How to simulate rising levels of water over time in FEA

In a time based analysis (MES) Hydrostatic pressure is a straight forward load you can apply to any surface within Simulation Mechanical. All you have to do is to;

• pick a surface,
• define the direction of gravity (which will increase the pressure load linearly in that direction) and
• enter the fluid density

But what if you wanted to simulate effects of increase in the amount of water over time?  

Think of heavy rains over a short period of time and its effects on a dam gate like the one shown here.

Hydrostatic pressure load definition does not give you the option to change the water level over time. 

No need to panic J

Instead of increasing the water level, you can simply use prescribed displacements to move the object deeper and deeper in to the water which will increase the pressure acting on the surface.

To accomplish this I recommend creating 2 load curves:

• The 1^st one will be ramp up style and it will control the motion.
• The 2^nd one will be a steady load curve and it will control the hydro static pressure.
• Make sure the hydrostatic pressure you have applied has the “follows displacement” option enabled. 

When you run the simulation you will see that the deformations will increase as your design dips deeper in to the water which represents rising water levels. 

The video on the right shows the increase in stress levels as the pressure builds up

How and When to Take Advantage of Symmetry and Antisymmetry

When creating a model for finite element analysis, natural lines of symmetry and antisymmetry can allow you to analyze a structure or system by modeling only a portion of it. This technique can reduce the size of the model (the total number of nodes and elements), which can reduce the analysis run time as well as the demands on computer resources.

Symmetry

Symmetry means a model is identical on either side of a dividing line or plane (see Figures 1-3). Along the line or plane of symmetry, boundary conditions must be applied to represent the symmetrical part as follows:

• Out-of-plane displacement = 0
• The two in-plane rotations = 0

Figure 1: Model with a Line of Symmetry

Figure 2: Model with a Plane of Symmetry

Figure 3: Example of Symmetry for Plate Elements

Antisymmetry

Antisymmetry means the loading of a model is oppositely balanced on either side of a dividing line or plane (see Figures 4-5). Boundary conditions must be applied along the line of symmetry as follows:

• Out-of-plane rotation = 0
• The two in-plane displacements = 0

Figure 4: Antisymmetrical Model

Figure 5: Example of Antisymmetry for Plate Elements

Figure 6 shows an example of how to specify an antisymmetrical boundary condition in Autodesk Simulation Mechanical software.

Figure 6: Defining an Antisymmetrical Boundary Condition

Required Conditions

To take advantage of the symmetrical modeling technique, the following conditions for symmetry (or antisymmetry) must exist:

• the geometry, material properties and boundary conditions are symmetric; and
• the loading is symmetric or antisymmetric.

Then, you can build a model of the symmetrical portion (half, quarter, eighth, etc.) and apply the appropriate boundary conditions.

Advantages of a symmetrical/antisymmetrical model include the following:

• Analyzing a symmetrical portion of a structure means faster processing than if you modeled the whole structure.
• You can often increase the mesh density of the symmetrical model for greater accuracy and still have fewer elements than if you modeled the whole structure.
• You can compare the results of a symmetrical model to those of a full model to confirm the validity

How to sum reaction forces

The summation of reaction forces in a model is often used to verify input loading, validate model behavior or determine floor load distributions. In the Results environment, the "Inquire: Results" dialog can be used to sum the reaction forces of selected nodes.

Another typical application of summing reaction forces is to determine the total force of a pressure load when the area of pressure is unknown and cannot be readily calculated. As shown in Figure 1, the cutting frame has a pressure load applied to two surfaces of unknown area and is fully constrained at the bottom of each of the four legs. The total force of the pressure can be calculated by summing the vertical reactions of all of the constrained nodes.

Figure 1: Note the locations of the pressure loads and constraints in this display of the vertical reaction forces in the cutting frame.

To sum the reaction forces in the Results environment for a Static Stress Analysis:

• Select and display the desired reaction (X, Y or Z) using the "Results Contours” tab,  “Other Results” panel, “Reactions” pull-down menu “Reaction Force (Negative) ” pull-out menu;
• Select the nodes that will be used in the summation;
• Right click anywhere in the working area;
• In the pop-up menu that appears, select "Inquire Results"; and
• In the "Inquire: Results" dialog (Figure 2), click on the "Summary" pull-down menu and select "Sum".

Figure 2: The "Inquire: Results" dialog displays information about the selected nodes and the calculated "Summary" value.

The summary of the reaction forces of all selected nodes will now be displayed in the "Inquire: Results" dialog. If desired, the area could be calculated since the pressure and force values are now known.

Understanding Degrees of Freedom

For finite element analysis (FEA) users, it's important to keep in mind that some types of elements might not transmit all types of loads through their nodes. For example, two structural beam elements connected together behave like a fully welded connection because the beam elements will transmit three forces (axial and two shears) and three moments (torsion and two bending). However, a beam element connected to a truss element behaves like a pinned joint because the truss element can only transmit axial forces. The concept of what forces are transmitted and consequently what loads and restraints can be applied is known as degree of freedom (DOF).

