Modeling NITINOL

[Jam3s]

Hello,

I've seen that there are some topics about this problem but I haven't found an answer for my question, so I explain my problem.

I need to model nitinol; in literature I've found a lot of parameters that describe nitinol and I've extract some of them that I think they are sufficient for my purpose. In Abaqus/CAE, under Materials, I've found the possibility to develop a user-defined material where you can put a list of parameters: I wonder what is the order with which I should put them there.
Reading Abaqus documentation and similar topic, I understand that I should use a VUMAT routine (I'm working in explicit): in this case, how can I put these parameters (they are temperatures, Young's moduli, startind and ending stress for both two condition, austenite and martensite: lastly, I need something simple) in a VUMAT routine?

Regards,
Jam3s

 

[glassyoffshore]

Hi James,

I'm not sure what documentation you've got but its actaully quite simple to implement, particularly if you just want to input your data for one temperature (maybe 37 degrees C). Here's some stuff off the abaqus answers site... Its a bit long winded but should help. Give it a go.
attached are the associated input files:

http://files.engineering.com/getfil...6af1&file=Templates_InputFiles_References.zip

Best of luck


offshore

wish to model the superelastic behavior of shape memory alloys such as Nitinol. Which material model should I use?
Answer
Introduction
For Version 6.4 of Abaqus, a constitutive model to simulate the superelastic behavior of alloys such as Nitinol (a nickel-titanium alloy commonly used in medical devices, such as cardiovascular stents and orthodontic wires) at finite strains is provided in the form of a UMAT subroutine for Abaqus/Standard and a VUMAT subroutine for Abaqus/Explicit. For Versions 6.5-1 and higher, the model is provided in the form of a built-in user material model for both Abaqus/Standard and Abaqus/Explicit. This model has been well tested and performs robustly for all applicable elements.
Alloys such as Nitinol exhibit superelastic behavior as they undergo reversible phase transformations between the austenite phase and martensite phase, both phases being linear elastic. This transformation produces a substantial amount of strain, which upon unloading is reversible.
The model is based on an additive strain decomposition, in which the total strain is taken as the sum of the elastic strain and the transformation strain. The transformation strain is of the order of 6%, but the elastic strain is much smaller, and should be limited to a maximum of 2%. Since the transformation strains are large compared to typical elastic strains in a metal, the material is said to be superelastic [1,2].
The material data required by the model are obtained from straightforward observations of uniaxial tests. The data characterize the start and end of the phase transformation during loading, unloading and reverse loading. The different elastic constants for the austenite and martensite phases are accounted for and user control of volumetric transformation strains is allowed. Temperature effects are included as well. At present the material formulation does not incorporate plasticity or the shape memory effects of these alloys. (If your simulation requires the modeling of plasticity or shape memory effects, please contact Abaqus West at (510) 794-5891 or via e-mail info@abaquswest.com)
User interface
The superelastic behavior is based on the uniaxial behavior shown in the attached (V)UMAT user interface documents ( umat-superelasticity.pdf and vumat-superelasticity.pdf). As explained in detail below, this material is included in the model by using the *USER MATERIAL option. The formulation uses 24 solution-dependent state variables (SDVs); this number is specified using the *DEPVAR option. Because library files are provided for Version 6.4, (rather than source code or object files), an analysis using the material model cannot be run from Abaqus/CAE. This limitation does not apply to Versions 6.5-1 and higher.
The material data required as input are explained in the aforementioned user interface documents. Different behavior in tension and compression can be specified by providing ?cLS (start of transformation during compression). The model also allows for user control of the volumetric transformation strain (?VL ) in the cases for which the user has different behavior in tension and in compression. If ?VL is not specified, it is assumed to be zero and a non-associated Drucker-Prager type formulation is used. This is recommended as the default behavior, if such data is not available, since ?VL is usually very small. As a matter of convenience, an associated Drucker-Prager formulation is used if ?VL is (artificially) made equal to ?L. Use of the unsymmetric solver is recommended when ?VL is not equal to ?L in order to avoid convergence issues.
Abaqus/Standard
Using this material model requires the user to specify 15 + NA material constants on the data lines of the *USER MATERIAL option, where NA is the number of anneals (see the Annealing section below for description of annealing) that are performed. Note that if the analysis will involve importing the model into Abaqus/Explicit, the NAME parameter must be used consistently with the conventions defined below for Abaqus/Explicit. A detailed example of the keyword usage for Abaqus/Standard is shown in umat-superelasticity.pdf
Version 6.4: The NAME parameter on *MATERIAL must be set to SUPERELASTIC, N1D_SUPERELASTIC, N2D_SUPERELASTIC or N3D_SUPERELASTIC.
Versions 6.5-1 and higher: The NAME parameter on *MATERIAL must start with ABQ_SUPER_ELASTIC. For example, a material may be named ABQ_SUPER_ELASTIC_1.
Abaqus/Explicit
Using this material model requires the user to specify 14 material constants on the data lines of the *USER MATERIAL option. A detailed example of the keyword usage for Abaqus/Explicit is shown in vumat-superelasticity.pdf
Version 6.4: The NAME parameter on *MATERIAL must be N1D_SUPERELASTIC, N2D_SUPERELASTIC, or N3D_SUPERELASTIC depending on the element type used (refer to the VUMAT interface document vumat-superelasticity.pdf).
Versions 6.5-1 and higher: The NAME parameter on *MATERIAL must start with ABQ_SUPER_ELASTIC_N1D (beam elements), ABQ_SUPER_ELASTIC_N2D (plane stress, shell, and membrane elements), or ABQ_SUPER_ELASTIC_N3D (plane strain, axisymmetric, 3D solid elements).
Supported elements
The elements that are supported for use with the material model are:
3D solids
Plane strain
Axisymmetric
Plane stress
3D shells
3D membranes
3D beams
Analysis Procedures
The material model can be used with analysis procedures that support mechanical behavior. The following procedures are commonly used in typical applications involving superelastic alloys: *STATIC, *COUPLED TEMPERATURE-DISPLACEMENT, *DYNAMIC, *DYNAMIC, EXPLICIT.
The Nitinol VUMAT does not contain any non thread-safe statements such as data, save, and common. Thus, it is safe to use this VUMAT in parallel execution for both thread-based (mp_mode=threads) parallelization and mpi-based (mp_mode=mpi) parallelization.
Installation and use
Currently, the supported platforms include Windows, Linux/Pentium, IBM, SGI, and HP Alpha, Itanium or PA-RISC.
Version 6.4

