The Results Available for Thin Shell Elements
The results available for thin shell elements
Thin shell elements write the results to the .PTF file. The following tables show the raw data components, and those derived by D3PLOT.
Symmetric stress tensor: |
|
|
|
|
||
This is assumed to be written in the global Cartesian coordinate system at <maxint> surfaces. Its output is on by default, but may be switched off using the SIGFLG parameter on the *DATABASE_EXTENT_BINARY control card. (See Controllable contents of the complete state file )
The stress components that can be derived by D3PLOT ( Manipulations of Stress Tensor Components ) are:
In addition D3PLOT will calculate the 2D in-plane maximum and minimum principal stresses and maximum shear stress:
These "2D" values are calculated by the following process:
- Rotate the global stress tensor to the element local axis system.
- Using only the local Sxx , Syy and Txy terms calculate the 2D max and min principal stresses
This means that the local Tyz and Tzx terms are implicitly treated as being zero and the element is treated as being plane stress, which may be more or less true in the middle of a panel but is unlikely to be the case at the edges of a panel and at connections. Therefore please use these terms with care.
Effective plastic strain |
|
The effective plastic strain is written at the same <maxint> surfaces as the stress tensor. It has no intrinsic direction. By default it is switched on , but may be turned off using the EPSFLG parameter on the *DATABASE_EXTENT_BINARY control card. (see A further explanation of strain components for more information about strains)
Strain rate for thin shells
For shell elements where bending takes place knowledge of nodal rotations would be required, and this information is not available. Therefore the strain rate in shells is approximated by:
This value is a poor approximation because effective plastic strain will only ever increase, so the result will always be zero or positive, and moreover it does not consider any elastic strains. Nevertheless in a loading regime that is mostly uniaxial it gives a reasonable result.
Extra variables for thin shells
If NEIPS has been defined on the *DATABASE_EXTENT_BINARY control card then <neips> "extra" variables will be written at each of <maxint> surfaces (as for the stress tensor above). D3PLOT will accept any number of these, but will only process the first 99. These have the names:
| SH1_SHELL_EXTRA_1 | to | SH9_SHELL_EXTRA_99 |
They are treated as separate scalar values of unknown type which may be contoured and written out, but not processed in any way.
*DEFINE_MATERIAL_HISTORIES for thin shellsIf *DEFINE_MATERIAL_HISTORIES cards have been defined, these will overrule the value of NEIPS on the *DATABASE_EXTENT_BINARY control card and the number of "extra" variables will be defined by the number of *DEFINE_MATERIAL_HISTORIES cards. D3PLOT will accept any number of these, but will only process the first 99. These have the names: They are treated as separate scalar values of unknown type which may be contoured and written out, but not processed in any way. The *DEFINE_MATERIAL_HISTORIES component category is only available in D3PLOT if a ZTF file is present. These variables will also be present in D3PLOT in the Extra component category as described above. When the NAMES option is active, history variable components are given this name in D3PLOT (the first 27 characters of the name will be displayed), otherwise they are given the corresponding label. |
Directional strain tensor for thin shellsIf STRFLG has been set on the *DATABASE_EXTENT_BINARY control card the symmetric strain tensor for thin shells will be written out at the innermost and outermost integration points only, regardless of the value of <maxint> . This is assumed to be oriented in the global Cartesian coordinate system. (see A further explanation of strain components for more information about strains) |
|
|
And the strains derived from these by D3PLOT ( Manipulations of Strain Tensor Components ):
For shells, the engineering strains are derivied ( Manipulations of Strain Tensor Components ):
The following components are the shear strain components multiplied by a factor of 2. See Manipulations of Strain Tensor Components for more details.
In addition D3PLOT will calculate the 2D in-plane maximum and minimum principal strains and maximum shear strain:
These "2D" values are calculated by the following process:
- Rotate the global strain tensor to the element local axis system.
- Using only the local Exx , Eyy and Exy terms calculate the 2D max and min principal strains
This means that the local Ezz , Eyz and Ezx terms are all implicitly treated as being zero and the element is treated as being plane strain. Bearing in mind that Ansys LS-DYNA populates all 6 terms of the strain tensor (local Ezz being finite due to the need to conserve volume) this is a gross simplification, and these terms should be used with care.
D3PLOT will calculate the ratio of E2MIN_2D_PRINC_STRAIN / E2MAX_2D_PRINC_STRAIN which can be used to give an indication of the stress state:
A problem arises when trying to distinguish between biaxial tension and biaxial compression as in both cases they return a +ve value. In fracture predictions it is important to distinguish between the two so, whilst it is possible that a compressive state could give a shear fracture, the most likely outcome would be buckling. Therefore, when both E2MAX_2D_PRINC_STRAIN and E2MIN_2D_PRINC_STRAIN are negative (or 0) a value of 1.1 is returned to indicate a compressive state.
The ratio is capped to -100 to avoid large values if E2MAX_2D_PRINC_STRAIN is relatively small compared to E2MIN_2D_PRINC_STRAIN.
Shell force and moment resultants
Shell force and moment resultants are written as <Force/unit width> and <moment/unit width> in the element local coordinate system. By default these are on , but they can be switched off with the RLTFLG flag on the *DATABASE_EXTENT_ BINARY control card. (These components are explained in FX_ etc Explanation of Shell Force and Moment Resultants .)
|
|
Stresses derived by D3PLOT from the force & moment resultants. (These components are explained in XA_ etc Stresses in Thin Shells Derived from Force and Moment Resultants .)
|
|
Thickness and Internal energy density components
By default these components are written. They can be turned off with the ENGFLG flag on the *DATABASE_EXTENT_BINARY control card.
Components derived geometrically by D3PLOT
Shell area is calculated from the nodal coordinates:
| AS_AREA_OF_SHELL | ON_OUTWARD_NORMAL |
Geometric componentsThese components are extracted from the topology, and can be output in :
|