually has some rather complicated considerations. To start with, there are electrical factors, there are fabrication factors, and there are usability factors.

The fabrication factors come from the process of etching the copper pattern on the printed wiring board (PWB). Although you may draw a trace of a particular width in your PWB layout software, the trace that's actually created on a physical PWB may be wider or narrower than your drawing. The etchant resist material (laser toner, photo emulsion, etc) can smear along its edge, and the etching process may undercut (or occasionally stop short of) the resist.

Usability factors are related to human interactions with the PWB. A narrow trace or a thin trace is more easily damaged in normal handling than a wide or thick one. They are also more likely to lift or separate from the epoxy board material during soldering. Small spacings between traces are more likely to have shorts ("solder bridges") between them and are more difficult to to probe with test equipment. Small spacings will also reduce the electrical isolation between different parts of the circuit, especially as the PWB accumulates dust, pollution, and other contaminants as it is in-service. (The solder mask coating should NOT be considered as insulation, and it is not chemically robust.)

To analyze the electrical factors you need to start with the thickness of the conductor, and how much of it is truly copper versus how much is built-up from other plating material. I think that so-called "one-ounce copper equivalent" is the norm for the majority of PWB fabricators. "One-ounce" refers to the thickness you get if you rolled that one ounce of copper into a foil of one square foot. Knowing the thickness, the width of a trace, and the physical properties of copper you can calculate the electrical resistance as so-many ohms per foot (or centimeter, or furlong, or whatever your favorite units are). There are web sites and engineering handbooks with formulas, charts and tables to do this. You may encounter values less than "one ounce equivalent" - especially with bargain-priced, or fast-turnaround vendors. (Not only does the copper itself have a cost, but a thicker foil takes longer to etch and uses more etching chemical.)

Once you know the resistance of a certain trace length you can calculate the voltage drop using Ohm's law. An acceptable voltage drop depends on the application as well as the function of the trace. There will also be a temperature rise of the trace conductor, which is more difficult to calculate, but in high-power circuits may be more important than the voltage drop. (The trace also has inductance but the amount of inductance is relatively independent of trace width and thickness. For PWB's in practical audio projects the trace inductance is probably a few tens of nanohenries at most, and not a significant factor until you get into the VHF frequency range.)

As your question implied, you could keep a small army of engineers (or, a VERY expensive computer program) busy for a lifetime if you had to analyze the effect of every PWB trace in a circuit, considering its manufacturing tolerances, etc. Seeding a search engine with "PCB design guidelines" will uncover dozens of web pages and documents giving suggestion for not only trace width and spacing but also many other factors in PWB layout and design. Believe it or not, the PWB is MUCH MORE than just a convenient place to park and connect your circuit components! One document I've had in my "Bookmarks" for quite a while is "PCB Design Tutorial" at http://alternatezone.com/electronics...torialRevA.pdf .

A common suggestion is to start with a standard trace width of 0.010" (sometimes called "ten mils", or "ten thou") for 1-ounce copper and adjust as necessary. I believe this is supposed to be adequate for carrying currents up to 1 amp in non-critical circuits. They say the same 10 mils should be used as the minimum spacing between any two unconnected copper features: trace-to-trace, trace-to-pads, pads-to-ground-planes, etc. This guideline is often called a "ten-ten design rule" (or "10/10"). Currently (2013), commercial PWB fab houses can do 8/8 and even 6/6 design rules as a "standard" product, and down to 4/4 or less at extra charge.

Dale
  Reply With Quote
Old 28th April 2013, 04:29 AM   #3
diyAudio Member
 
Dan Moos's Avatar
 
Join Date: Mar 2013
Location: Lynden, WA USA
Thanks! Funny you mentioned that .pdf. After I sent my message, I remembered I had downloaded that very tutorial. I read it (Its not to long, but surprisingly informative for its length). It is a pretty good document, and Illuminated a great deal for me.

He mentions the notion of keeping your power rails and ground close together. I was wondering why? Is that so any noise on one rail is canceled out by the noise on the other from an emf standpoint?
  Reply With Quote
Old 28th April 2013, 11:05 AM   #4
AndrewT is offline AndrewT  Scotland
diyAudio Member
 
Join Date: Jul 2004
Location: Scottish Borders
Keep all flow and return pairs very close, to minimise loop area.
This applies to every wire pair and every trace pair. The flow and return currents are in opposite directions and the fields caused by each current tend to cancel in the far distance. They don't cancel well at very close distance and here twisting of the flow and return pair is a big help in reducing the emitted fields.
__________________
regards Andrew T.

