ANSYS - Static Structural Analysis

How ANSYS solves a Linear Static Structural Analysis

-always solves the following matrix: [K]{x} = (F)

Assumptions:

[K] is constant

• linear elastic material behavior is assumed
• small deflection theory is used
• some non-linear boundary conditions may be included

(F) is Statically applied

• no time-varying forces are considered
• no inertial effects (mass, damping) are included

These assumptions are only held for linear static analysis, and are not true with a non linear static analysis or a dynamic analysis

NOTE: for all geometry, need to specify a material and material properties (if none specified, ANSYS will just default to whatever it has set in the program as the default, depending on what material your using, you will need to set it up in the "Engineering Data" application

• you will always need at the very least Young's Modulus and Poisson's ratio
• mass density is required if any inertial loads are present
• thermal expansion coefficient is needed if a temperature load is applied (thermal conductivity not needed)
• Stress Limits are needed if using any of the stress tools
• Fatigue Properties are needed if using any fatigue tools

In ANSYS there are different Types of contacts

• bonded implies that the 2 surfaces are part of the same piece (what all of chassis members should be set to when connected to one another)
• No seperation is for when you have seperate and distinct parts that arent allowed to not be in contact with eachother, but they can slide along eachother
• The others are all non-linear, and we aren't really dealing with them

There is also a function called "Spot Welds" which allows you to define a connection at discrete points when you're connecting shell assemblies (Usually set up before hand in your CAD software) we won't be using this for our simulation

Bellow is a summary of the contact types that can be used with your different body elements

Loads and Supports

ANSYS has both loads (the things we can use to model how the car will be impacted) and supports (restrictions to how the model can move, so that we prevent the car from flying off into space)

All loads and supports are represented in terms of degrees of freedom. In solids, they can be applied/move in X, Y, Z translations, and shells can also have rotations about X, Y, and/or Z.

ANSYS can model the following Loads Types:

Inertial

• These loads act on the entire system.
• Density is required for mass calculations.
• These are only loads which act on defined Point Masses.

Structural loads

• Forces or moments acting on parts of the system.

Structural supports (probably won't be using)

• Constraints that prevent movement on certain regions.

Thermal Loads (which we won't be using)

• The thermal loads which result in a temperature field causing thermal expansion/contraction in the model.

With all your loads, you can specify the directions that they are applied in.

Acceleration

• Acts on entire model in length/time2 units.
• Acceleration can be defined by Components or Vector.
• Body will move in the opposite direction of the applied acceleration.

Standard Earth Gravity

• Value applied coincides with selected unit system.
• Standard Earth Gravity direction is defined along one of three global or local coordinate system axes.
• Body will move in the same direction of the applied gravity.

Rotational Velocity

• Entire model rotates about an axis at a given rate.
• Define by vector or component method.
• Input can be in radians per second (default) or RPM.

Pressure Loading

• Applied to surfaces, acts normal to the surface.
• Positive value into surface, negative value acts out of surface.
• Units of pressure are in force per area.

Force Loading

• Forces can be applied on vertices, edges, or surfaces.
• The force will be evenly distributed on all entities. Units are mass*length/time2.
• Force can be defined via vector or component methods.

Hydrostatic Pressure

• Applies a linearly varying load to a surface (solid or shell) to mimic fluid force acting on the structure.

• Fluid may be contained or external.

  • User specifies:

    • Magnitude and direction of acceleration.

    • Fluid Density.

    • Coordinate system representing the free surface of the fluid.

    • For Shells, a Top/Bottom face option is provided.

Bearing Load

• Force component distributed on compressive side using projected area.

  • Axial components are not allowed.

  • Use only one bearing load per cylindrical surface.

    • If the cylindrical surface is split be sure to select both halves of cylindrical surface when applying this load.

• Bearing load can be defined via vector or component method

Moment Loading

• For solid bodies moments can be applied on a surface only.
• If multiple surfaces are selected, the moment load is evenly distributed.
• Vector or component method can be employed using the right hand rule.
• For surface bodies a moment can be applied to a vertex, edge or surface.
• Units of moment are in Force*length.

Remote Loading

Bolt Pretension

Line Pressure Loading