Can I change material model in-between step in ABAQUS using field variable? 1

[Wonder_Women]

I want to change my material model in-between step in a 5-step analysis. In the first 4 steps, I want to use Concrete damage plasticity model and in the last 5 step I want to use Concrete Drucker Prager model.
Is it possible to do without using subroutine USDFLD file. Since I am not familiar with this.

 

[Mustaine3]

It's not possible. You can only change the material parameter, but not the underlying material model.

Maybe you can run the first 4 steps. Then you define a new analysis for step 5 with the deformed mesh, define the new material model and reuse the latest result as initial conditions. See keyword reference manual at *Initial Conditions.

 

[FEA way]

Here’s an example of how to set time dependence of material properties using field variables:

https://www.eng-tips.com/viewthread.cfm?qid=459126

Unfortunately it’s not possible to change material model this way.

 

[Wonder_Women]

Thank you so much Mustaine3 and FEA way for your reply. I will try to implement your suggestion.
So, (to be sure) I can't change the material model in between steps. There is no way except the suggestion you gave me? Right? not even any subroutine?
I am asking because I was struggling from weeks to figure it out.

 

[FEA way]

Impossible to do it this way with or without subroutine. You can’t define CDP and Drucker Prager model for the same material simultaneously (they are mutually exclusive). And you can’t assign two different materials to the same section. And if you assign two section to the same elset, the first one will be overriden by the second one.

 

[Wonder_Women]

Ok Thanks.
My 5th step is thermal stress analysis. I am using sequentially coupled thermal stress analysis. So, In the 5th step I am already taking Nodal-Time temperature values in the predefined field by calling .odb file( obtain from heat transfer analysis).

So if i create 2 separate models.
Model-1: contains 4 steps (with concrete damaged plasticity model.)
Model-2: contains 1 step (with Drucker Prager model): I will be creating 2 predefined fields. one for nodal time-temp curve in step-1. and second in initial step to take the results of Model-1 as the initial state. (as shown in attached file)

Is this correct? This is what you meant?

 

[Mustaine3]

No. When you use this option you would do an Import analysis. So you would reuse the part with all it's results, but also with it's material model.

You have to choose 'Mechanical' and then 'Stress'. This would only transfer the stresses to a new part with a different material model.

But you have to import the part into CAE first, so you use the same mesh. Otherwise the Element IDs won't fit between both analysis and the transfer of data will create weird stuff.

Test it on a simple example first.

 

[JAIN-FEM]

Hi Mustain3 and FEA way

I have similar problem, following is the input file
while importing the input file after doing *INITIAL CONDITIONS and *FIELD keywords , i am getting this warning in abaqus command line. Would you be able to suggest anything. also even after trying this, the material seems to remain the same i.e. the first one with field 1=1. Please help!

WARNING: The following keywords/parameters are not yet supported by the input file reader:
---------------------------------------------------------------------------------
*FIELD
*INITIAL CONDITIONS, TYPE=FIELD
*PREPRINT


INPUT FILE SNIPPET

** MATERIALS
**
*Material, name=MATERIAL-1
*Density
1800.,
*Elastic, dependencies=1
3e+07, 0.3, , 1.
6E07, 0.3, , 2.
**
** BOUNDARY CONDITIONS
**
** Name: Disp-BC-1 Type: Symmetry/Antisymmetry/Encastre
*Boundary
_PICKEDSET6, ENCASTRE
** Name: Disp-BC-2 Type: Symmetry/Antisymmetry/Encastre
*Boundary
_PICKEDSET5, PINNED
** ----------------------------------------------------------------
**
[highlight #FCE94F]*INITIAL CONDITIONS, TYPE=FIELD
NODESET, 1.0[/highlight]
** STEP: Step-1
**
*Step, name=Step-1, nlgeom=NO
*Static
2., 2., 2e-05, 2.
**
** LOADS
**
** Name: SURFFORCE-1 Type: Pressure
*Dsload
_PICKEDSURF7, P, 5000.
**
** OUTPUT REQUESTS
**
*Restart, write, frequency=0
**
** FIELD OUTPUT: F-Output-1
**
*Output, field, variable=PRESELECT
**
** HISTORY OUTPUT: H-Output-1
**
*Output, history, variable=PRESELECT
*End Step
** ----------------------------------------------------------------
**
** STEP: Step-2
**
*Step, name=Step-2, nlgeom=NO
*Static
2., 2., 2e-05, 2.
[highlight #FCE94F]*FIELD
NODESET, 2.0[/highlight]
**
** LOADS
**
** Name: Load-2 Type: Pressure
*Dsload
_PickedSurf11, P, 5000.
**
** OUTPUT REQUESTS