Last edited by AndrewT; 28th April 2013 at 11:17 AM.
  Reply With Quote
Old 28th April 2013, 02:43 PM   #5
JMFahey is offline JMFahey  Argentina
diyAudio Member
 
JMFahey's Avatar
 
Join Date: Mar 2009
Location: Buenos Aires - Argentina
FWIW, although you *can* go down to 10 mil traces in toner transfers PCBs, I prefer to use 30/40/50 mils if possible , even more in power/ground/speaker tracks (70/100 mils) and liberally apply fills, specially to ground.
Never use the cheesy automatic copper fill, but hand apply fills where *I* want.
I *might* neck down to 15 mils for a very short length, as in passing between 2 transistor pads, but go up to 30 as soon as I'm through.
Problem with toner is that it's a "barely melted solid", and it does not "flow" to cover pinholes.
Now, a pinhole which does not matter in a 30 or more mils track, may be a thin track killer.
Worst of all is that etching *enlarges* pinholes (imagine a cavity in a tooth, and for the exact same method: acid corrosion), in PCB speak it's called "undercutting" which means exactly that, at edges and holes, acid eats **under** the ink , making holes larger and tracks thinner than intended
Talk about raining on your parade!!
What's nothing on a thick track, becomes a problem in a thin one.
As an example, here's a 2x15W amplifier PCB (single supply) showing that.
It's *easily* printable with toner transfer.

EDIT: I forgot, try to use 100 mil pads for parts, more for larger ones like filter caps, power diodes, etc.
Copper is your friend
Attached Images
File Type: png TDA2030St-BL.png (6.9 KB, 155 views)

Last edited by JMFahey; 28th April 2013 at 02:51 PM.
  Reply With Quote
Old 28th April 2013, 04:34 PM   #6
diyAudio Member
 
Dan Moos's Avatar
 
Join Date: Mar 2013
Location: Lynden, WA USA
@JmFahey:

could you post the schematic that goes with that and maybe an image of the PCB that shows the components layer? That looks way cleaner than my experimentation, and I suspect its a more complicated circuit.
  Reply With Quote
Old 28th April 2013, 07:34 PM   #7
JMFahey is offline JMFahey  Argentina
diyAudio Member
 
JMFahey's Avatar
 
Join Date: Mar 2009
Location: Buenos Aires - Argentina
Ok, if 2x15W is enough for you
The schematic is basically the single ended application shown in the datasheet, I'll print the component overlay.
Give me a couple days, because I still use pre-historic Autotrax and Tango PCB, DOS version , so I have to make some Graphic format conversion.
  Reply With Quote
Old 28th April 2013, 10:05 PM   #8
diyAudio Member
 
Dan Moos's Avatar
 
Join Date: Mar 2013
Location: Lynden, WA USA
Thanks! 15 watts is right in the range of what I', interested in doing these days. I doubt I'd build the amp. I more want to see how proper routing is done with a project simple enough that I can follow it. I could tell from the pic that its 2 channels, but that's about it.

When doing toner transfer, is it difficult to get those labels to etch cleanly? (the in, and what I presume are labels for the power rails)

I was just given a free laser printer, which was the one element I lacked, so I should be in business soon!
  Reply With Quote
Old 29th April 2013, 12:51 AM   #9
JMFahey is offline JMFahey  Argentina
diyAudio Member
 
JMFahey's Avatar
 
Join Date: Mar 2009
Location: Buenos Aires - Argentina
Ok.
The smallest ones, yes, you often get some broken letter , or lose some dot.
Those letters use 10 mil traces, that's why I said that's the practical limit for a kitchen made PCB.
I make production quantities and silkscreen them, but that's not practical with ones and twos.
If you have an important project, photopositive PCBs give you *incredible* detail, although they are somewhat more expensive.
  Reply With Quote

Reply


Hide this!Advertise here!
Thread Tools Search this Thread
Search this Thread:

Advanced Search

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are Off
Refbacks are Off


Similar Threads
Thread Thread Starter Forum Replies Last Post
pcb safety spacing gearheadgene Power Supplies 47 4th December 2013 11:41 AM
PCB track epilot Power Supplies 10 26th November 2011 09:55 AM
PCB track width? per_electric Construction Tips 11 6th November 2009 05:19 PM
PCB track spacing (HV) keyne Parts 3 1st November 2004 05:57 AM


New To Site? Need Help?

All times are GMT. The time now is 04:17 AM.


vBulletin Optimisation provided by vB Optimise (Pro) - vBulletin Mods & Addons Copyright © 2014 DragonByte Technologies Ltd.
Copyright 1999-2014 diyAudio

Content Relevant URLs by vBSEO 3.3.2