You are here
Convergence test in ANSYS
Hi, i tried to solve a simple plane stress cantilever problem using ansys but it did not converged to the exact value and it goes beyond the exact value for stress and diplacment domain as i go on making finer mesh. the problem is as shown below, i tried 4 noded solid plane82 and 8 noded plane 182 element type. Can anybody tell me the procedure for convergence test in ansys
»
- gohelvivek's blog
- Log in or register to post comments
- 13449 reads
Comments
possible answer to problem
Hello,
In your picture of the cantilever beam you show that it is fixed at the left support. The exact solution from elasticity is not exactly fixed, so if you simply used pinned supports at the nodes at the left edge, that will not give the correct results.
Instead, in your model you must impose the elasticity displacement solution at the left boundary nodes so that your model will converge to the elasticity solution. If you look in the paper by Belytschko et al.
T. Belytschko, Y. Krongauz, D. Organ, M. Fleming, and P. Krysl. Meshless methods:
An overview and recent developments. Computer Methods in Applied Mechanics and
Engineering, 139:3–47, 1996.
you will see that they provide the elasticity solution in a nice form. That is what you must use. Or you may look in Appendix D of my dissertation p. 146 for the elasticity solution (http://people.wallawalla.edu/~louie.yaw/PhD_Dissertation/yawUCD.pdf)
Maybe that will fix the difficulties you are having with convergence.
regards,
Louie
Convergengce in ansys
Hello Louie,
Thank you, for your support.
I have used fixed support on left side and that i have done with ANSYS by making displacement in ux and uy direction 0. is it right?
Constraints in Ansys
Hi,
If you want the results to match with simple canilever equation, try to fix UX for all nodes, but fix UY only at one centralnode. The idea is not to constrain the deformations due to Poisson effect. When using 3D, you will have to think in the same line, to find proper nodal constraints.
Hope it helps... Regards,
Jayadeep
If you are trying to match
If you are trying to match the elasticity solution, it is INCORRECT to make all ux and uy values zero at the fixed support.
You must impose the displacement solution values on the nodes at the support. The elasticity solution has values for ux and uy as a function of load and position on the cantilever beam. If you use the elasticity solution and put in the coordinates of the support nodes you can calculate the prescribed ux and uy values that you should impose on the nodes. See my post above which directs you to the elasticity solution.
This is at least one thing you should do to fix your problem. It is uncertain if you have errors besides this one that I have mentioned.
regards,
Louie
do not fix all nodes in ux direction
It is incorrect to fix all nodes at the support in the ux direction if you wish to match the elasticity solution.
You should use the elasticity solution for the displacements, then impose these displacements at the support nodes.