4.19 PLATE NO.19 WITH 16 NODES

This is a curvilinear Lagrange- Reissner- Mindlin plate element with cubic shape functions. The transformation is isoparametric. The integration is carried out numerically in both axises according to Gauss- Legendre. Consequently, the integration order can be selected in Z88I1.TXT in the material information lines. The order 4 (= 4 x 4 points) is very good. This element calculates both displacements and stresses very precisely. The input amount is heavy, you should use the mesher Z88N.

The integration order can be chosen again for the stress calculation. The stresses are calculated in the corner nodes (good for an overview) or calculated in the Gauss points (substantially more exactly). Area loads are defined in the appropriate material lines, file Z88I1.TXT, instead of Second moment of inertia RIYY. For this element you need to set the plate flag IPFLAG to 1. Attention: In contrary to the usual rules of the classic mechanics Z88 defines ThetaX the rotation around the X- axis and ThetaY the rotation around the Y- axis.

Mesh generation with Z88N: Use plates No.20 for super elements, resulting in finite elements of type 19 (plates No.20 may generated by AutoCAD or Pro/ENGINEER, ref. the chapters of Z88X and Z88G). A bit tricky, but works quite fine.

For example, some lines from a mesh generator input file Z88NI.TXT:
.....
5 20 super element 5 of type 20
20 25 27 22 24 26 28 21
.....
5 19 generate from super element 5 (which is of type 20 is, see above) finite elements of type 19
3 E 3 E .. and subdivide them threetimes equidistant in X-direction and threetimes equidistant in Y- direction

Input:

CAD : 1-2-3-4-5-6-7-8-9-10-11-12-13-14-15-16-1 , ref. chap. 2.7.2. Usually, you will not work in this way. It's much more easier to build within a CAD program a super elements mesh with 8- node plates No.20. Export this mesh as a DXF file and use Z88X to produce a mesh generator input file Z88NI.TXT. Run the mesher Z88N and generate a finite elements mesh with plates No.19. Plot this mesh using Z88P, read off the appropriate node numbers and edit the boundary conditions file Z88I2.TXT.

Z88I1.TXT
> KFLAG for cartesian (0) or cylindrical coordinates (1)
> set plate flag IPFLAG to 1 (or 2, if you want to reduce the shear influence)
> set surface and pressure loads flag IQFLAG to 0 for your convenience. Then the entry of the pressure is done via the "Second moment of inertia RIYY", see below. If IQFLAG is set to 1, then the entry of the pressure is done via the surface and pressure loads file Z88I5.TXT
> 3 degrees of freedom for each node (w, ThetaX, ThetaY )
> Element type is 19
> 16 nodes per element
> Cross-section parameter QPARA is the element thickness
> "Second moment of inertia RIYY" is the area load
> Integration order INTORD per each mat info line. 4 is usually good.

Z88I3.TXT
> Integration order INTORD: Basically, it is a good idea to use the same value as chosen in Z88I1.TXT , but different values are permitted
0 = Calculation of the stresses in the corner nodes
1, 2, 3, 4 = Calculation of the stresses in the Gauss points

> KFLAG has no meaning

> Reduced stress flag ISFLAG:
0 = no calculation of reduced stresses
1 = von Mises stresses in the Gauss points ( INTORD not 0 !)
2 = principal stresses in the Gauss points (INTORD not 0!)
3 = Tresca stresses in the Gauss points (INTORD not 0!)

Z88I5.TXT

This file is optional and normally not used here because it is much more convenient to enter the pressure data for the plate elements into Z88I1.TXT in the section material informations. However, the possibility for entering the pressure loads by the surface and pressure loads file Z88I5.TXT, too, is implemented for universal use of this file. Then set IQFLAG to 1 and proceed as follows:

> Element number with pressure load

> Pressure, positive if poiting towards the edge

Results:

Displacements in Z (i.e. w) and rotations ThetaX around X- axis and ThetaY around the Y- axis.
Stresses: The stresses are calculated in the corner nodes or Gauss points and printed along with their locations. The following results will be presented:

- plate bending moments Mxx and Myy (unit: force x lenght / length)
- plate torsion moments Mxy = Myx (unit: force x length / length)
- the shear forces Qyz and Qzx (unit: force / length)
- the true stresses resulting from plate bending moments and plate torsion moments

Optional von Mises stresses
Nodal forces in X and Y for each element and each node.