Silent termination in orthotropic material analysis

Analysis issues
1

Hello,

I am encountering a silent termination issue when running an orthotropic material analysis in CalculiX.

The solver stops without any error message, and no .dat or .frd results are generated.

Details:

  • CalculiX version: 2.20
  • Platform: Windows
  • Model: simple test model
  • Material: orthotropic elastic constants

Observations:

  • Isotropic material works fine
  • When switching to orthotropic definition, the solver terminates silently

I suspect it might be related to:

  • *ELASTIC, TYPE=ENGINEERING CONSTANTS
  • or orientation definition

Could you please advise what might cause this behavior?

Thank you.
Here is the minimal input file:
The only difference between the two cases is the material definition.
iso_case.inp (works)
*HEADING
ISO VS ORTHO COMPARISON - ISO CASE

*NODE
1,0,0,0
2,1,0,0
3,1,1,0
4,0,1,0
5,0,0,1
6,1,0,1
7,1,1,1
8,0,1,1

*ELEMENT, TYPE=C3D8, ELSET=EALL
1,1,2,3,4,5,6,7,8

*SOLID SECTION, ELSET=EALL, MATERIAL=MAT1

*MATERIAL, NAME=MAT1
*ELASTIC
210000., 0.3

*BOUNDARY
1,1,3,0.
4,1,3,0.
5,1,3,0.

*STEP
*STATIC
*CLOAD
7,3,-1000.
*END STEP
ortho_case.inp (fails)
*HEADING
ISO VS ORTHO COMPARISON - ORTHO CASE

*NODE
1,0,0,0
2,1,0,0
3,1,1,0
4,0,1,0
5,0,0,1
6,1,0,1
7,1,1,1
8,0,1,1

*ELEMENT, TYPE=C3D8, ELSET=EALL
1,1,2,3,4,5,6,7,8

*SOLID SECTION, ELSET=EALL, MATERIAL=MAT1

*MATERIAL, NAME=MAT1
*ELASTIC, TYPE=ORTHOTROPIC
210000., 210000., 210000.,
0.3, 0.3, 0.3,
80769., 80769., 80769.

*BOUNDARY
1,1,3,0.
4,1,3,0.
5,1,3,0.

*STEP
*STATIC
*CLOAD
7,3,-1000.
*END STEP

2

If you want to use E, v and G instead of the stiffness matrix terms, you should use TYPE=ENGINEERING CONSTANTS.

With orthotropy, you have to be careful when it comes to what goes to which data line:

*ELASTIC, TYPE=ENGINEERING CONSTANTS
E1, E2, E3, ν12, ν13, ν23, G12, G13
G23
2 Likes
3

@Calc_em already gave a working solution, but to clarify:

The correct type is TYPE=ORTHO and the constants must be specified in two lines, e.g.:

*ELASTIC, TYPE=ORTHO
210000., 210000., 210000., 0.3, 0.3, 0.3, 80769., 80769.,
80769.

Nonetheless CalculiX should be able to deal with this and raise an error. I’ll try to check why this isn’t the case.

Edit: note that the constants under ortho are just for showing the correct format, but would need to be converted to stifness coefficients.

4

But this type uses the stiffness matrix coefficients:

D1111, D1122, D2222, D1133, D2233, D3333, D1212, D1313
D2323

instead of E, v and G. The values used by the OP are typical E, v and G values for steel while the stiffness matrix coefficients are:

image
image471×420 20.2 KB

1 Like
5

Correct, I was just elaborating on why the original input file doesn’t work. Your solution is definitely the one to use in his case.

6

I think that formula might be using a different convention.

