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.

Current Density PCB track

Status
Not open for further replies.

Draytek321

Newbie level 5
Joined
Apr 4, 2020
Messages
9
Helped
0
Reputation
0
Reaction score
0
Trophy points
1
Activity points
111
Hello,

Does anyone know what is rule of thumb for maximum current density on PCB tracks (Extracted from a DC Drop Analysis) ? I know for wires is usually 500A/cm2. How do I know if a local hotspot with 2000A/cm2 or 5000A/cm2 is bad or not.

Thanks
 

Thanks d123

Not sure if that answers my question though. When doing a DC Drop analysis, like in hyperlinx PI, I obtain the current density A/cm2 for the whole power plane or via array. I may have a high current density concentrated in a very specific spot, so I would like to know what is the safe value.
 

If you convert the linked current capacity numbers for typical trace widths to current density, you get a first answer.

- - - Updated - - -

Acceptable current density values are set by thermal considerations, hence they depend strongly on the conductor geometry and heat dissipation conditions. At a much higher current density level above 1e6 A/cm², electromigration takes place, but it's hardly reached in PCB.
 

Hi,

... I obtain the current density A/cm2 for the whole power plane or via array. I may have a high current density concentrated in a very specific spot, so I would like to know what is the safe value.

are you sure about that? In my opinion the program should result in the current capability of the "weakest spot". Have you ever tried to create two huge power planes and connect them by a thin trace? I would expect the current capability of the thin trace as a result. Is there no function included resulting in the maximum current only (without geometry)? Such functions are even included in "cheaper" EDA programs.

A program I frequently use for PCB related parameters is Saturn PCB Design Toolkit [1]. Have a try, it is for free.

[1] https://saturnpcb.com/pcb_toolkit/

greets
 
Last edited:

Hyperlynx has a default current density warning level of 10 mA/mil² (about 1700 A/cm²). An 1 oz, 1mm (40 mils) wide trace carrying 2 A, a still acceptable value according to Saturn etc., has already 5700 A/cm². Even higher current densities are usually achieved around high current pins of power connectors or semiconductors.
 

Hyperlynx has a default current density warning level of 10 mA/mil² (about 1700 A/cm²). An 1 oz, 1mm (40 mils) wide trace carrying 2 A, a still acceptable value according to Saturn etc., has already 5700 A/cm². Even higher current densities are usually achieved around high current pins of power connectors or semiconductors.
Something that strikes me is the fact that , according to Saturn, there is an inverse relationship between cross sectional area and current density

These are values obtained for 20C rise

For 1oz, 1mm : 2.52 Ampacity -> 6970A/cm2
For 1oz, 10mm : 9.79Ampacity -> 2720A/cm2
For 1oz, 100mm : 46.9Ampacity -> 1300A/cm2

When the opposite would make more sense to me, i.e. with more area , more surface to radiate the heat away, hence more current per cm2 should be allowed
 

When the opposite would make more sense to me, i.e. with more area , more surface to radiate the heat away, hence more current per cm2 should be allowed.

No. Small trace is dissipating most heat by lateral conduction, thus higher specific rating. Large plane must dissipate all heat vertically. By the way, radiation plays a minor role in heat dissipation at usual PCB temperatures. Mostly surface convection.
 

Hi,

When the opposite would make more sense to me, i.e. with more area , more surface to radiate the heat away, hence more current per cm2 should be allowed

This is correct: more area --> more power to dissipate

But the ratio will be less.

Imagine:
An area of 1cm x 1cm ... let´s imagine it can dissipate 1W...

Now use 9 identical such areas in an 3 x 3 arrangement. Best if you focus on the center area, it is surrounded by 8 areas, that also generate heat.

A single is surrounded by "cold" area, where in the 3x3 arrangement the center one is surrounded by "hot" area.

***
Now you may say: but the "cold" border of the 3x3 arrangement is longer than with the 1cm x 1cm area.
True. But the length of the border increases with the square root of the area, where the power increases linearely with the area.

border length of a 1x1 cm square = 4cm, area = 1 cm^2
border length of a 3x3 cm square = 12cm, area = 9 cm^2. ( border length is not 9x 4cm = 36 cm)

****
As FvM mentioned, you must not only focus on the vertically radiated heat, but also on the horizontally spread heat.

Klaus
 

Hi,



are you sure about that? In my opinion the program should result in the current capability of the "weakest spot". Have you ever tried to create two huge power planes and connect them by a thin trace? I would expect the current capability of the thin trace as a result. Is there no function included resulting in the maximum current only (without geometry)? Such functions are even included in "cheaper" EDA programs.

A program I frequently use for PCB related parameters is Saturn PCB Design Toolkit [1]. Have a try, it is for free.

[1] https://saturnpcb.com/pcb_toolkit/

greets
The saturn PCB toolkit is indeed an awesome program. Far better than any web-based calculators, and it has numerous modeling functions.

For pcb current capacity, make sure you refer to IPC-2152, instead of IPC-2221 (a much older standard which most online calculators refer to). Especially for inner layers. I believe saturn pcb uses IPC-2152 by default.
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top