The attached archives are named as follows:
Platform Attached Archive Name
Windows Windows.ZIP
Linux/Pentium Linux32.tar
IBM IBM.tar
SGI Origin2000.tar
HP Alpha, Itanium or PA-RISC HP_Alpha_Itanium_PARISC.zip
1. Download and unzip the attached user subroutine library archive file for the platform of interest.
2. Each archive contains six separate library files. Individual .tar files for each platform are included in the HP_Alpha_Itanium_PARISC.zip archive.
3. Use the following instructions if these subroutines are never to be used with other user subroutines:
The provided user subroutine shared libraries are used by specifying the path to the installed libraries using the usub_lib_dir variable in the Abaqus environment file abaqus_v6.env. In this case, it does not matter where the libraries reside, as long as the usub_lib_dir variable is set correctly. Sample environment files are attached for Windows and Unix/Linux.
Use the following instructions if these subroutines are to be used along with other user subroutines; e.g. DLOAD, RSURFU. (This procedure might require administrative privileges).
• Find out where the Abaqus release is installed by typing (UNIX and Windows NT)
abaqus whereami
This command will give the full path to the directory where Abaqus is installed, referred to here as abaqus_dir.
• The library files contained in the archive will already exist in the abaqus_dir/cae/exec/lbr directory. Create a backup of these libraries.
• Copy the static and shared libraries from the downloaded archive to the abaqus_dir/cae/exec/lbr directory.
4.
5. Run the Abaqus analysis. If you will be using another user subroutine in addition to the Nitinol material subroutine, specify the other user subroutine file via the user parameter on the command line:
abaqus job=jobname
If the Nitinol material subroutine is the only user subroutine being used, the user parameter is not required if the usub_lib_dir variable has been correctly defined.
For additional information see:
• 'System customization parameters,' Section 4.1.4 of the Version 6.4 Abaqus Installation and Licensing Guide
• 'Execution procedure for Abaqus/Standard and Abaqus/Explicit,' Section 3.2.2 of the Version 6.4 Abaqus Analysis User's Manual
Version 6.5-1 and higher
No shared libraries or user subroutines are needed to use the model in Versions 6.5-1 and higher; the model is included in these releases as a built-in user material. When running the job, it is not necessary to include the user parameter on the command line to invoke the material model.
Limitations
For Version 6.4, the Nitinol material model may not be used with another user-defined material subroutine ((V)UMAT). This limitation has been removed for Versions 6.5-1 and higher when using the built-in user material model.
Annealing
By resetting the state variables to zero the user may anneal the material in the middle of an analysis to provide a new unloaded configuration. This procedure is different for Abaqus/Standard and Abaqus/Explicit. Sample templates are provided to illustrate the differences.
In Abaqus/Standard, annealing is done by removing the elements using *MODEL CHANGE, REMOVE and adding them back strain-free using *MODEL CHANGE, ADD=STRAIN FREE. The number of anneals to be performed during the analysis (NA) and the step numbers in which the elements are added strain free are provided on the data lines of the *USER MATERIAL option (refer to the input file template annealing-template-standard.inp in attachment Templates_InputFiles_References.zip and the UMAT user interface document).
In Abaqus/Explicit, annealing is done using the keyword option *ANNEAL (refer to the input file template annealing-template-explicit.inp in attachment Templates_InputFiles_References.zip).
Sample input files

