ANSYS - Static Structural Analysis

Owned by Joshua White (Unlicensed)
Last updated: Nov 24, 2018

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

Geometry

A structural Analysis can simulate any kind of body element

Examples:

Solid Body: the body has both a surface are and a volume

Surface Body: body has a surface area, but no volume

Line body: body consisting of edges, no surface are or volume (

Planar: a surface body that only exists in a 2D place (only really used in 2D analysis)

Winding bodies: a body made only of line bodies (made to represent things like coils of wires)

Note: for surface bodies, you need to define a thickness for them Which can be done by entering a value in the "details view of the Geometry branch



Point mass:

Used to model parts that you may not have necessarily modeled.

  • can only be associated with surfaces
  • can be defined by entering X,Y,Z coordinates or
  • selecting other geometry to define its location
  • Point mass is affected by Acceleration, gravity, and rotational velocity
  • point masses ignore any other loads that you apply to your mode

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


Assemblies

Contact Regions

When importing assemblies of solid parts, contact regions are automatically created between the solid bodies.

  • Contact allows non-matching meshes at boundaries between solid parts
  • Tolerance controls under “Contact”branch allows the user to specify distance of auto contact detection via slider bar
  • when a contact is made, ANSYS will assume one surface is the "contact" and the other the "target"
  • A contact surface cannot penetrate through the target surface, but a target surface can penetrate through the contact surface
  • ANSYS defaults to setting up symmetric contacts meaning the two surfaces are both the contact and target (i.e. neither can penetrate the other)

Note: Although ANSYS defines contact regions automatically, some times it has problems when you have complex geometry. In MSXII, we a few weird contact regions were made when we imported our model, which prevented us from being able to solve it. As such, just review all of your contact regions to make sure ANSYS didn't do anything to weird

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

Analysis Settings

The “Analysis Settings”details provide general control over the solution process:

  • Step Controls:
    • manual and auto time stepping controls
    • specify the number of steps in an analysis and an end "time" for each step
    • "time" is just the tracking mechanism they use to know what "step" they're at in a simulation.
  • Solver controls
    • two solvers available
      • direct solver
      • iterative solver
    • weak springs
      • simulation tries to anticipate under-constrained models

We won't be playing around too much with the analysis settings, at most we may play around with changing the "step controls" so we can get a better picture of how the model reacts over a period of time and how things propogate throughout the model, but we won't really be doing anything too fancy.

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

Supports in ANSYS

Fixed Support

  • -constrains all degrees of freedom on vertex, edge or surface
    • Solid bodies: constrains x, y, z
    • Surface and line bodies: constrains x, y, z, rotx, roty, rotz


Given Displacement

  • Applies known displacement on vertex, edge or surface
  • allows for imposed transnational displacement in x, y, z (in user defined coordinate system)
  • Entering "0" means that the direction is constrained (i.e. not free to move in that direction). Leaving the direction blank means the the component is able to move freely in that direction.
  • we may use this type of support when the geometry for the suspension is more well defined.

Elastic Support

  • Allows faces/edges to deform according to a spring behavior
  • Foundation stiffness is the pressure required to produce unit normal deflection of the foundation.

Friction-less Support

  • applies constraints (fixes) in normal direction on surfaces
  • for solid bodies, this support can be used to apply a "symmetry" boundary
    • in our case we can use this to section the car in half to simplify the simulation.

Cylindrical Support

  • provides individual control for axial, radial or tangential constraints
  • applied on cylindrical surfaces

Compression Only Support

  • applies a constraint in the normal compressive direction only
  • can be used on a cylindrical surface to model a pin, bolt, etc.
  • requires an iterative (nonlinear) solution
  • we most likely won't be using this kind of support

Simply Supported

  • can be applied on an edge or vertex of surface/line bodies
  • prevents all translations, but all rotations are free

Fixed Rotation

  • can be applied on surface, edge, or vertex of surface or line bodies
  • constrains rotations but translations are free

Results

ANSYS can solve and show you different structural Results

Plotting Results

contour and vector plots are usually shown on the deformed geometry

use the context toolbar to change settings


Deformation

The deformation of the model can be plotted. In ansys total deformation is plotted as a scalar quantity

Utotal = sqrt(Ux^2 + Uy^2 + Uz^2)

Where Ux,y,z are the deformations of an element in each respective direction

The x, y, z, components of deformation can be shown under "Directional" in either global or local coordinate systems

Vector plots of deformation are also available to be shown (we won't really be using this)


Stresses and Strains

Stresses and (elastic) strains have six components (x, y, z, xy, yz, xz)

for stresses and strains, components can be requested under normal (x, y, z) and shear (xy, yz, xz)

principle stresses can also be shown and are always arranged such that s1 > s2 > s3

where s1 is the principal stress in direction 1 s2 is the principal stress in direction 2 and s3 is the principal stress in direction 3.

-we don't really need to know which direction is which in terms of x,y,z, we care more about just knowing the value so we can see if the component will fail or not. If we want to see how it deforms or is impacted we can simply just look at the contour plots

-Stress/strain intensity is defined as the absolute maximum of the following values

-- s1-s2, s2 - s3, or s3-s1

Safety Factors

Safety factors can be chosen from 4 different failure theories

Ductile theories: 

  -maximum equivalent stress

  -maximum shear stress

Brittle Theories

  -mohr-coloumb stress

  -maximum tensile stress


For us we are assuming a ductile material and will be using the ductile theories, in most cases we will be using maximum equivalent stress

Within each stress tool, safety factor, safety margin and stress ratio can be plotted


Ansys also supports user defined results, however we will not be using this for midnight sun.


For more detailed of things please read over the following Power point

WB-Mech_120_Ch04_Static.pdf