Department of Engineering

IT Services


3. Elements

Q3.1 : How do I find the positive normal of a shell element?

For shells the positive normal is given by the right-hand rule going around the nodes of the element in the order they are given in the element-nodal connectivity data line (datalines which follow the keyword *ELEMENT line).

30, 101, 102, 202, 201

If using the ABAQUS/CAE click on Tools and choose Query... option and from the new form select Shell/Membrane Normals then click on the component in the viewport.
 Colour coding :   Brown - Positive   Magenta - Negative
Click on Done when finished.

If you using ABAQUS Viewer with an *.odb file then Plot Material Orientation icon in the Visualization module can be used to plot the normal. The Red line indicates the Normal direction of the shell. The local-1 direction is drawn in Cyan and the local-2 direction in Yellow.

Q3.2 : What is the difference between a shell element and a 2D solid element?

The 2D Planar elements (For example : CPE4, CPE8 - plane strain analysis and CP4, CPS8 - plane stress analysis) are only used in situations where the loading is confined to the plane of the elements. The elements only have planar variables (d.o.f) ux, uy. This means that there is no variation in the Z direction.
Shell elements are needed for out-of-plane loading. Consider a square plate subjected to a loading normal to the plane of the plate. This requires shell elements and use of plane stress/plane strain type of elements would be inappropriate under these circumstances.

Shell elements can also be used where the loading is planar but the material is made of composites. Since shell elements by definition allow for through thickness variation of material properties these are the appropriate elements to be used in these cases.

Q3.3 : How do I specify the local-1 direction for a beam in space?

See the section on Cross-section orientation in the chapter Using Beam Elements of the Getting Started with ABAQUS/Standard manual for a description of this.
There are a number of ways of specifying this. In the following figure n1 represents the local-1 direction. Consider a beam element of rectangular cross-section. Then local-1 direction is the direction parallel to the width (or base of the element).

If the beams all lie in the X-Y plane then by default the negative Z axis is taken as the local-1 direction. The following are the different methods available in specifying the local-1 direction.
  1. Specify an additional node in the element entry for the beam. If a third node is specified then the direction connecting node 1 to 3 defines the v direction in the above figure. This direction is used as an approximate n1 direction. ABAQUS then defines n2 direction as t x v. Having determined n2, ABAQUS defines the actual n1 direction as n2 x t. To summarise as long as v lies in the same plane as the t and n1 vectors no errors are introduced.
  2. Specify the approximate n1 direction on the element section option. Then ABAQUS uses the same procedure as above (method 1) to calculate the n2 direction first and then re-calculates the n1 direction again which it uses in the analysis.

If both the additional node and the n1 direction were specified as part of the section properties then the additional node takes precedence.
As mentioned earlier ABAQUS calculates the n2 direction from the t and the approximate n1 directions. There are two methods that can be used to override this.
  1. Give the components of n2 as the 4th, 5th and the 6th data values following the nodal coordinates on the data lines of the *NODE option.
  2. Use the *NORMAL option.
If both methods are used then *NORMAL takes precedence. When n2 direction is specified using one of the above methods the beam element tangent t is calculated as n1 x n2.

Q3.4 : Why do you need to specify the local-1 direction for a beam in space?

Consider a non-circular cross-section (example : rectangular section). The bending stiffness is affected by which way the width is oriented. local-1 direction fixes the orientation without any ambiguity.

Q3.5 : I am having a problem interpreting the stress output from a shell element?

If you are using the shell elements (example : S4, S8R5) then you need to be aware that the stresses are defined in local directions which in turn are dependent on the orientation of each element w.r.t the global axes.
The Shell element sign convention explains the sign convention for the local directions.

Q3.6 : How does one specify the ply directions in a flat (plane) composite shell?

Here a rectangular local co-ordinate system is defined using the *ORIENTATION statement for each of the plies. The Z axis is the normal axis to the rectangular plate. The ply directions are specified as a rotation about the normal for all 3 plies.