The attached input files (Uniaxial22.inp, Uniaxial37.inp) model the superelastic behavior in a uniaxial test, where successively larger strains are imposed (refer to Figure 3 in Rebelo et al. [1]). The keyword format is for Version 6.4. The files are included in attachment Templates_InputFiles_References.zip. Additional examples demonstrating the user interface for Versions 6.5-1 and higher are included in attachment Templates_InputFiles_References.zip. The names of these files end with the _65.inp string.
References
Included in attachment Templates_InputFiles_References.zip:
1. 'Simulation of implantable nitinol stents,' Nuno Rebelo, Norm Walker and Hoss Foadian, Proceedings of the 2001 Abaqus Users conference
2. Spring 2001 issue of SIMULIA Answers
Additional references:
• Auricchio, F. and Taylor, R.L., "Shape-memory alloys: modeling and numerical simulations of the finite-strain superelastic behavior," Computer Methods in Applied Mechanics and Engineering, 1997, vol. 143, pp. 175-194.
• Auricchio, F., Taylor, R.L. and Lubliner, J., "Shape-memory alloys: macromodeling and numerical simulations of the superelastic behavior," Computer Methods in Applied Mechanics and Engineering, 1997, vol. 146, pp. 281-312.
[attach_link]http://files.engineering.com/getfile.aspx?folder=06040b7b-313c-49d3-b4c7-509944e86af1&file=Templates_InputFiles_References.zip[/attach_link]

 

[amubashar]

Hi

glassyoffshore:

Are the files attached in your post from Abaqus my support website? As far as I know, these are only available to customers with support.

 

[bassmanjax]

What glassyoffshore posted is available to customers without support, so I don't think there is an issue there.

Martin Stokes CEng MIMechE

 

[Jam3s]

Hi glassyoffshore,
thanks for the reply.
I had a look at your post and at the file that you attached and I would ask you some questions because I haven't solved my problem (perhaps, simply I don't understand your reply).

I tried two ways: first, I've change my .inp file simply introducing some lines that I took from files that are in .zip file that you attach; second, in Abaqus/CAE I've created a USER DEFINED material copying the value in the same order with which they appear in the files you attach.
In both case, the software returns to me error.
Where do I mistake? I don't think could be a problem of library because I work on Abaqus 6.8EF1.
Regards,
Jam3s