online trace calculator is confused me 
, i want to put trace which allows 20 amps , what should i do now?
Which “online trace calculator” are you using?
So you want 20A . . . what is an acceptable temperature rise when 20A is flowing in this track ? what thickness of copper will you have on your PCB ? 1oz or 2oz ?
1 Like
The calculator RaptorUK shows is built into KiCad:
and 20A is a serious amount of current. Those calculators are not very accurate for such currents, and other things such as the connectors, and how they are mounted on the PCB is also important.
1 Like
i used advanced circuit online calculator. and one thing how do i calculate trace length from one component to another component.
thanks for your replay 
, but how you do put 100mm in conductor length. in this place what it be mean conductor length. is it trace length is equal to conductor length ? , i didn’t understand.can you explain this? please.
okay , thanks for your assist 
Hello @THANGADURAI_M
Your questions are about general PCB designs and NOT about using Kicad.
This forum is for questions regarding the use of Kicad.
It’s the length of the track that will carry the 20A, but it’s not really relevant for current carrying capability but more relevant to voltage drop . . .
Try the calculator, have a play, see what changes when you change different parameters . . . it’s how I learned.
Lets break this down and keeping this KiCad centric.
cross-sectional area of a trace influences how much current it can carry, the length influences the voltage drop.
Fundamentally a track is just a resistor and thus also exhibits the same traits in as far as it will warm up and drop some voltage AND at some point fail … To choose the correct track characteristics you need three additional inputs
- What is the copper weight you will be asking your fabricator to build - 0.5oz, 1oz …
- How hot do you want this track to operate at - +5C, +10C…
- How much voltage drop across this track can you accomodate?
Since the current handling capability is associated with the cross sectional area once you know the copper weight of your PCB you know the depth (0.5oz ~ 18um) and thus the only other parameter you can influence is track width.
Under Board setup you can predefine track widths and under Net Classes you can assign certain widths to certain nets (following rules).
So how wide should you use? Well KiCad also includes a calculator. NOTE: this follows the IPC-2221 definition which isn’t accurate and this does need to be updated to IPC-2152 …which is harsher (I have some code to submit 
)
So once the trackwidth is determined for a certain PCB copper thickness and for a certain temperature rise KiCad can be configured for this.
It is then the responsibility of the PCB design to track this from SOURCE to LOAD… the longer the track the higher the voltage drop this “resistor/track” will create which will reduce the voltage seen at the LOAD. You might have 15V at the SOURCE but could end up with 14V at the LOAD (if poorly designed) and if this isn’t acceptable then the voltage drop needs to be reduced and the only things that can be done are
- shorten the track
- widen then track
- increase the copper weight.
The other consideration is the FUSING … Onderdonk’s equation (again in KiCad calculator).
So for 20A and 100mm…
Additional design constrains could be
- Temprise <5C
- Voltage drop < 0.1V
- 18um (0.5oz) copper
The KiCad calculator (IPC-2221) advises:
External: 55mm wide track and 0.068V drop
Internal: 144mm wide track and 0.026V drop
An IPC-2152 calculator advises:
Calc: 180mm wide track and 0.02V drop
3 Likes
OK, let’s look at this from another angle: is this PCB designed for a long production run, or are we talking about a handful of hand-made units? If you are talking hand-made units, then you might want to consider “beefing up” the track with some thick wire, soldered in place (best: solder the wire pad to pad, next best, put suitable PCB holes right next to the pads).
I remember back in the day of boards full of 5 volt TTL logic chips, you could buy ‘busbars’, metal strips with pins, that you soldered to the PCB, to give low-resistance distribution of the power (and even 0v)
If you are looking at this for production, then yes, you need to make sure you have enough copper.
1 Like
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.