Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Register Log in

How to determine the PCB track width

Status
Not open for further replies.
A

Antenna (^.^)

Member level 3
Member level 3
Joined
Jul 6, 2015
Messages
54
Helped
0
Reputation
0
Reaction score
0
Trophy points
6
Activity points
499
How do I determine the track width of a pcb?
Also, what factors should I consider when making this decision?
 

pcb track width is based on current flowing through the track.
 
What you need it the Saturn PCB Toolkit to calculate your track widths, it has one of the most upto date calculators for this and most I know use it.
You need to consider the board material, track width, thickness, current, ambient temp of board in enclosure, max temp, height ASL, internal or external tracks etc.

Fill the calculator out & work out your track widths.

P.S. you provide the board manufacturer with tracks at the finished width you want - they will adjust for etch compensation etc.
 

Firstly determine what the track is used for, is it a signal,
is it a digital signal, does it require a controlled impedance.
Is it an analogue signal, current, voltage drop etc.
Is it a power signal, as above current capacity.
As you are likely to use all of these on a board your question is a bit ambiguous; ambiguous and PCB don't mix that's when things go wrong, learn to be precise.
 

How much should be my width of the track for my relay, which carries 230VAC. I use T80. Is it enough? Also how do i measure the impedance of my track?
 

Hi,

Is it a power signal, as above current capacity.
Click to expand...

230V is no current.
--> (power) Track width depends on current, not on voltage.

Klaus
 

For power devices, in general I do not use the available track width calculators, due this often yields a prohibitive result, and instead of this I just remove the solder mask to increase its capacity to deal with higher currents than the nominal for the varnished copper.
 

@andre. Are you trying to say that when you measure the temperature rise for a PCB track of given paramterers, the temperature rise given by the calculation is "prohibitive"? really? Isn't a 30 mil track sufficient? I know there are websites on which one can enter the parameters of a PCB track and the website shall calculate the temperature rise of a given amount of current through the track.

- - - Updated - - -

@senilicus, why should the impedance of the track carrying power supply signals matter? Only resistance should matter isn't it? isn't it so?
impedance matters for tracks that carry high speed signals which means signals which have a rise/fall time much shorter than the propgation delay of the signal on the track.
 

matrixofdynamism said:
@andre. Are you trying to say that when you measure the temperature rise for a PCB track of given paramterers, the temperature rise given by the calculation is "prohibitive"? really? Isn't a 30 mil track sufficient? I know there are websites on which one can enter the parameters of a PCB track and the website shall calculate the temperature rise of a given amount of current through the track
Click to expand...

Exactly, for instance a Triac carrying 20A RMS current at a PCB of 2Oz thickness, even alleviating others parameters (e.g DT=40oC / Lengh=1 inch), will result in a width larger than spacing of the pins of the component itself: ~400mils. Calculations performed here.

Obviously it is not the case of the load above mentioned, but OP gave the current consumption just after my reply. Anyway, I think that the fields on the width calculator somehow answer the original question that is, ''what are the factors considered in defining track width".
:thumbsup:
 

Hi,

a 30 mil trace makes 17mohm per inch.
with 3A it makes 150mW per inch.

It will not burn, but you will feel the temperature rise.

Klaus
 

I would suggest you ditch calcualtors based on IPC-2221 and use calculators based on IPC-2152, the 2152 spec and the background to it is an interesting read.
Where power is concerned I like to use copper pours where possible, more copper more heat dissipation... started doing this after got some boards rejected by UL for traces over-heating in their view.
 

marce said:
Where power is concerned I like to use copper pours where possible, more copper more heat dissipation...
Click to expand...

In addition, another suited measure when there is no much space available to route at the same surface is to split the track among 2 opposite layers Top/Bottom, increasing the dissipation ability.
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top