# \*DEFORMATION PLASTICITY depends on \*ORIENTATION **URL:** \ **Category:** Analysis issues\ **Created:** [March 24, 2026, 11:54pm UTC](https://calculix.discourse.group/t/deformation-plasticity-depends-on-orientation/3844 "2026-03-24T23:54:08Z")\ **Posts on this page:** 6\ **Page:** 1
**Author:** ![vicmw](https://avatars.discourse-cdn.com/v4/letter/v/6de8d8/32.png) [@vicmw](https://calculix.discourse.group/u/vicmw)\ **Post date:** [March 24, 2026, 11:54pm UTC](https://calculix.discourse.group/t/deformation-plasticity-depends-on-orientation/3844/1 "2026-03-24T23:54:08Z")
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](https://global.discourse-cdn.com/free1/uploads/calculix/original/2X/2/21dc82a9a226e7564815378ab582d91ed4e31c61.png) ```plaintext ** 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 ``` ---
**Author:** ![xyont](https://yyz2.discourse-cdn.com/free1/user_avatar/calculix.discourse.group/xyont/32/3553_2.png) [@xyont](https://calculix.discourse.group/u/xyont)\ **Post date:** [April 2, 2026, 2:49am UTC](https://calculix.discourse.group/t/deformation-plasticity-depends-on-orientation/3844/2 "2026-04-02T02:49:34Z")
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](https://global.discourse-cdn.com/free1/uploads/calculix/original/2X/2/266d0c5cd2882dbb9fd750f55a93f3eb03e12801.png) ---
**Author:** ![vicmw](https://avatars.discourse-cdn.com/v4/letter/v/6de8d8/32.png) [@vicmw](https://calculix.discourse.group/u/vicmw)\ **Post date:** [April 2, 2026, 3:21am UTC](https://calculix.discourse.group/t/deformation-plasticity-depends-on-orientation/3844/3 "2026-04-02T03:21:47Z")
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? ---
**Author:** ![xyont](https://yyz2.discourse-cdn.com/free1/user_avatar/calculix.discourse.group/xyont/32/3553_2.png) [@xyont](https://calculix.discourse.group/u/xyont)\ **Post date:** [April 2, 2026, 5:18am UTC](https://calculix.discourse.group/t/deformation-plasticity-depends-on-orientation/3844/4 "2026-04-02T05:18:24Z")
right, an error message shown orientation not allowed to be used for this type of material. ---
**Author:** ![rsmith](https://yyz2.discourse-cdn.com/free1/user_avatar/calculix.discourse.group/rsmith/32/1684_2.png) [@rsmith](https://calculix.discourse.group/u/rsmith)\ **Post date:** [April 2, 2026, 10:59am UTC](https://calculix.discourse.group/t/deformation-plasticity-depends-on-orientation/3844/5 "2026-04-02T10:59:49Z")
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. ---
**Author:** ![shah](https://avatars.discourse-cdn.com/v4/letter/s/f4b2a3/32.png) [@shah](https://calculix.discourse.group/u/shah)\ **Post date:** [April 2, 2026, 3:52pm UTC](https://calculix.discourse.group/t/deformation-plasticity-depends-on-orientation/3844/6 "2026-04-02T15:52:25Z")
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](https://global.discourse-cdn.com/free1/uploads/calculix/original/2X/c/c990ea3e9a20fb5ec51832857a9886babdb46c17.png) The R-O material properties: ```auto *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: ```auto *ORIENTATION,NAME=O3 0,1,0,-1,0,0 ``` ```auto *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](https://global.discourse-cdn.com/free1/uploads/calculix/original/2X/b/b1237b5d42e40ea64f66e151771a2bb56ad00972.png)