The DOF is important to understand in determining how loads can be applied, how boundary conditions restrain the model and how different element types need to be connected together. A translational DOF indicates that forces are transmitted through the nodes and a rotational DOF indicates that moments are transmitted through the nodes.

For example, two-dimensional (2-D) elements only have translational DOFs. Thus, you cannot apply a nodal moment to a 2-D element; mathematically, the element cannot react to the moment.

Figure 1: 2D Elements (Triangular)		Figure 2: 2D Elements (Quadrilateral)

In addition, a "fully fixed" boundary condition cannot provide a moment restraint to a brick element because brick elements only have translational DOFs.

Figure 3: Brick Elements (8 noded)

Finally, the beam to truss element connections could be unstable because the truss element will not prevent the beam element from rotating; if the other end of the beam is free to translate, then the connection behaves like a ball joint.

Figure 4: Beam Element to Truss Element connection

The last two examples may result in model stability messages (such as "model not tied down enough") during a linear static stress analysis.

Table 1: DOFs for common structural element types.

Element	Degrees of Freedom
Truss	translation in X, Y, Z
Beam	translation in X, Y, Z; rotation in X, Y, Z
2-D	translation in Y, Z
Brick	translation in X, Y, Z
Plate	translation in X, Y, Z; Two in-plane rotation DOFs (The out-of-plane rotational DOF is not considered for plate elements)

Note: This is a small subset of the available element types in Autodesk Simulation Mechanical software, see the User's Guide for a full list.

How to define surface contact in 2D analyses

For linear static stress analysis of two-dimensional (2-D) assembly models that are created using Autodesk Simulation’s sketching, modeling and meshing capabilities, you can conveniently and quickly define contact between parts. To do so, use the following general method:

1. Sketch the 2-D parts (the parts must share at least one identical-length, coincident edge).
2. Select the sketches in the tree view and click on the “Generate 2D Mesh” button within the “Mesh” panel under the “Mesh” tab (see Figure 1). The "2-D Mesh Generation" dialog will appear.

Figure 1: In the tree view, select the sketches that share a coincident edge and then click “Generate 2D Mesh” to access the "2D Mesh Generation" command.

3. Adjust the mesh settings as necessary and press “Apply” to generate the mesh.
4. In the model display, select the coincident surfaces and right click. In the pop-up menu, choose "Contact" and then specify the type of contact from five applicable options (see Figure 2):
• Bonded - The nodes on the two edges will be matched and will be in perfect contact throughout the analysis. When a node on one edge deflects, the node on the adjoining edge will deflect the same amount in the same direction. This is the default option.
• Free/No Contact - The nodes on the two edges will not be matched and will be free to move relative to each other.
• Surface Contact - The nodes on the two edges will be matched and will be free to move away from each other. If the nodes move toward each other, a stiffness will be applied to resist this movement.

o   Sliding/No Separation – Bonds contact faces in normal to face direction while sliding under deformation.

o   Separation/No Sliding – Separates contact faces partially or fully without them sliding against each other.

Note that Edge Contact and Welded Contact are not applicable to 2D elements.

Figure 2: Once the mesh is generated, you can select and right click on the coincident surfaces and specify the type of contact.

4. After defining the type of contact, the contact surfaces will be listed in the tree view.
5. In the tree view, right click on the contact pair and choose "Settings..." (see Figure 3).

Figure 3: Right click on the contact pair in the tree view and choose "Settings...".

6. In the "Contact Options" dialog, you can specify the coefficient of friction for the contact pair (see Figure 4).

Figure 4: Choose whether or not to include friction in the analysis and specify the static friction coefficient.

7. Set up for linear static stress analysis (define element information, material properties, loadings and constraints) and run the analysis.
8. In the Results environment, you can inquire on the total contact force for each contact pair in the model. Right click on the heading for the contact pair in the tree view and choose the "Contact Force..." command (see Figure 5).

Figure 5: In Results environment, you can inquire on the total contact force. A "Total Contact Force" dialog will appear with the total contact force for that pair.

Thus, the ability to quickly and easily define 2-D contact helps you to perform linear static stress analysis of 2-D assembly models that were created with Autodesk Simulation’s sketching, modeling and meshing tools.

Useful Links

With the release of Autodesk Knowledge Network (AKN) some of the website you are looking for may have moved around a little. So here are some of the links I find useful

1) Autodesk Simulation Mechanical Accuracy Verification: Link

2) How to install Simulation Mechanical Help locally?  Link

3) How do I download the latest Service Pack for Simulation Mechanical?  Link

4) SIMTV: Link

-Sualp