Thin Shell Integration Points
Thin shell integration points
From 1 to n through the thickness.The majority of shell element formulations in Ansys LS-DYNA have a single integration point on plan, with from 1 to <n> integration points through their thickness. The "fully integrated" formulations have 2 x 2 integration points on plan, and again from 1 to <n> points through the thickness. For more information about shell formulations refer to the Ansys LS-DYNA theory manual.
If MAXINT is a positive value then Ansys LS-DYNA will write results at the element centre as viewed on plane. For fully integrated formulations this will be the averaged value of the in-plane integration points.
If MAXINT is a negative value then Ansys LS-DYNA will write results at 2 x 2 integration points as viewed on plane. This is true for all element formulations regardless of whether they are fully integrated or not. If a ZTF file has been written from PRIMER, then D3PLOT will be able to determine which integration point results are valid for each Shell element and disregard them if they are not relevant. Without the ZTF file D3PLOT will not have the information required to determine this and will only read data from the first on plan integration point.
For the purposes of this discussion we will consider the case where MAXINT is positive since we can then ignore the number of integration points on plan. What we are concerned with here is the number through the thickness, (as viewed in elevation) and we must consider two cases:
Case 1: MAXINT on the *DATABASE_EXTENT_BINARY card is set to the default of three.
In this situation, regardless of the number of integration points through the thickness used in the shell element formulation(s ), stress tensor and plastic strain output for all shell elements is written at three "surfaces":
| "Top" | : | The outermost integration point |
| "Middle" | : | The neutral axis |
| "Bottom" | : | The innermost integration point |
The outer integration point is located on the +ve local Z' of the neutral axis, the inner on the -ve Z' side. (Membrane elements with a single integration point write the same value to all three surfaces.)
The important thing to note here is that, unlike linear-elastic codes, Ansys LS-DYNA reports "top and bottom surface" stresses at the outer and inner integration points, and not at the element outer fibres.
Assuming the default Gaussian integration scheme is used the location of the outermost integration points is given in the following table as a function of shell thickness/2 ( t/2 ) for the range of 1 to 6 integration points through the thickness.
| No of Points |
Distance from neutral axis as a proportion of t/2 (Gaussian integration) |
|
| 1 | 0.0 (membrane) |
|
| 2 |
0.577 |
|
| 3 | 0.775 | |
| 4 |
0.861 |
|
| 5 | 0.906 | |
| 6 | 0.932 | |
Note:
| Prior to LS-960 | If the element formulation uses >5 integration points through its thickness then trapezoidal integration is used - even if Gaussian is specified.. |
| From LS-960 onwards | The user manual claims that Gaussian integration is used for any number of points if specified. |
It is possible to specify "user-defined" integration rules, which may locate integration points at different points through the thickness. For example Gauss-Lobatto quadrature will locate the outer and inner integration points on their respective outer fibres, but there is a speed penalty to pay for this.
In addition, in many analyses the section will be largely plastic, and the exact values of stress will be somewhat academic. Generally highly nonlinear problems are more concerned with plasticity and consequent energy absorption. However if you are in, or close to, the linear elastic region, and/or exact stress levels are important, you should consider using more integration points in order to extract results more precisely.
Case 2: "Layer" output with MAXINT set to some value other than the default of 3
In this situation Ansys LS-DYNA writes out the stress tensor and plastic strain values for the first <maxint> integration points in the shell, starting at the innermost (bottom) one. You would generally only use this for composites analysis where results in all layers are significant.
|
(1) |
Ansys LS-DYNA no longer calculates the "middle" neutral axis values for you. If you have an odd number of integration points D3Plot assumes that the middle one is the neutral axis value, if you have an even number of integration points D3Plot averages the central pair to produce an approximate "middle" value. |
| (2) |
There is no check that
MAXINT
is equal
to #integration points in a shell.
If MAXINT is less than the number of integration points in a shell you will be missing results; if greater the extra results will probably be junk. The true number of integration points in a shell is not written to the .PTF file, so D3PLOT cannot check this for you. |
| (3) |
There is a special case when the #integration points in a shell = 5.
If, and only if, #integration points = 5 then results are written out in the integration point order: #3, #1, #2, #4, #5. There is no obvious reason for Ansys LS-DYNA doing this, and it is not documented anywhere, but a simple shell bending test model will reveal it to be true. |
In this situation D3Plot will still permit you to select "top", "middle" and "bottom" surfaces as before (with the "middle" surface being defined as in (1) or (3) above). But it will also permit you to define a Layer number instead in the range 1 to <maxint> . An example of this is shown in SURFACE / INT Point .
If you choose this output option it is your responsibility to ensure that you interpret your results correctly.
Case 3: "Composite Ply" output with MAXINT set to some value other than the default of 3
From Version 13 onwards if the model contains composite plys then D3Plot will permit users to plot data on a surface composed of plys (see SURFACE with composite plys ). This requires composites to be set-up in PRIMER using the Composites tool, or equivalently *SHELL_COMPOSITE_LONG cards, and a .ztf file. (Composite plys created using a *PART_COMPOSITE card are not available in this feature.) To plot the data a surface composed of plys D3Plot extracts the data for each shell at the integration point the composite ply corresponds to.
To summarise the order of Ansys LS-DYNA output for Thin Shells is:
| MAXINT value | Surface output order | |||
| 3 | Always MIDDLE, BOTTOM, TOP | |||
| Anything else |
|
If a .ZTF file is present, D3Plot will know how many integration points a shell has and will therefore be able to determine the correct value to read for a selected surface, based on the rules above.
From v11.0 onwards Layer 1->Layer n is always Bottom->Top (so long as a .ZTF file is present). Prior to this 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.
|
If a .ZTF file is not present D3PLOT has no means of knowing how many integration points a given element has actually specified on its section definition; nor whether it uses Gaussian, Lobatto or user-defined rules. It is up to you to interpret your results correctly. |