Instructions for using FEMM program to analyze current
densities of PCB Planes/Traces. Only
useful for a single plane as multiple power planes of the same signals cannot be
analyzed.
Export from PCB Layout
1.
Fill all planes/copper
shapes for PCB.
2.
Select the layer to be exported including Board Outline, 2D Lines, Copper Pours or Planes, Traces.
3. Export to DXF format
Import into FEMM
1.
In FEMM create a new project File->New
2.
Select “Current Flow Problem” in the “Create a
new problem” dialog
3.
Import DXF file using File->Import DXF
a.
Select file that was exported from PADS Layout
b.
Use default “Tolerance for DXF Import”
4.
Wait for
import to complete (complex designs will take longer)
5.
Simplify the imported design
a.
Delete unnecessary point (ones not being
analyzed)
b.
Reduce Arc complexity by selecting arc points,
pressing “Space Bar” and make Max Segments filed to 45 degrees.
c.
Check that polygons are closed (most likely for
planes)
Setup Materials
1.
Setup material for Copper and Air select
Properties->Materials and create new properties
a.
Copper (sigma = 59600000)
b.
Air (sigma = 0)
Setup Conductor Properties
Output Voltage and Input Currents
1.
Setup Conductor Properties of copper, select
Properties->Conductors
2.
Create a property for each signal Source and Sink
points; <SIGNAL NAME>_<{SOURCE,SINK}> (ie: V28_POS_SOURCE)
a.
Source has a Fixed Voltage (nominal)
b. Sink has a Fixed Negative Current (max)
c.
Ground/Return Source has Fixed Zero Voltage
d.
Ground/Return Sink has a fixed Positive Current
(max)
Assign Copper and Air Plane Areas
1.
To assign and area as Copper or Air Material,
select the “Operate on Block Label” button
2. Left click in a copper plane area to set a Block Label with default label <None>.
3.
Right click on this label to select it.
4.
Press
Space Bar to bring up “Properties for selected block” to modify Block type
5.
From the “Block type” drop-down, select “Copper”
and click OK button
6.
Use the PCB Layer in PADS Layout to assign the
Copper Block type to all the areas of Copper, including component pads and all
the copper areas.
7.
Add Block Labels and Assign Block Types to areas
that are not Copper Planes/Traces/Pads, but select “Set as default block label”
check box in the Properties for selected block
Assign Conductors
1.
To assign Conductors to Sources and Sinks,
select the “Operate on nodes” button 
2.
Right click on a Square Box Node in the Drawing
area to select it
3.
Press space Bar to bring up “Specify Nodal
Property” dialog box to assign a Conductor.
4.
From the “In conductor” drop-down, select to
Source or Sink that that point belongs to.
Generally, a pad or through-hole would be as source/sink and all Nodes
(Square Box) need to be assigned
5.
To select multiple points of a pad or trace use
one of these buttons 
to draw a box or circle to select the points
then use Space Bar for “Specify Nodal Property”
6.
Every Conductor Source and Sink needs to
be defined as part of a node for the analysis to be done.
General Setup for Analysis.
1.
Setup parameter for analysis select the Problem
menu and a Problem Definition dialog will open
2.
Set Length Units to Mils
3.
Set Frequency, Hz to 1 (DC analysis)
4.
Set Depth to Layer Thickness (from PADS Layout)
|
½ oz |
0.7 mils |
|
1 oz |
1.4 mils |
|
2 oz |
2.8 mils |
|
3 oz |
4.2 mils |
|
4 oz |
5.6 mils |
5.
Create the analysis mesh select menu
Analysis->Create Mesh after a few minutes (<10mins) a mesh of triangles
will be created and the status will be shown
6.
Verify that Copper Planes are defined in
Yellow. If they are not double check
that Materials and Conductors are properly assigned. Check that the shapes are
closed.
Run and View Analysis
1.
To run the analysis, select menu Analysis->Analyze
2.
A Status dialog will appear and a progress meter
will appear below “BiConjugate Gradient Solver”. After a few minutes (<10mins) it will
complete and close. If it takes too long simplify the design after importing
the DXF, also double check proper settings for “Conductor Properties”
3.
To view the results, select the menu
Analysis->View and a new window tab will open with a color gradient map for
the Plane Areas.
4.
Select menu View->Density to change to the
Current Density dialog.
5.
Set Plotted Value to “RE(J) (A/m^2)”
6.
Set Lower Bound to “0”
7.
Set Upper Bound to “15500000” (approx. double
the recommended current density for copper)
8.
To the Right of the window is the Legend
9.
The recommended Current Density for Copper
(unless otherwise specified by the PCB manufacturer) is 5mA/mil2 or
77500000A/m2. The Planes will
have varying density but should be below 7.750e+006 (Sunny Yellow) in the
legend.
10.
This tool cannot analyze multiple planes at the
same time.
Remedies
These are general guidelines.
1.
Increase the Plane thickness (1/2 oz -> 1oz
copper) and adjust in Problem Definition and re-run Analysis.
2.
Add additional layers, but FEMM cannot analyze
more than one at a time and the current share between planes is not equal. If a plane is double, adjust the Problem
Definition Depths times two.
3.
Remove cutouts and obstacles in the plane
(re-import the new DXF file).
4.
Make a plane wider (re-import the new DXF file).
