*DEFORMATION PLASTICITY depends on *ORIENTATION

Analysis issues
1

With *DEFORMATION PLASTICITY, stiffness depends on the orientation of the element coordinate system but I think it’s an isotropic material that should be independent of orientation.

In this example, I expect Y-displacement to be equal on both elements (eg. at nodes 1 and 9) but it’s about 20% different. At lower loads, the difference vanishes and at higher loads it fails to converge, so maybe that’s related.

CCX version 2.23

image
image410×576 4.54 KB

** Generated by Mecway 33
*NODE
1,0.001,0.001,0
2,0.001,0.001,0.0002
3,0,0,0.0002
4,0,0,0
5,0.001,0,0.0002
6,0.001,0,0
7,0,0.001,0
8,0,0.001,0.0002
9,0.003,0.001,0
10,0.003,0.001,0.0002
11,0.002,0,0.0002
12,0.002,0,0
13,0.003,0,0.0002
14,0.003,0,0
15,0.002,0.001,0
16,0.002,0.001,0.0002
*ELEMENT,TYPE=C3D8I
1,4,6,1,7,3,5,2,8
2,12,14,9,15,11,13,10,16
*ELSET,ELSET=1
1
*ELSET,ELSET=2
2
*SURFACE,NAME=PRESSURE_FACES
2,S5
1,S5
*ORIENTATION,NAME=O3
0,1,0,-1,0,0
*MATERIAL,NAME=MATERIAL
*DEFORMATION PLASTICITY
200000000000,0,150000000,3.4,1.2
*SOLID SECTION,ELSET=1,MATERIAL=MATERIAL
*SOLID SECTION,ELSET=2,MATERIAL=MATERIAL,ORIENTATION=O3
*BOUNDARY
3,2,,0
4,1,,0
4,2,,0
4,3,,0
5,2,,0
6,2,,0
6,3,,0
11,2,,0
12,1,,0
12,2,,0
12,3,,0
13,2,,0
14,2,,0
14,3,,0
*STEP,NLGEOM=YES,INC=100
*STATIC
1,1,1E-06,0
*DSLOAD
PRESSURE_FACES,P,-400000000
*NODE FILE,GLOBAL=YES
U
*END STEP
2

trying replicate the problems using MFront material library but the solver stopped and thrown some error messages instead of continuing.

RAMBERGOSGOODNONLINEARELASTICITY:no orientation shall be defined for an istropic behaviour

2026-04-02 01_02_52-or1mod.inp - SciTE
2026-04-02 01_02_52-or1mod.inp - SciTE1351×733 50.2 KB

3

I don’t understand the context of MFRONT but is your finding consistent with the author of that library knowing about this problem and making it a fatal error to prevent incorrect behavior?

4

right, an error message shown orientation not allowed to be used for this type of material.

5

According to the CalculiX manual, inhomogeneous boundary conditions are only allowed within a *STEP/*END STEP.
But I tested that and it doesn’t make a difference.

I also tried C3D8 instead of C3D8I, again no difference.

A similar test with C3D20R elements did not show a difference, though.
Edit1: C3D20R also shows the same difference in elongation.

This definetely seems like a bug.

It seems to me that ORIENTATION should have no effect on an isotropic material. Or it should not be allowed for isotropic materials.

Looking through my own files, I don’t think that I’ve ever used ORIENTATION in combination with an isotropic material.

Edit2: ORIENTATION does not have an effect on a normal *ELASTIC/*PLASTIC material.

1 Like
6

I also replicated the problem using a simple tension model that is uniaxially stretched by the displacement BC as shown below (modeled in Prepomax):

image
image665×508 15.3 KB

The R-O material properties:

*MATERIAL,NAME=AA
*DEFORMATION PLASTICITY 
70000.0,0.3,360.,14.,7.

I tried the following three cases:

  1. Stretched uniaxially in the y-direction, original CSYS
  2. Stretched uniaxially in the x-direction, original CSYS
  3. Stretched uniaxially in the x-direction of the CSYS rotated by 90deg around Z-axis, using the ORIENTATION keyword as below:
*ORIENTATION,NAME=O3
0,1,0,-1,0,0

*Solid section, Elset=Solid-1, Material=AA, Orientation=O3

The stress-strain outputs show that the case 3 diverges from the first two cases:

image
image477×452 16 KB

3 Likes