Learning Forum

[Nuwad]

Hello, I have been tracking down an unknow cause of deformation in a Static Structural Analysis where I would expect displacement. After some work I have determined it to be a result of the APDL stabilization command. I have set up a basic model to demonstrate my issue.

The actual model's material is a lot more complex and non-linear but the overall concept is the same: I am using blocks to change the shape of a material. The material is represented by the top meshed body in this image

[Nuwad]

To add to my confusion when I look at the solver output after running an a model I see this message :
Material number 7 (used by element 14360) should normally have at least Material number 7 (used by element 14105) should normally have at least one MP or one TB type command associated with it. Output of energy by one MP or one TB type command associated with it. Output of energy by material may not be available.
Is this the reason I am not able to probe the stabilization energy? When I try to find the element it is not in my model in-fact the model has less than 14360 elements? All discussions about this Warning seem to say to ignore it, I just can not

What are MP and TB type commands?

[Sheldon Imaoka]

Review the Mechanical help documentation for "Stabilization Energy" - it is an output available after you solve for a converged substep. You can compare this to Strain Energy, for example. The Stabilization Energy is the artificial energy associated with work done by the dampers placed on all nodes for Nonlinear Stabilization. If these values are large, you need to decrease the stabilization parameter in the "Analysis Settings" branch.
Nonlinear Stabilization adds dampers to each node in your model. If the damping value is 'high', then the nodes will resist motion, so that explains why your part is behaving as such with nonlinear stabilization on - most likely, even the default value is too high, so it should be lowered. It is dependent on your model parameters, so it may take a little trial and error to include just enough stabilization to get a converged result but not too much to adversely affect your result. (We typically don't have a feel for the magnitude of damping coefficient, for example, so that is why it can be a trial-and-error process.)
An alternative is to put a low gravity field to put the piece towards the moving plate. If you have nothing constraining the piece, it may undergo rigid-body motion, but having a weak acceleration field (like gravity) pushing the piece towards the rigid plate can help keep all parts touching each other. (In a static analysis, you can't solve for situations undergoing rigid-body motion since that's a singular matrix and no unique solution.) I'm not sure if that is the cause of your error but just thought I'd mention it.
FYI, the warning message you cited in your second post can be ignored. TB and MP commands are APDL commands used to define material properties, but in this case, special elements (such as those used to represent boundary conditions or contact) may be present but don't need to have material property definition - the warning is just to let the user know that some elements have no material definition, which is usually fine for such cases.
Regards Sheldon

[Nuwad]

you are correct stabilization was decreased and the unexpected deformation was minimized. Also, interestingly enough probing # contacting (in the actual model) showed that the material displaces after number contacting changes to 1 which is exactly as expected. Implementing this in the actual complicated model involved increasing the number of steps but still worked. I have high hopes of success.

I have (in the past) implemented an "artificial" gravity field, I did and do not understand what this will actually do. What does it add to the solver or can you briefly explain this idea a little for me?

[Sheldon Imaoka]

In your case, you have a rigid plate that is moving vertically. Are there any boundary conditions applied on your meshed rectangular material? If not, the part is unconstrained, so it can move in the positive vertical (y-axis) direction with a tiny amount of force. By putting a small acceleration field ('gravity'), the piece is continually pushed against the small block, so it remains in contact.
In a static analysis, we should not have an unconstrained part. Having a load, such as gravity, acting in the downward direction, helps to ensure that all parts are in contact with each other and not experiencing rigid-body motion.
Regards Sheldon