Error #2133 and Warning # 312 in OptiStruct
Altair EmployeeA few error were encountered during an FE-Analysis of a carbon - composite monocoque:
The first error was:
*** ERROR # 2133 ***
There are d.o.f.s that must be constrained, see the above table.
the number of d.o.f. = 1
grid # component : comments
----------------------------------------------------------------------
25570 5 : has no stiffness and is not constrained (*1)
----------------------------------------------------------------------
*1 : These d.o.f. must be constrained in order to run analysis.
How is it possible to detect the node that is mentioned in the error message?
The second error was:
A fatal error has occurred during computations:
FEASIBLE DESIGN (ALL CONSTRAINTS SATISFIED).
which might be related to:
*** WARNING # 312
In static load case 1, the compliance is negative or large 6.52117e+011.
Optimization/buckling analysis cannot be performed.
due to possible rigid body mode.
What does this error mean and how can it be avoided?
The third question is, if there is any documentation on the solver control cards in the online help?
Answers
-
To answer the three questions, it would be helpful to have a look at the model file. Here are some hints how you can check your model:
1) This first error is related to a single FE node that is not properly attached to your structure, e.g. an unconnected node in an RBE element or a temporary node which is in the input deck. To really tell you in detail, you would need to find this node or upload the model. Here is a short video on how to detect the node ID in HyperMesh:
By the way: the 'component' mentioned in the error is the degree of freedom (not the HyperMesh component) so in this case the rotation around y-axis is unconstrained
http://screencast.com/t/FXF6n5fwNTv
2) The warning #312 hints to very large deformations in your model. This might be due to
- unconstrained nodes in your model which lead to large displacements or rigid body translation / rotation
- unrealisticly high loading on your structure
- the overall large 'size' of your model, e.g. in shipbuilding or offshore simulation models
To avoid the error, please run a simple analysis instead of optimization and check your displacements. See if there are parts that deform or translate heavily and try to constrain them in the model.
3) To get some help on the control cards,you can usually enter the name of the control card in the OptiStruct Solver help -> Index. This will give a documentation how to use the control card.
An overview / listing of some most important run parameters can be found under the index search 'PARAM'.
Jan
0