User login

Navigation

You are here

Details About "NLGEOM"Command in ANSYS

I am developing an FEA code for a viscoelastic contact analysis. Right now the formulation is assuming small deformations. After deformation I am getting the volume of the body to be less than the original. I want to preserve the volume. ANSYS gives exact results as my code by carrying a normal contact analysis.

 But if I include the "NLGEOM ON" for the same problem in ANSYS, I get a different result and the volume is conserved in this case. Can anyone please tell me what formulation does ANSYS use mathematically When the "NLGEOM" flag is turned on? If I know that, I can modify my code accordingly to conserve the volume.

I tried including the deformation gradient to convert the integration to the current domain and tried using the current strain and shape function derivatives (4 node quad element), but in vain.

It would be really helpful if someone is able to guide me on this.

It uses a Hencky or logarithmic strain measure, which is ln(U), where U is the right stretch matrix obtained by polar decomposition of the deformation gradient. For calculating Hencky strain, it uses the eigen values and eigen vectors of U. You can read more in ANSYS theory manual, there is a chapter on structural nonlinearity.

 

Chandra Veer Singh

Chandra,

Thanks for the reply.

I couldn't find the technical details in the ANSYS help menu. By theory manual do you mean the 'help' section or it is something different? Please let me know.

 

Thanks once again.

Shriram 

The NLGEOM command activates corrections for large rigid body rotations and translations when a small strain constitutive relation is used.   It is also activated for large strain material models.  For details on the implementation you can go to Chapter 3. Structures with Geometric Nonlinearities of the ANSYS Theory Manual.

Using NLGEOM should have no impact on whether the incompressibility condition is satisfied.  Incompressibility is usually satisfied using a Lagrange multiplier approach which can lead only to approximate satisfaction of incompressibility in a numerical code.  However, there are are stress update algorithms that satisfy incompressibility exactly, often by using an exponential map - see Weber and Anand, 1988 (or so).

A cut/paste job from the ANSYS manual follows.

 

-- Biswajit 

3.3. Large Rotation

If the rotations are large but the mechanical strains (those that cause stresses) are small, then a large rotation procedure can be used. A large rotation analysis is performed in a static (ANTYPE,STATIC) or transient (ANTYPE,TRANS) analysis while flagging large deformations (NLGEOM,ON) when the appropriate element type is used. Note that all large strain elements also support this capability, since both options account for the large rotations and for small strains, the logarithmic strain measure and the engineering strain measure coincide.

3.3.1. Theory

Large Strain presented the theory for general motion of a material point. Large rotation theory follows a similar development, except that the logarithmic strain measure ((Equation 3–6)) is replaced by the Biot, or small (engineering) strain measure: (3–37)where: [U] = stretch matrix [I] = 3 x 3 identity matrix 3.3.2.

Implementation

A corotational (or convected coordinate) approach is used in solving large rotation/small strain problems (Rankin and Brogan(66)). "Corotational" may be thought of as "rotated with". The nonlinearities are contained in the strain-displacement relationship which for this algorithm takes on the special form:(3–38)where: [Bv] = usual small strain-displacement relationship in the original (virgin) element coordinate system [Tn] = orthogonal transformation relating the original element coordinates to the convected (or rotated) element coordinates

The convected element coordinate frame differs from the original element coordinate frame by the amount of rigid body rotation. Hence [Tn] is computed by separating the rigid body rotation from the total deformation {un} using the polar decomposition theorem, (Equation 3–5). From (Equation 3–38), the element tangent stiffness matrix has the form: (3–39)and the element restoring force is: (3–40)where the elastic strain is computed from: (3–41) is the element deformation which causes straining as described in a subsequent subsection.

The large rotation process can be summarized as a three step process for each element:

Determine the updated transformation matrix [Tn] for the element.

Extract the deformational displacement  from the total element displacement {un} for computing the stresses as well as the restoring force  .

After the rotational increments in {Δu} are computed, update the node rotations appropriately.

All three steps require the concept of a rotational pseudovector in order to be efficiently implemented (Rankin and Brogan(66), Argyris(67)).

Biswajit,

Thanks for the reply.

If I consider a small problem; a square as an axisymmetric model (giving rise to a cylinder in 3D). The material model is viscoelastic. If I have a line on the top surface and bottom surface and press the top surface to about half the height with the lower surface fixed (contact analysis, no friction) I get a deformed rectangle. I do the same with ANSYS and with my FEA code in FORTRAN. What happens is:

Without NLGEOM ON, I get an exact match with my code and ANSYS, but the volume is not conserved.

With NLGEON ON, I get a slightly larger rectangle and the volume is conserved in ANSYS in this case.

I want to conserve the volume in my FEA code also, and hence I am trying to understand what modification do I need to do in my FEA code? My FEA code follows Newton Raphson Method and the same algorithm as ANSYS for viscoelastic stress calculations. I am stuck in my research because of this. Please guide me with whatever you know.

 

Thanks,

Shriram

Research Assistant
Structural and Multidisciplinary Optimization Lab.

University of Florida

Subscribe to Comments for "Details About "NLGEOM"Command in ANSYS"

Recent comments

More comments

Syndicate

Subscribe to Syndicate