Surface/Integration Points
This option can be used to select which surface data is plotted for for Shell and Thick Elements and how multiple integration point data is plotted for Shell, Thick Shell and Solid Elements. If the model contains fully integrated shells with results output at each on plan integration point (MAXINT set to a negative value on the *DATABASE_EXTENT_BINARY card) or fully integrated solids with results output at each integration point (NINTSLD set to 8 on the *DATABASE_EXTENT_BINARY card) then an option can be set to plot all the individual on plan points / solid integration points (default) or average them to a single point per shell / per solid and then plot. By plotting all integration points, the variation of data across the Shell or Solid can be seen.
If the current data component is a Beam Component then this option can be used to select the Beam Integration point.
Shell Surfaces
This figure shows the shell integration point selection box, which applies to stress and strain tensor derived results.
By default shells write results at 3 "surfaces":
| Top |
Is the outermost (most +ve local Z) integration point. |
Note that when using the default Gaussian integration rules in Ansys LS-DYNA the inner and outer integration points of shells are NOT the "outer fibres" of the element. For a fuller explanation see the WARNING below. |
| Middle | Is the neutral axis, i.e. mid-plane. | |
| Bottom |
Is the innermost (most -ve local Z) integration point. |
In this example shell output has been defined with < maxint > = 11, giving the option of each of the 11 integration points in the element.
Before D3PLOT 11.0, the layers were in the order of the integration points output by Ansys LS-DYNA, e.g. for < maxint >=3 Layer 1 was the MIDDLE surface, Layer 2 was the BOTTOM surface and Layer 3 was the TOP surface (see Thin shell integration points ). From v11.0 onwards Layer 1->Layer n is always Bottom->Top (so long as a .ztf file is present).
|
From Version 13 onwards, if there is no data for the selected integration point the shells are greyed out. In this example "Layer 3" is selected, but some shells only have data at two integration points.  |
|
Normally you will be interested in results at a given integration point, but it is also possible to extract the following values scanned from all integration points through the thickness of the element and the derived mid-surface value if the element does not have an integration point at the mid-surface:
It should be noted that when shell results for surfaces MAX_ALL, MIN_ALL or MAG_ALL are calculated at nodes, first the nodal values (averaged over the connected elements) at each integration point are calculated and then these values are scanned to find the max, min or mag value. This means that the max/min/mag value at a node can be different to the average of the corresponding max/min/mag values of the connected shells as the shell values may not all come from the same through thickness integration point. |
Shell integration point data written from Ansys LS-DYNA
There are two issues to be considered here:
- The number of through thickness integration points in the shell element formulation.
- How many integration points worth of data are written to the database files.
Unfortunately these two parameters are not directly related in Ansys LS-DYNA, and have to be set independently:
- Shell element through-thickness integration points are controlled on the *SECTION_SHELL card. (Composites are different)
- The number of "surfaces" output is controlled by parameter < maxint > on the *DATABASE_EXTENT_BINARY card
By default (< maxint > = 3) data at three "surfaces" (top, middle and bottom) are written for all shell elements, regardless of the actual number of integration points in any element formulation. Normally this is satisfactory, since in most models with significant plastic strain the detailed distribution of stress and strain through element thickness is not that important, but where models remain mainly elastic or where composites are used it may be necessary to set a different value. See Thin shell integration points for a fuller discussion of these parameters and how they affect output.
Note 1: While thick shells write results at surfaces too, by default this flag has no effect when they are plotted since their (visual) thickness permits all three surface results to be displayed simultaneously on their respective faces. This can be changed so that each surface is plotted separately, as described in Contour Display Options for Thick Shells
Note 2: Historically Ansys LS-DYNA has reverted to trapezoidal integration for 6+ integration points, although this is undocumented and the author has a sneaking suspicion that more recent versions of Ansys LS-DYNA may use Gaussian integration for up to 11 points. Examine such results with care!
A more detailed description of shell output, with particular reference to "surfaces",
"layers" and integration schemes, is given in
Thin Shell Integration Points
.
Beam Integration Points
This figure shows the beam integration point selection box, which applies to results from "integrated" (Hughes-Liu etc) beams.
The "extra" results for these beam types only are written at the specified integration points. Only one can be plotted at a time, and this is selected here.