Postprocessing——Extra History Variables in LS-DYNA

caeguy

Postprocessing
  
Extra History Variables in LS-DYNA
  
Ref: See NEIPH and NEIPS in *database_extent_binary.
  
For Euler/ALE materials:
  
History variable number ...  
  
1  =  density  
2  = volume fraction of 1st multi-material group (formulation 11) or single Eulerian material (formulation 12)   
3 = volume fraction of 2nd multi-material group (formulation 11)  
etc.  
n+1 = volume fraction of nth multi-material group (formulation 11)  
n+2 = group number of the predominant multi-material group in the current cell (element)  
  
for STRFLG=0, where n is the number of multi-material groups
  
History variable number n+2 (where n is the total number of multi-material groups) is the identity of the principal material in each element. For instance, consider an Eulerian simulation comprised of three multi-material groups and a cell (element) with volume fractions of 0.3, 0.5 and 0.2, respectively, for the three materials. History variable 5 would then equal 2.0, because material group 2 is the majority material group for that element. Use the n+2 history variable to visualize the movement of material through cells by fringing that component in LS-POST.  
  
If STRFLG is set to 1 (strains saved) in *database_extent_binary, the first six history variables for the Euler/ALE solid elements are the six logarithmic strain components. Density will be the 6+1=7th history variable.
  
For Lagrangian materials:
  
For Lagrangian materials, the number of and meaning of extra history variables are dependent on the material model and element type. Unfortunately, there is no comprehensive documentation on this subject. There is mention of extra history variables in the User's Manual for a few material models, e.g., mat 22. For other materials, the only definitive means of identifying the extra history variables is through painstaking examination of the source code. In some cases, the extra history variables may be of some interest to the user, but more often, they are not of any interest and can be ignored.
  
If STRFLG is set to 1 (strains saved), the last six extra history variables for Lagrangian solid elements are strains.
  
Post-processing Extra History Variables in LS-POST
  
Extra history variables, when written to the d3plot database, may be fringed using LS-POST by selecting Fcomp > Misc > history var #. A time history plot of the extra history variable may then be created by selecting History > Scalar.
  
Extra History Variables for User-Defined Materials
  
Extra history variables can be employed to great benefit in the case of a user-defined material routine. Clearly in that situation, the user knows what the extra history variables are. In pre-970 versions of LS-DYNA, the 1st history variable in the umat subroutine won't be stored as history var#1 in the d3plot database. The storage location is dependent on a number of factors such as whether the subroutine is vectorized or nonvectorized, whethere the elements are shells or solids, etc. More on this subject comes from Lee Bindeman:
  
"When using a vectorized subroutine (i.e. umat46v instead of umat46) and a 3D user defined material (for 3D solid elements), there are 6 history variables automatically used for 6 terms of the transformation matrix, whether or not the user defined material is orthotropic. When the material is orthotropic (IORTHO=1), these 6 variables are automatically allocated, however, when the material is not orthotropic (IORTHO=0), the variables are not and it is essential that these be allocated by the user defined material input. Therefore, if your material uses 46 history variables, you need to set NHV=52. In order to write your 46 history variables to the d3plot files, you need to request 52 extra history variables by setting NEIPH=52 on *DATABASE_EXTENT_BINARY.
  
When post processing, history variables 1 to 6 will contain the transformation matrix terms. If the material is isotropic, these will all be zero. History variables 7 to 52 will contain history variables 1 to 46 in your subroutine.
  
The above rules change for 2D materials (for shell elements). In that case, there are only 2 transformation terms stored so only 2 extra history variables need to be allocated and requested.
  
Perhaps some good news is that I made a fix today to eliminate much of this confusion. The fix is in version 970 revisions 2903 and later.
  
With this fix, it is no longer necessary to allocate extra history variables with NHV, or to request 6 (or 2) extra history variables in the d3plot file. You simply need to allocate the same number of history variables that you want to use, and to request the number that you want written to the d3plot file. If the material is isotropic (IORTHO=0), then the transformation terms will be omitted and then the history variable numbers in the user subroutine will match those in the d3plot file. However, if the material is orthotropic (IORTHO=1), then the 6 (or 2) transformation terms will be written to the d3plot file so there will be a mismatch in the numbering of history variables in the user subroutine and the d3plot file."
  
jpd 12/2002
3/4/2003
4/4/2003
6/4/2003
  
Finding Maximum Component Values
  
To identify the location of minimum or maximum fringed components, choose Range > Ident Max value or Range > Ident Min value after you create your fringe plot. When selected, the option highlights the element associated with the min/max quantity and posts the element ID on the fringe plot.
  
To create a fringe plot which displays the maximum value of a particular component through all time for each element, use the Frin button in the Fcomp menu. For example, to fringe maximum x-stresses lick on Frin (just below the Apply button) and select XFrn . Next, select Fcomp > Stress > x-stress > Apply . This fringe plot is useful for determining the spatial distribution of peak response. Subsequently using Range > No Average and Output > ElementResults will produce an ASCII file of peak values for each element but not an abbreviated list of peak values for each part.
  
To create a time history plot which displays the maximum value of a particular component (e.g., x-stress) at each point in time across an entire part, use History > Element > x-stress > Plot . Before choosing Plot , click on Value: Elm (located under the list of components), select Max, and select a part by clicking on it in the graphics window. This history plot is useful for determining the temporal variation of peak response within a single part. On the history plot, an element ID, peak value, and time of the peak value is listed.
  
jpd 12/2002

三颗智齿

查找损伤的时候发现这篇好帖子，解答了我大部分的问题，沉了实在可惜，顶起来，想知道损伤输出设定的筒子们好好看看吧。