When inspecting the stiffness matrix of a simple cantilever beam, modelled in ABAQUS, it becomes apparent that the fixed-end boundary conditions are applied by assigning very large (O(1036)) stiffness terms to the DoF of the first node. However, this renders the stiffness matrix, K very ill-conditioned. Using an incomplete Cholesky preconditioner with threshold dropping gives some improvement, but the inversion condition number of K is still on the order of several billion. Is this how FEM software always applies boundary conditions? What approaches are used to deal with these issues in practice?
Thank you!
K.-J. Bathe in his "Finite Element Procedures" (1996, Prentice-Hall, Inc., P.190) writes the next: "In an alternative approach, the required displacements can also be imposed by adding to the finite element equilibrium equations the constraint equations that express the prescribed displacement conditions. Assume that the displacement is to be specified at degree of freedom i, say Ui = b; then the constraint equation k Ui = k b is added to the equilibrium equations, where k >> kii. Therefore, the solution of the modified equilibrium equations must now give Ui = b, and we note that … only the diagonal element in the stiffness matrix was affected, resulting in a numerically stable solution. Physically, this procedure can be interpreted as adding at the degree of freedom i a spring of large stiffness k and specifying a load which, because of the relatively flexible element assemblage, produces at this degree of freedom the required displacement b. Mathematically, the procedure corresponds to an application of the penalty method."
You might be interested in
Article Detecting the causes of ill-conditioning in structural finit...
That should not be so unless you have some additional constraints and/or contact, and if you are using Abaqus explicit.
The standard technique is to eliminate the specified DOFs from the matrix.
I suggest checking the model settings thoroughly.
Thank you all for your suggestions.
Victor J. Аdlucky, I will check out the text.
Nils Wagner, I know the article, but here the model is just a 2D cantilever beam with B23 elements, so I don't think there are any problems per se.
Chennakesava Kadapa, thanks. This is something I was thinking, but wouldn't this be difficult to do for a complex model with multiple fix-constraints.
To give a bit more context I attach the input file (with matrix output commands). I would appreciate it if you have comments (and time to provide them).
Regards,
Dear Peter O Hristov,
I looked at the stiffness matrix of your beam. To my mind, in this case Abaqus uses penalty method to take into account encastre BC (as Bathe has described). The large diagonal terms can not spoil the conditioning of the matrix - quite the contrary.
Peter O Hristov
The problem with commercial software is that they don't provide any details of the implementation.
To check whether Abaqus uses the penalty method for applying BCs or not, you can extract the stiffness matrix of your model without and with specifying any boundary conditions. Comparison of the entries in the matrices will provide answers.
In case it does use the penalty method, choose the direct solver option instead of an iterative solver.
Chennakesava Kadapa, yes. That's certainly a problem. I did this some time ago and will need to remind myself the result. The whole issue here is that I am experimenting with a custom iterative solver. As a matter of fact, when using the "\" in MATLAB, the software is issuing a warning, but produces the correct displacement vector. Another problem is that in order to get the stiffness matrix for the model, I seem to have to run the ABAQUS solver, which makes it all pointless (but this is for another question).
Victor J. Аdlucky, thanks for taking the time to do this. I am not sure this is the case. One thing I can do (as suggested above) is to enforce the BC by removing the first three diagonal entries of K and the first three terms in the force vector. Тhen, the condition number goes down from к(K) = O(1033) to к(K) = O(109). If I understand this correctly, one of the reasons for poor conditioning is having disproportionately large stiffness terms in K. I am yet to go to the text you recommended and see if I can get an inspiration there.
Thank you both!
Maybe it will be interesting, when parameter ELEMENT BY ELEMENT is used to generate local element matrices
*Matrix Generate, Stiffness, ELEMENT BY ELEMENT
no large diagonal terms will be added.
Victor J. Аdlucky , you are right there are no large diagonal terms, but this is expected, since BCs are applied to the assembled matrix.
Chennakesava Kadapa , I checked. Indeed it seems ABAQUS is using the penalty method.
- Badges
- Science topic