I have translate some material properties from ENGINIEERING to ORTHO and my cube doesn’t behave the same way. I’m using TRI as example with the reference values given in the table below.

imagen
imagen1045×770 89.8 KB

*MATERIAL,NAME=ENGINEERING_E
*DENSITY
800
*ELASTIC, TYPE=ENGINEERING CONSTANTS
21477000000.00,13530000000.00,12041000000.00,0.49,0.12,0.15,9126000000.00,3670000000.00,
3670000000.00,294.00

*MATERIAL,NAME=ORTHO_E
*DENSITY
800
*ELASTIC,TYPE=ORTHO
40903746625.48,33987763234.38,25757754185.96,14483592552.92,7228556374.39,14560484005.32,9126000000.00,3670000000.00,
3670000000.00,294.00

*SOLID SECTION,ELSET=MaterialTest_ENGINEERING_E, MATERIAL=ENGINEERING_E
*SOLID SECTION,ELSET=MaterialTest_ORTHO, MATERIAL=ORTHO_E
7

Perhaps there is some difference or even bug in CalculiX. The formulas I pasted are from the Abaqus documentation.

8

Sorry.
I have just noticed my Poisson nu21 was bigger than .5. Wrong convention from my side.

I have now recall having some issue some time ago due to Compliance matrix indexing convention compared to my reference. That’s important when reading material properties. knowing the indexing criteria. It could lead to wrong results or analisys failure like mine.

Calculix uses:

imagen

imagen
imagen1025×745 95.5 KB

Now both cards compare fine.

*MATERIAL,NAME=ENGINEERING_E
*DENSITY
800
*ELASTIC, TYPE=ENGINEERING CONSTANTS
21477000000.00,13530000000.00,12041000000.00,0.49,0.12,0.15,9126000000.00,3670000000.00,
3670000000.00,294.00


*MATERIAL,NAME=ORTHO_E
*DENSITY
800
*ELASTIC,TYPE=ORTHO
25821280046.90,8399497747.13,16465162168.22,2858460302.72,2763069026.27,12537970606.80,9126000000.00,3670000000.00,
3670000000.00,294.00


*SOLID SECTION,ELSET=MaterialTest_ENGINEERING_E, MATERIAL=ENGINEERING_E
*SOLID SECTION,ELSET=MaterialTest_ORTHO, MATERIAL=ORTHO_E
1 Like
9

Dear CalculiX Support Team,

I hope this message finds you well.

Thank you very much for your helpful guidance regarding the definition of orthotropic material properties.

Following your advice, I carefully reviewed and corrected the data ordering for
*ELASTIC, TYPE=ENGINEERING CONSTANTS (E1, E2, E3, ν12, ν13, ν23, G12, G13 / G23), and was able to resolve the input issue.

Subsequently, I performed analyses under identical conditions using the following two approaches:

  • Engineering Constants definition
  • Orthotropic definition with direct Cij input

As a result, I confirmed that both displacement and stress results are consistent, demonstrating the equivalence between the two formulations.

I also noted your comment regarding possible differences in conventions and the reference to Abaqus documentation. In my verification, both approaches produced consistent results within CalculiX, so I believe the definitions are internally consistent in this context.

Your guidance greatly improved my understanding of orthotropic material modeling in CalculiX. I sincerely appreciate your support.

Thank you again for your assistance.

Best regards,
Yasufumi Kanki

2 Likes
10

Dear Calc_em,

Thank you for your explanation and for clarifying the difference between TYPE=ORTHOTROPIC and TYPE=ENGINEERING CONSTANTS.

After reviewing your comments and rechecking my model, I believe the discrepancy I observed is likely due to differences in convention and the transformation process from engineering constants to the stiffness matrix.

In particular, I suspect that:

  • The conversion from engineering constants to the stiffness matrix (Cij) may not have been fully consistent
  • The Poisson ratio relationships (νij vs νji) and indexing conventions may have introduced inconsistencies
  • There may also be slight differences between Abaqus documentation formulas and CalculiX implementation

I will re-derive the stiffness matrix carefully from the compliance matrix and verify the symmetry and consistency of the material properties.

Thank you again for pointing me in the right direction. Your comments were very helpful.

Best regards,
YAKANKI