I currently have a portion of a stent and balloon that I have assigned boundary conditions to such that they will account for symmetry and only move in the appropriate directions.
Here is the setup for my simulation:
- Homogeneous solid for the stent & homogeneous shell for the balloon
- SS 316 for Stent and rubber for balloon (Young Modulus: 4000MPa ; Poisson: 0.45)
- "General Contact" interaction with "No friction" and "Hard Contact" interaction properties
- two steps: the initial and a displacement step
In the displacement step, I have assigned a boundary condition to the balloon such that the nodes all move radially outward, interact with the stent, and will ultimately inflate the stent.
- Displacement step: Time period: 5 ; NLGEOM: On ; # of increments: 1000
One of the main problems, if not THE problem, is that the time step increment decreases so much that the simulation always maxes out the number of increments I have assigned.
I have the simulation set to run for 5s and after about 2.75s (total time) the time step has dropped to the 10^-16 magnitude. This always causes the simulation to abort because it has reach the max number of increments.
Does anyone know what I can do to get this simulation running properly? Thanks.
whats the message you receive in the log or msg files ?
do you use abaqus standard or explicit ?
The message I get is the "Error: too many increments needed to complete this step" but that is because the simulation's time steps become so slow. Other than that erro, There aren't any other error in the message file that indicate why the time step slows.
I am using Abaqus Standard.
Hi. Is there anything you can do with Hourglass in Abaqus.? I'm pretty sure Hourglass can help the time step not drop too much!
You should look at the warnings before you get the final error. (Abaqus will tel you that it needs to cut back on the time increment because of something.) Look at the points in the model where the largest residuals and displacement corrections occur (you can do this in the Job monitor). Possible problems you encounter may be an instability (due to plasticity or to a geometric effect, e.g. the thickness of some part reducing so that the load cannot be borne). Since yo use rubber, you should use hybrid elements (element name contains an "H") to avoid trouble from volumetric locking.
It is difficult to be more specific without seeing the model.
Your problem is highly nonlinear: large deformation and contact. It would be better for the convergence if you run the model with explicit algorithm available in Abaqus.
@N. Huynh Nguyen
I strongly disagree. It is much better to understand the origin of convergence problems (and thus gain a better understanding of the model and its behaviour) than to simply rely on the explicit method, especially in a problem where dynamic effects will be small to non-existent.
The balloon is inflated, so there may be a buckling as snap-through. If you want to stay in static, an arc-length algorithm should be used (Riks method in Abaqus).
However. This is a quasi static problem so explicit can be used too.
Checking the deformation of the model is also necessary, if it looks physical or not.
@N. Huynh Nguyen
That's exactly why I would recommend to first understand the problem in the implicit simulation and then look for a way to solve it - otherwise one might waste time by switching to, e.g., Riks or explicit, even if this proves to be unneccesary or not helpful.
I think that time spent in understanding convergence issues is always well invested.
Hey,
I've just worked on a similar case, I had the same problem.
I worked using "axisymmetric shell" instead of solid.
I thought I had a problem with my model..but the surprise was that it was sufficient to change the initial step and it worked!
Komeli:
The are a good amount of hourglass controls I can implement when selecting the "Element Type." For the stent, I am using the 3D stress family so it will use the defaults for Hourglass stiffness and will not let me chance it. If I switch the type to "Continuum Shell" there are four different "Hourglass Controls" (default, Enhanced, relax stiffness, and stiffness) do you have any recommendations for this? For the shell (balloon portion), I cannot alter the Bending hourglass stiffness but can play with the "Drilling hourglass scaling factor." Should I specify that? If so, to what?
Martin:
The only error messages that I get before it Aborts is:
There is zero MOMENT everywhere in the model based on the default criterion. please check the value of the average MOMENT during the current iteration to verify that the MOMENT is small enough to be treated as zero. if not, please use the solution controls to reset the criterion for zero MOMENT.
When I first start the simulation I also get a recommendation about specifying the *CONTACT INITIALIZATION ASSIGNMENT because I am working in the general contact domain.
I also get a warning about 8 distorted elements and 2 unconnected regions.
Martin & Nguyen:
I am not very well versed in what to use with regard to standard vs. explicit. Let me know what your thought are as we go forward.
Dana:
How do I go about using an axisymmetric shell? I have the balloon as a "Shell / Continuum Shell, Homogeneous" and my stent as a "Solid, Homogeneous" part. I am looking for "axisymmetric shell" under the "Sections" but do not see it.
Thank you very much for the help thus far! This has all been a major help in understanding how abaqus works and functions.
@Jared
I'm quite sure you are overlooking something, otherwise it would be a very weird error. The moment warning is usually irrelevant, but if Abaqus cuts back the time increments, there must be a reason for this. If you look at the final attempt of the final increment, directly before the "time increment too small" error, there should be a message "cutback of time increment is required". And directly before *that*, there should be some hint why this cutback is needed. Or you could upload your msg-file for us to look at.
@Martin
Here is was the msg file reads out:
...
***WARNING: THERE IS ZERO MOMENT EVERYWHERE IN THE MODEL BASED ON THE DEFAULT CRITERION. PLEASE CHECK THE VALUE OF THE AVERAGE MOMENT DURING THE CURRENT ITERATION TO VERIFY THAT THE MOMENT IS SMALL ENOUGH TO BE TREATED AS ZERO. IF NOT, PLEASE USE THE SOLUTION CONTROLS TO RESET THE CRITERION FOR ZERO MOMENT.
COMPATIBILITY ERRORS:
TYPE; NUMBER EXCEEDING TOLERANCE; MAXIMUM ERROR; IN ELEMENT VOLUMETRIC 0 2.870E-09 4706
INSTANCE: F13_STENT_6LEAF_FORABAQUS_1-24_SHELL_F
***NOTE: THE SOLUTION FAILS TO CONVERGE IN THE MAXIMUM NUMBER OF EQUILIBRIUM ITERATIONS ALLOWED.
***ERROR: TOO MANY ATTEMPTS MADE FOR THIS INCREMENT
***ERROR: THE ANALYSIS HAS BEEN TERMINATED DUE TO PREVIOUS ERRORS. ALL OUTPUT REQUESTS HAVE BEEN WRITTEN FOR THE LAST CONVERGED INCREMENT.
...
I took a look at element 4706 and it is not a distorted element; it looks like it is a normal element that would function accordingly. I am not sure if that is the element causing the problem or something else.
@Jared
O.k. - this is still not too helpful (not your fault...), but it may be that convergence is simply too difficult without any clear error/warning given. (You can look at the force balance info in the msg file to see whether the residual force is too large or whether it is the disp. correction - the momentum warning is usually irrelevant).
One thing to try is to increase the numbr of iterations in the nonlinear analysis. If you work with the inp-file, add
*controls, analysis=discontinuous
to the step-definition, in CAE you can do this somewhere in the step module under controls (I think it's general solution controls). This often helps resolving convergence issues if there is no instability but just a difficult solution process.
If this does not help, could you upload your model?
- Badges
- Science topic