 

[JAIN-FEM]

In another attempt, with following input file, it does not recognises *FIELD and *PREPRINT and gives this warning

WARNING: The following keywords/parameters are not yet supported by the input file reader:
---------------------------------------------------------------------------------
*FIELD
*PREPRINT




INPUT FILE SNIPPET
ASSEMBLY
**
*Assembly, name=Assembly
**
*Instance, name=Part-1-1, part=Part-1
*End Instance
**
*Nset, nset=NODESET, instance=Part-1-1, generate
1, 66, 1
*Nset, nset=_PickedSet5, internal, instance=Part-1-1
1, 11, 12, 22, 23, 33, 34, 44, 45, 55, 56, 66
*Elset, elset=_PickedSet5, internal, instance=Part-1-1
2, 19, 22, 39, 42, 59, 62, 79, 82, 99
*Nset, nset=_PickedSet6, internal, instance=Part-1-1, generate
56, 66, 1
*Elset, elset=_PickedSet6, internal, instance=Part-1-1, generate
82, 100, 2
*Elset, elset=__PickedSurf7_S1, internal, instance=Part-1-1, generate
1, 19, 2
*Surface, type=ELEMENT, name=_PickedSurf7, internal
__PickedSurf7_S1, S1
*Elset, elset=__PickedSurf9_S1, internal, instance=Part-1-1, generate
1, 19, 2
*Surface, type=ELEMENT, name=_PickedSurf9, internal
__PickedSurf9_S1, S1
*End Assembly
[highlight #FCAF3E]*Amplitude, name=Amp-1, time=TOTAL TIME
0., 1., 2., 2., 4., 3.[/highlight]
**
** MATERIALS
**
*Material, name=Material-1
*Density
1800.,
[highlight #FCE94F]*Elastic, dependencies=1
3e+07, 0.3, , 1.
1.2e+08, 0.3, , 2.
1.6e+08, 0.3, , 3.[/highlight]
**
** BOUNDARY CONDITIONS
**
** Name: BC-1 Type: Symmetry/Antisymmetry/Encastre
*Boundary
_PickedSet6, ENCASTRE
** Name: BC-2 Type: Symmetry/Antisymmetry/Encastre
*Boundary
_PickedSet5, PINNED
** ----------------------------------------------------------------
**
** STEP: Step-1
**
*Step, name=Step-1, nlgeom=NO
*Static
2., 2., 2e-05, 2.
**
[highlight #FCAF3E]** field variable definition
*FIELD, VARIABLE=1, AMPLITUDE=Amp-1
NODESET, 2[/highlight]
** LOADS
**
** Name: Load-1 Type: Pressure
*Dsload
_PickedSurf7, P, 5000.
**
** OUTPUT REQUESTS
**
*Restart, write, frequency=0
**
** FIELD OUTPUT: F-Output-1
**
*Output, field, variable=PRESELECT
**
** HISTORY OUTPUT: H-Output-1
**
*Output, history, variable=PRESELECT
*End Step


After importing the inp file by going to FILE-->IMPORT-->MODEL--> input filename, I went to MODEL-->Edit keywords-->selected my model name , which showed the input file(attached below) but when compared from input file that i imported, these two were different. The difference is that ABAQUS is completely overlooking **field variable definition, this is not visible there. Can you pl. guide?

https://files.engineering.com/getfile.aspx?folder=c4e9a9b7-ee98-4803-83d7-d578cd6ee74c&file=1.JPG

https://files.engineering.com/getfile.aspx?folder=aa624d38-0ee5-48ae-9256-a6b18e9fceae&file=2.JPG

https://files.engineering.com/getfile.aspx?folder=d4b605ac-2f17-47dd-b15d-7f23c11ccb36&file=3.JPG