July 25, 2023 at 5:02 pmPirelli93Subscriber
I would like to know what is the precise theory/formulation behind the enhanced assumed strain method for 8-noded hexahedral element that Ansys Mechanical uses. More precisely SOLID185 element with KEYOPT(2)=2 and KEYOPT(6)=0.
In the Ansys Mechanical Theory Reference manual it is mentioned that: "SOLID185 with KEYOPT(2)=2 or 3 the enhanced strain formulations from the work of Simo and Rifai( (p. 935)),Simo and Armero( (p. 935)), Simo et al.( (p. 935)), Andelfinger and Ramm( (p. 935)), and Nagtegaal and Fox( (p. 935)) are used. It introduces 13 internal degrees of freedom to prevent shear and volumetric locking for KEYOPT(2) = 2, and 9 degrees of freedom to prevent shear locking only for KEYOPT(2) = 3. If mixed u-P formulation is employed with the enhanced strain formulations, only 9 degrees of freedom for overcoming shear locking are activated."
I have found the correct theory for the "Simplified" Enhanced Assumed Strain formulation for SOLID185 with KEYOPT(2)=3 and KEYOPT(6)=0 from Andelfinger's paper or at least this calculated indentical results.
In the theory of Simo et al.( it is mentioned that the Simo's modified EAS formulation needs special 9-point quadrature rule (instead of the traditional 8-point 2x2x2 Gaussian quadrature rule) for the numerical integration. Does the SOLID185 with KEYOPT(2)=2 and KEYOPT(6)=0 use the identical approach ?
So the question is that from which paper or where could I find the correct theory/formulation for the SOLID185 with KEYOPT(2)=2 and KEYOPT(6)=0 ?
July 27, 2023 at 5:49 pmJohn DoyleAnsys Employee
There are two sets of terms added for Enhanced Strain when it is invoked for SOLID185 via KEYO(2)=2. – one set addresses shear locking (with 9 internal DOF) and another set addresses volumetric locking (with 4 internal DOF), if mixed u-P formulation is inactive, via KEYO(6)=0. However, if mixed u-P is activated, via KEYO(6)=1, the volumetric locking terms of Enhanced Strain are not added.
Simplified Enhanced Strain (KEYO(2)=3) adds the same shear locking terms as Enhanced Strain. However, Simplified Enhanced Strain never includes terms for volumetric locking, even when mixed u-P is inactive (KEYO(6)=0).
Enhanced Strain and Simplified Enhanced Strain are identical when mixed u-P is invoked, via KEYO(6)=1.
July 28, 2023 at 12:43 pmPirelli93Subscriber
Thank you for your reply !
I understand the difference between mixed u-P and pure displacement formulations when enhanced assumed strain method is used. I know how to implement/use these different formulations in Ansys Mechanical, but I want to know what is the specific theory behind the Enhanced Assumed Strain method, SOLID185 with KEYO(2)=2 and KEYO(6)=0. From which paper or book I can find this spesific theory ?
The thing is that I have calculation “code” snippet in symbolic math software and I’m able to get identical results with Ansys for the Simplified Enhanced Assumed Strain (KEYO(2)=3 and KEYO(6)=0) with the method described in Andelfinger and Ramm( paper, but I can’t get identical results for Enhanced Assumed Strain method (KEYO(2)=2 and KEYO(6)=0), because I don’t know what specific EAS- version or theory it uses.
1. When SOLID185 is used with KEYO(2)=2 and KEYO(6)=0, is the special 9-point (2x2x2 + 1) or 27-point (3x3x3) or standard 8-point (2x2x2) Gaussian quadrature used for calculating stiffness matrix ?
2. Is the transformation matrix T_0 (6×6 matrix, used for the enhanced interpolation matrix M_xi) the same as in Simplified Assumed Strain method ?
3. What is the enhanced interpolation matrix M_xi for the Enhanced Assumed Strain ? I haven’t found M_xi matrix where is 9+4 enhanced parameters. I have only found 9+3 version and additionally Andelfinger and Ramm( paper’s possible choices for M_xi: 9 (EAS-9), 9+6 (EAS-15), 9+12 (EAS-21), 9+21 (EAS-30).
4. There are also many different versions for calculting the gradients / “B-matrices”. For example calculate gradients in the element centroid, calculate the average of the gradients, use and multiply the relation of jacobian determinants det(J(0,0,0))/det(J(xi,eta,zeta)), etc… These different versions are for the enhanced assumed strain element to pass the patch test and for example to take account effects of initially distorted elements.
August 10, 2023 at 3:29 pmPirelli93Subscriber
I have tried with the following enhanced interpolation matrix (9+3):
This gives indentical results with SOLID185, (KEYO(2)=2 and KEYO(6)=0) when the hexahedral is perfect cube and traditional 2x2x2 Gaussian quadrature rule is used and same 6×6 transformation matrix T_0 is used than in Andelfinger and Ramm( paper.
However when the hexahedral element is initially parallelepiped or arbitrarily distorted there is difference between the results so this enhanced interpolation matrix M_xi is not correct one.
I also tried this 9+4 version of the enhanced interpolation matrix, but it gives almost identical results with the above one:
I have read many PhD theses and scientific publications about these EAS methods, but I haven’t yet found the 9+4 version for the enhanced interpolation matrix which is mentioned in the Ansys Theory manual.
Could someone explain or show what is the correct form for the matrix and are there other aspects to consider ? This isn’t explained in the Ansys Theory Manual clearly.
- You must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- Solver Pivot Warning in Beam Element Model
- Saving & sharing of Working project files in .wbpz format
- Understanding Force Convergence Solution Output
- User manual
- An Unknown error occurred during solution. Check the Solver Output…..
- What is the difference between bonded contact region and fixed joint
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- whether have the difference between using contact and target bodies
- Defining rigid body and contact
- Colors and Mesh Display
© 2023 Copyright ANSYS, Inc. All rights reserved.