Simulation of Planar Magnetic membranes; tweeter and midrange

[FEAnalyst]

@solhaga

My guess is that Shell_part-2 is the correct one.

Yes, the first one was created using your approach to visualize the duplicated thickness. The second one comes from midsurface extraction approach. Thickness is then defined as shell section property.

[solhaga]

@FEAnalyst

Thickness is then defined as shell section property.

So this should give the correct Z-positions then:

Section	Face-Z	Offset

PEN	0	+0.5

Aluminium	12 µm	+0.5

Varnish	0	−0.5

I can then just let Varnish have different thicknesses.

[FEAnalyst]

So Face-Z is the Z coordinate of a surface ? If you use proper offsets (depending on the element normals) then you can indeed have overlapping parts. Use the Check Model run to see if you defined all sections and their offsets correctly.

[solhaga]

PEN and Varnish are both at Z=0 but with different offsets.

PEN is 12µm thick, so the aluminum starts at 12µm with an offset of 0.5.

Here’s the result of Check Model:

05/26/2026 12:00:23

######## Starting run step number: 1 Increment number: 1 ########

Running command: C:\PrePoMax v2.5.1 dev\Solver\ccx_dynamic.exe Analysis-1

---

CalculiX Version 2.22, Copyright(C) 1998-2024 Guido Dhondt
CalculiX comes with ABSOLUTELY NO WARRANTY. This is free
software, and you are welcome to redistribute it under
certain conditions, see gpl.htm

---

You are using an executable made on Sun Aug 4 19:44:24 2024

The numbers below are estimated upper bounds

number of:

nodes: 6224187
elements: 92944
one-dimensional elements: 0
two-dimensional elements: 92944
integration points per element: 27
degrees of freedom per node: 3
layers per element: 1

distributed facial loads: 0
distributed volumetric loads: 0
concentrated loads: 0
single point constraints: 6691968
multiple point constraints: 11153281
terms in all multiple point constraints: 71380993
tie constraints: 0
dependent nodes tied by cyclic constraints: 0
dependent nodes in pre-tension constraints: 0

sets: 10
terms in all sets: 240016

materials: 3
constants per material and temperature: 2
temperature points per material: 1
plastic data points per material: 1

orientations: 92944
amplitudes: 0
data points in all amplitudes: 0
print requests: 0
transformations: 0
property cards: 0

*ERROR reading *PLASTIC: *PLASTIC should be preceded
by an *ELASTIC,TYPE=ISO card or
by an *ELASTIC,TYPE=ORTHO card

STEP 1

*WARNING reading *STATIC: a nonlinear analysis is requested
but no time increment nor step is specified
the defaults (1,1) are used

*WARNING: no analysis option was chosen
*ERROR in calinput: at least one fatal
error message while reading the
input deck: CalculiX stops.

Process elapsed time: 5.227 s

Where do I set the ELASTIC TYPE?

[solhaga]

I simply removed the Plastic properties for the materials:

05/26/2026 13:51:26

######## Starting run step number: 1 Increment number: 1 ########

Running command: C:\PrePoMax v2.5.1 dev\Solver\ccx_dynamic.exe Analysis-1

---

CalculiX Version 2.22, Copyright(C) 1998-2024 Guido Dhondt
CalculiX comes with ABSOLUTELY NO WARRANTY. This is free
software, and you are welcome to redistribute it under
certain conditions, see gpl.htm

---

You are using an executable made on Sun Aug 4 19:44:24 2024

The numbers below are estimated upper bounds

number of:

nodes: 6224187
elements: 92944
one-dimensional elements: 0
two-dimensional elements: 92944
integration points per element: 27
degrees of freedom per node: 3
layers per element: 1

distributed facial loads: 0
distributed volumetric loads: 0
concentrated loads: 0
single point constraints: 6691968
multiple point constraints: 11153281
terms in all multiple point constraints: 71380993
tie constraints: 0
dependent nodes tied by cyclic constraints: 0
dependent nodes in pre-tension constraints: 0

sets: 10
terms in all sets: 240016

materials: 3
constants per material and temperature: 2
temperature points per material: 1
plastic data points per material: 0

orientations: 92944
amplitudes: 0
data points in all amplitudes: 0
print requests: 0
transformations: 0
property cards: 0

STEP 1

*WARNING: no analysis option was chosen
*WARNING in calinput: no elastic constants
were assigned to material VARNISH
in a (thermo)mechanical calculation

No analysis was selected

Decascading the MPC’s

Determining the structure of the matrix:
Using up to 1 cpu(s) for setting up the structure of the matrix.
number of equations
1928877
number of nonzero lower triangular matrix elements
113591868

Using up to 1 cpu(s) for the stress calculation.

Using up to 1 cpu(s) for the symmetric stiffness/mass contributions.

Process elapsed time: 38.058 s

[FEAnalyst]

@solhaga

Where do I set the ELASTIC TYPE?

In the material definition as one of the behaviors (in addition to plasticity here).

