NE is it similar to E (Strain)

[afefdridi]

Helllo

please i hae a question in abaqus is the E similar to NE (Nominal strain) i would like to know which of these terms to use to compare with experimental tensile test data please any suggestion

 

[afefdridi]

Any help please

 

[Dave442]

Straight from the users manual:

Strain output

The total strain E is composed of the elastic strain EE, the inelastic strain IE, and the thermal strain THE. The inelastic strain IE consists of the plastic strain PE and the creep strain CE.

For geometrically nonlinear analysis Abaqus/Standard makes it possible to output different strain measures as well as elastic and various inelastic strains. The various total strain measures (integrated strain measure E, nominal strain measure NE, and logarithmic strain measure LE) are described in “Conventions,” Section 1.2.2. The default strain measure for output to the data (.dat) and results (.fil) files is E. However, for geometrically nonlinear analysis using element formulations that support finite strains, E is not available for output to the output database (.odb) file, and LE is the default strain measure.

Stress and strain measures

The stress measure used in Abaqus is Cauchy or “true” stress, which corresponds to the force per current area. See “Stress measures,” Section 1.5.2 of the Abaqus Theory Guide, and “Stress rates,” Section 1.5.3 of the Abaqus Theory Guide, for more details on stress measures.

For geometrically nonlinear analysis, a large number of different strain measures exist. Unlike “true” stress, there is no clearly preferred “true” strain. For the same physical deformation different strain measures will report different values in large-strain analysis. The optimal choice of strain measure depends on analysis type, material behavior, and (to some degree) personal preference. See “Strain measures,” Section 1.4.2 of the Abaqus Theory Guide, for more details on strain measures.

By default, the strain output in Abaqus/Standard is the “integrated” total strain (output variable E). For large-strain shells, membranes, and solid elements in Abaqus/Standard two other measures of total strain can be requested: logarithmic strain (output variable LE) and nominal strain (output variable NE).

Logarithmic strain (output variable LE) is the default strain output in Abaqus/Explicit; nominal strain (output variable NE) can be requested as well. The “integrated” total strain is not available in Abaqus/Explicit.

 

[afefdridi]

thanks a lot for your response another question please. If i use an hyperelastic material and i have a tensile test data (true and engeneerng data) which one must i use when i define the material. thanks a lot

 

[Dave442]

Again, straight from the users manual (you should read it):

The strain data should be given as nominal strain values (change in length per unit of original length). For the uniaxial, equibiaxial, and planar tests stress data are given as nominal stress values (force per unit of original cross-sectional area). These tests allow for entering both compression and tension data. Compressive stresses and strains are entered as negative values.

Good Luck,
Dave

 

[afefdridi]

Thanks dave i tried to read what you advised me to read but i can not find "conventions' if you can please give me exactly in which module of the documentation can i find it

 

[Dave442]

Everything I pasted is from the Abaqus Analysis User's manual. The section your'e looking for is 1.2.2 Conventions. Within that section there is a topic Stress and Strain Measures. There is also 22.5.1 Hyperelastic Behaviour of Rubberlike Materials. You should read that too.

Within the documentation there are links to relevant sections of other manuals that you can also follow and read. Read it all.