Centrifugal force?

[optics_guy]

I'm trying to determine the elastic deformation of a part that is being rotated at a known angular velocity. Can this be done in Elmer? I'm not very experienced with the program yet so there may be an easy way to do this that I just haven't found yet. I would really appreciate it if someone could point me in the right direction. Thanks for any help you can provide.

[raback]

Hi

Well, as the centrifugal force is \rho*w^2*r and oriented in the radial direction you could derive MATC expressions for the body forces in style

Code: Select all

 
Stress Bodyforce 1 = Variable Coordinate 
  Real MATC "omega^2*sqrt(tx(0)^2+tx(1)^2+tx(2)^2)*nx"

where nx is the normal vector component that should be expressed also with tx=(rx ry rz). Likewise for components 2 and 3.

-Peter

[optics_guy]

I haven't tried anything with matc yet so I'll do some reading and see if I can make it work. Thanks for the reply!

[muraer]

Hi guys,

I'm also trying to simulate a spinning disk....

And I don't really get it with the centrifugal force.
I want the centrifugal force to act as a body force.

Under Model => Setup i could switch to a cylindric symmetric coordinate system. But somehow, it doesn't really work...Any Ideas how to do this?

And i don't understand the MATC-Stuff mentioned above - can someone explain this a bit deeper?

Thank you and best regards!
Mario

[muraer]

Or does anyone know how the cylindric symmetric coordinate system works?

Or how i can "access" the unity vectors?

Best regards from switzerland
Mario

[raback]

Hi

The correct form of the bodyforce was perhaps too simple so I gave some confusing guidance. The following might work assuming the axis of ratation is z-axis (i.e. 3rd coordinate in cartesian system):

Code: Select all

 
Stress Bodyforce 1 = Variable Coordinate 1
  Real MATC "omega^2*tx"
Stress Bodyforce 2 = Variable Coordinate 2
  Real MATC "omega^2*tx"

Note that cylindrical coordinate system has nothing to do here. It assumes a dimensionally reduced system where the primary coordinates are (r,z). If you're using that coordinate system then include just the first expression.

-Peter

[muraer]

Hi Peter,

Thanks a lot for the explanation!
I assume that i have to directly edit the .sif file as following?

Code: Select all

Header
  CHECK KEYWORDS Warn
  Mesh DB "." "."
  Include Path ""
  Results Directory ""
End

Simulation
  Max Output Level = 4
  Coordinate System = Cartesian
  Coordinate Mapping(3) = 1 2 3
  Simulation Type = Steady state
  Steady State Max Iterations = 1
  Output Intervals = 1
  Timestepping Method = BDF
  BDF Order = 1
  Solver Input File = case.sif
  Post File = case.ep
End

Constants
  Gravity(4) = 0 -1 0 9.82
  Stefan Boltzmann = 5.67e-08
  Permittivity of Vacuum = 8.8542e-12
  Boltzmann Constant = 1.3807e-23
  Unit Charge = 1.602e-19
End

Body 1
  Target Bodies(1) = 1
  Name = "Body 1"
  Equation = 1
  Material = 1
  Body Force = 1
End

Solver 1
  Equation = Linear elasticity
  Procedure = "StressSolve" "StressSolver"
  Variable = -dofs 3 Displacement
  Exec Solver = Always
  Stabilize = True
  Bubbles = False
  Lumped Mass Matrix = False
  Optimize Bandwidth = True
  Steady State Convergence Tolerance = 1.0e-5
  Nonlinear System Convergence Tolerance = 1.0e-8
  Nonlinear System Max Iterations = 10
  Nonlinear System Newton After Iterations = 3
  Nonlinear System Newton After Tolerance = 1.0e-3
  Nonlinear System Relaxation Factor = 1
  Linear System Solver = Iterative
  Linear System Iterative Method = GCR
  Linear System Max Iterations = 500
  Linear System Convergence Tolerance = 1.0e-8
  Linear System Preconditioning = ILU1
  Linear System ILUT Tolerance = 1.0e-3
  Linear System Abort Not Converged = False
  Linear System Residual Output = 1
  Linear System Precondition Recompute = 1
End

Equation 1
  Name = "Elasticity"
  Calculate Stresses = True
  Active Solvers(1) = 1
End

Material 1
  Name = "Steel"
  Density = 7900
  Poisson ratio = 0.3
  Youngs modulus = 100.0e9
End

Body Force 1
  Name = "BodyForce 1"
  Stress Bodyforce 1 = Variable Coordinate 1
  Real MATC "50^2*tx"
End

Body Force 2
  Name = "BodyForce 2"
  Stress Bodyforce 2 = Variable Coordinate 2
  Real MATC "50^2*tx"
End

Boundary Condition 1
  Target Boundaries(1) = 1
  Name = ""
End

Boundary Condition 2
  Target Boundaries(1) = 4
  Name = "Wall"
  Displacement 3 = 0.0
  Displacement 2 = 0.0
  Displacement 1 = 0.0
End

But somehow, this doesn't work, it just produces nonsense results... I.E. The Postprocessor (not VTK) doesn't display my body, just something crumpled...

What might be wrong?

Best regards and thanks a lot in advance!
Mario

[raback]

Hi

The two components belong to the same bodyforce:

Code: Select all

 
Body Force 1
  Stress Bodyforce 1 = Variable Coordinate 1
    Real MATC "omega^2*tx"
  Stress Bodyforce 2 = Variable Coordinate 2
    Real MATC "omega^2*tx"
End 

Other than that it's difficult to say what's wrong. You can well add this via ElmerGUI. When editing manually you'll have to abandon ElmerGUI.

-Peter

[muraer]

Aaaah, slowly, it starts to work ==> Thank you very much!!

I can't get him to add the term "variable coordinate" in the .sif file, but editing the .sif in the GUI also seems to work.

Another 2 questions: What are the Stresses 4-6 in linear elasticity for and what unit do they have? N/m^2?
And where do i find information like this? I've already plowed through all the docs but can't find it anywhere

Best regards and thanks a lot!
Mario

[raback]

Stress components are: 11, 22, 33, 12, 13, 23