The Check Model procedure not only allows you to verify model warnings/errors, but also visualize shell thicknesses and offsets (if OUTPUT=3D) to see if they are defined correctly.

[solhaga]

@FEAnalyst

In the material definition as one of the behaviors (in addition to plasticity here).

I can’t see any behavioral settings in the material definition:

@FEAnalyst

The Check Model procedure not only allows you to verify model warnings/errors, but also visualize shell thicknesses and offsets (if OUTPUT=3D) to see if they are defined correctly.

So where do I set OUTPUT=3D?

[FEAnalyst]

@solhaga

I can’t see any behavioral settings in the material definition:

I sometimes use Abaqus nomenclature:

But you already have Elastic for the 1060_Alloy material there, so you should just add it (from the Material Models list) to other materials if they don’t have it. All materials need it unless you use hyperelasticity via custom keywords.

@solhaga

So where do I set OUTPUT=3D?

It’s enabled by default, but can be changed here if needed:

[solhaga]

@FEAnalyst

But you already have Elastic for the 1060_Alloy material there, so you should just add it (from the Material Models list) to other materials if they don’t have it. All materials need it unless you use hyperelasticity via custom keywords

Got it! I probably had Plastic before Elastic in one of the materials.

@FEAnalyst

It’s enabled by default, but can be changed here if needed:

Got it!

So the check model is green now.

But I can’t see anything about the geometry in the analysis:

05/26/2026 17:43:43

######## Starting run step number: 1 Increment number: 1 ########

Running command: C:\PrePoMax v2.5.1 dev\Solver\ccx_dynamic.exe Tweeter

---

CalculiX Version 2.22, Copyright(C) 1998-2024 Guido Dhondt
CalculiX comes with ABSOLUTELY NO WARRANTY. This is free
software, and you are welcome to redistribute it under
certain conditions, see gpl.htm

---

You are using an executable made on Sun Aug 4 19:44:24 2024

The numbers below are estimated upper bounds

number of:

nodes: 6224187
elements: 92944
one-dimensional elements: 0
two-dimensional elements: 92944
integration points per element: 27
degrees of freedom per node: 3
layers per element: 1

distributed facial loads: 0
distributed volumetric loads: 0
concentrated loads: 0
single point constraints: 6691968
multiple point constraints: 11153281
terms in all multiple point constraints: 71380993
tie constraints: 0
dependent nodes tied by cyclic constraints: 0
dependent nodes in pre-tension constraints: 0

sets: 10
terms in all sets: 240016

materials: 3
constants per material and temperature: 2
temperature points per material: 1
plastic data points per material: 1

orientations: 92944
amplitudes: 1
data points in all amplitudes: 1
print requests: 0
transformations: 0
property cards: 0

STEP 1

*WARNING: no analysis option was chosen
No analysis was selected

Process elapsed time: 15.76 s

This is the current state:

And the back:

[FEAnalyst]

@solhaga

But I can’t see anything about the geometry in the analysis:

When Check Model is done, right-click on the name of the completed (green checkmark) analysis and select Results. Or select this option from the Monitor window if it’s still open after submitting the Check Model procedure. This will take you to the Results tab. You won’t see any contour maps for this kind of run, but you will get the expanded (solid) mesh.

[solhaga]

If I select Monitor I only get the results above.

If I select Results I get:

[FEAnalyst]

After running Check Model ? Try with a new analysis object:

[solhaga]

Same results. But perhaps the analysis must be set up differently?

[FEAnalyst]

Check if there’s .frd file with the same name as the Check Model analysis name (Analysis-1 or Analysis-2 here) in the Work directory (C:\PrePoMax v2.5.1 dev\Temp). If it’s not there or you can’t open it manually from there (using File → Open), please share the .pmx file.

[solhaga]

I get:

But if I open it in Notepad++, I get:

All files are not empty:

[solhaga]

Here’s the Tweeter.pmx file.

Tweeter.pmx (9.0 MB)

[FEAnalyst]

Indeed, it keeps failing. But it worked when I removed all material models other than density and elasticity. Btw. plasticity should start from yield strength vs 0 plastic strain.

It shows some overlap with the strips:

So use a larger offset in the proper direction and/or translate the surfaces with Model → Part → Transform → Translate.

[solhaga]

Thanks, I will check that tomorrow.

[solhaga]

So I finally got it right; for some reason the offsets should be inverted:

So that was the easy part.
Now it is time to get into the actual simulation.

To make it more obvious, I will have several model files with different setups of sections.

First up is to simulate PEN eigenmodes. That requires the PEN membrane rim to be fixed and a pre-tension applied to the PEN membrane.

[FEAnalyst]

@solhaga

for some reason the offsets should be inverted

This is based on the face normals, but might be difficult to understand because it’s not so intuitive - it’s actually understood as offsetting the reference (meshed) surface from the midsurface (of the expanded shell mesh). This example and description may help: https://wiki.freecad.org/FEM_ElementGeometry2D#Properties