The rest of the data required to completely define the shell properties are given below :

The following figure illustrates a PLY direction of -30 degrees ( anti-clockwise about normal is taken as positive).

Q3.7 : How does one specify the ply directions in a cylindrical composite shell?

First of all one need to specify local cylindrical co-ordinate system because of the geometry. Figure 3.6 shows the Global co-ordinate system. The axial direction (Z') is in the direction of the Global X-axis.
*ORIENTATION, SYSTEM=CYLINDRICAL, NAME=CYLIND < xa >, < ya > , < za > , < xb >, < yb > , < zb > < normal-axis > , < rotation angle >
For the above system, this will be *ORIENTATION, SYSTEM=CYLINDRICAL, NAME=CYLIND 0, 0, 0, 1, 0, 0 1, 0
The next line indicates which of the 3 (Local) axes is normal to the cylindrical surface. This is X' (Radial) axis (which is axis 1). Then the next number is the rotation about the normal axes if re-orientation is required in specifying the material directions. Any rotation applied will be counter-clockwise
Without any rotation the other 2 axes (Y' and Z') form the local directions. Y' and Z' become the material 1 and 2 directions respectively.
Referring to Figure 3.6 The Blue (circumferential line) is the material - 1 direction. The Cyan (axial) line is the material - 2 direction.

Material directions
Let us assume that the composite is made up of 3 plies which are +10, 0 -10 degrees to the cylindrical direction.
Then the composite shell will be specified as follows :
0.05, ,	WOVEN,  10
0.05, , PLYTRON, 0
0.05, ,	PLYTRON, 0
0.05, ,	WOVEN, -45
0.05, , PLYTRON, 90
0.05, ,	PLYTRON, 0
Let us consider another situation where the zero ply direction is aligned to the axial direction. The other 2 ply directions 30 degrees either side of this direction. In this situation it is preferrable to have the material-1 direction to be the axial direction. This is done by applying an additional rotation of 90 about the normal.
0.05, ,	WOVEN,  30
0.05, , PLYTRON, 0
0.05, ,	PLYTRON, -30

Q3.8 : Is it possible to use shell elements in a 2D-Solid (Plane stress/Plane Strain) type of analysis?

No it is not possible to add 3-dimensional Shell elements to a 2D-Solid analysis.
It will be possible to choose Wire in the sketcher and draw a line which would in theory represent the Shell element. It will also be possible to create a Shell section. However when it comes to assigning the shell section to the line the shell section will not appear in the scroll down list.
Instead model the surface using Beam elements.

Q3.9 : I need to model a spring which has a different stiffness in compression to that in tension. How do I do it?

Element defnition for the spring element :
*Element, type=Spring2, elset=Springs/Dashpots-1-spring
1, Bay1GroundFloor.5, Part-2-1.1
2, Bay1GroundFloor.7, Part-2-1.4
3, Bay1GroundFloor.8, Part-2-1.6
4, Bay1GroundFloor.3, Part-2-1.2
The spring stiffness is
*Spring, elset=Springs/Dashpots-1-spring
2, 2
** spring stiffness
By adding the nonlinear one could then define Spring behaviour which is different for compression and tension.
*Spring, elset=Springs/Dashpots-1-spring, nonlinear
2, 2
** Force1, Rel. Displacement-1
** Force2, Rel. Displacemnet-2
10.E8,  -0.1
10.E6,  -0.001
    0,   0
7.8E+06, 1.0

Q3.10 : I need to change the order (degree) of the elements I am using in a mesh How do I do this?

In the Mesh module click on the Element Type icon. In the dialog box which appears choose the element order you require (from the available list : Linear, Quadratic)
If using the quadratic (2D) and Hex elements (3D) choose Incompatible Mode elements if using the lower order elements.
© Cambridge University Engineering Dept
Information provided by abaqus-support
Last updated: 18 December 2011