Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronic 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

Current Density PCB track

Draytek321

Newbie
Joined
Apr 4, 2020
Messages
5
Helped
0
Reputation
0
Reaction score
0
Trophy points
1
Activity points
51
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
 

Draytek321

Newbie
Joined
Apr 4, 2020
Messages
5
Helped
0
Reputation
0
Reaction score
0
Trophy points
1
Activity points
51
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.
 

FvM

Super Moderator
Staff member
Joined
Jan 22, 2008
Messages
46,784
Helped
13,890
Reputation
28,028
Reaction score
12,523
Trophy points
1,393
Location
Bochum, Germany
Activity points
273,015
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.
 

stenzer

Full Member level 4
Joined
Oct 1, 2012
Messages
204
Helped
23
Reputation
46
Reaction score
22
Trophy points
1,298
Activity points
3,107
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] http://saturnpcb.com/pcb_toolkit/

greets
 
Last edited:

FvM

Super Moderator
Staff member
Joined
Jan 22, 2008
Messages
46,784
Helped
13,890
Reputation
28,028
Reaction score
12,523
Trophy points
1,393
Location
Bochum, Germany
Activity points
273,015
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.
 

Draytek321

Newbie
Joined
Apr 4, 2020
Messages
5
Helped
0
Reputation
0
Reaction score
0
Trophy points
1
Activity points
51
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
 

FvM

Super Moderator
Staff member
Joined
Jan 22, 2008
Messages
46,784
Helped
13,890
Reputation
28,028
Reaction score
12,523
Trophy points
1,393
Location
Bochum, Germany
Activity points
273,015
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.
 

KlausST

Super Moderator
Staff member
Joined
Apr 17, 2014
Messages
17,294
Helped
3,916
Reputation
7,830
Reaction score
3,779
Trophy points
113
Activity points
114,803
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
 

mtwieg

Advanced Member level 5
Joined
Jan 20, 2011
Messages
3,434
Helped
1,224
Reputation
2,454
Reaction score
1,197
Trophy points
1,393
Activity points
25,706
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] http://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.
 

Toggle Sidebar

Part and Inventory Search


Welcome to EDABoard.com

Sponsor

Sponsor

Design Fast


×
Top