RE: MAXINT

It is the first case, zeros for IPs # 5-58 and there is no alternate option to suppress the writing for these non-existent layers.

I am aware of a couple of options to create smaller d3plots:

1) Use *DEFINE_MATERIAL_HISTORIES to control the content of the history variables in the d3plot database. This feature is supported for solid, beam and shell elements.
2) Dynamore has a tool to create new d3plot files from existing ones which can be used to create a smaller database, see https://www.dynamore.de/en/products/tools/plotcprs.

babu
Ticket#2019071110000047

Hi Support,
 
One of our client has a big composites model. One of the parts of the model has 58 layers and they want to request output for each one of them (MAXINT=58).
 
The rest of the parts of the model only have 4 IP. However, as they set MAXINT to 58, for the thinner parts, when they look at the results in the post-processor, they still get output for 58 IP (from 5 to 58 it is all 0.0). They are worried about the size of the outputs.
 
The question is: for these 5 to 58 IPs (for the thinner parts), is LS-DYNA outputting 0.0 for each one of them (hence, creating very big output files with lots of zeros, expect for the only part that has 58 IPs)? Or is DYNA just not generating output for IP 5-58 of the thinner parts, and it is just the post-processor that shows the outputs for these IPs as 0.0 as they have no value defined?
 
If it is the first case, is there any way to supress the writing for these layers that “do not exist” in some parts in order to reduce the size of the output files?
 
___________________________________________________________________

Our stress update is done using increments of deformation.  The increments are calculated in the local coordinate system and used to calculate stress increments.  This is very fast, but for large shear, the choice of coordinate system changes the result.  It's not obvious in this problem because the motion is prescribed.  However, if force loading was used instead, the deformation would not be at all the same.  We really cannot solve this problem well using an updated Lagrangian type of approach.  There is no good fix for this.

The transformations that we do in the element and output are a good match so there is nothing to fix there either.  I'm going to close this as a "wontfix".

lpb
Bug 12322
Ticket#2016052610000153
______________________________________________________

Stress and strain output corresonds to integration point locations.   
Thus Lobatto integration (see INTGRD in *control_shell) is required to get 
output corresponding to the outer surfaces. 
In the case of stress or effective plastic strain, MAXINT in *database_extent_binary 
controls how many of the shell through-thickness integration points are output.   

If MAXINT is negative, all 4 of the in-plane integration point stresses are output
(no intpt averaging is done) at each of the |MAXINT| through thickness locations (applies
only to fully integrated shell formulations; affects only d3plot, d3part, d3thdt).
For corresponding control in elout data, see INTOUT in *database_extent_binary.

***NEW ~ Sep 2012 ***
In *control_output:
EOCS	Elout Coordinate System: controls the coordinate system to be used when writing out shell data to the elout file:
  EQ 0: default
  EQ 1: local element coordinate system
  EQ 2: global coordinate system
***********************

Tensorial (true) strains at output at the uppermost and lowermost integration points 
only and only when STRFLG=1 in *database_extent_binary.  
See the tables under *section_shell for integration point locations.

See also:
shellstrain
shell_resultants