Problem of an unconstrained model

[lukasz2]

Hi,
I have quite complicated .IGS model imported from SolidWorks. I meshed it using Shell93 element. And during the solving process I have error message like this:

The value of UX at node 18556 is 1.061435247E+11. It is greater than the current limit of 1000000.This generally indicates rigid of body motino as a result of an unconstrained model. Verify that your model is properly constrained.

One of the solution is to find all nodes and constrain it by appling DOF but it`s stupid solution... This is the only one problem with my analysis, and I don`t know how to manage with this.
Please help me!

 

[cbrn]

Hi,
I'm not sure I understand correctly. By "complicated", I suppose you mean that it's made of a lot of components. If this is true, you have a problem of connections between them (appropriated sets of contacts should solve this). If this is false, then you have a global degree-of-freedom problem, i.e. the restraint(s) you apply to your body are not so to "impeach" 3 independent translations and 3 independant rotations.
A modal analysis could be a way to understand the global DOFs left free: you will find one zero-frequency rigid-body mode for each DOF which is left unrestrained.
Regards

 

[lukasz2]

Ok lets simplify model to simple pipe which was created in SolidWorks, saved as .IGS and imported to ANSYS. Element type is SHELL93, then I go to real constants, material properties, mesh, displacement- one end constrained on the second end I apply force and run the solution (static). After few seconds there is the same warning about value at node that is greater than current limit 1000000...
In the same model created in ANSYS by modelling ->create-> piping model, there is no problem with solving…

 

[Transient1]

In your second case, are you applying a very large force that would produce a large displacement? Try reducing the force to a small value and see if that solves. If it solves, then you will need to turn on large displacement formulation for it to solve.

 

[lukasz2]

Force is OK, I tried calculate it also for gravity loads, the same: value at node is greater than current limit 1000000. I enclose file with pipe in attachment.

 

[cbrn]

OK, from your own post I desume the problem is not in the boundary conditions but in the model itself. Are you sure that the model coming from the external program is not treated as a collection of "independent" surfaces/bodies instead of one single "pipe"?
Second question: did you already try the modal analysis? If yes, did you find rigid body mode(s)? Did at least one of them correspond to the error message you are seing?

 

[lukasz2]

You`re right, I think that program treat my model as independent surfaces. I did modal analysis and I saw that some surfaces was outside the model. What should I do to delete this effect??? About modal analysis, the following frequences are increasing.

 

[balu25]

NUMMRG, Label, TOLER, GTOLER, Action, Switch

try this command

 

[cbrn]

Hi,
yes, diagnosis confirmed. Solution by Balu25 also.
In human terms, you have to "merge" the common lines / keypoints between the surfaces.
A word of caution, though: it is possible that in some cases the operation is impossible (degeneration of topology or other "kind" artifacts which are always possible when importing IGES files...)
Regards

 

[lukasz2]

Thanks it work but... not exacly. There is another problem, my model is windmill blade where Ansys see exterior surface as area, and bear beam and ribs inside as volume (one volume) and there is no connection between area and volume. It`s impossible to connect them by merging lines or keypoints. If there is possibility to connect them in one part??? I tried on enlargement connect them by lines or areas but it was useless...

 

[cbrn]

Hi,
this is a problem of tolerance in the IGES original conversion, or a problem of tolerance during import, or most probably the original model could have been built like that: complex surface as a "surface" and ribs and other structural elements as "solids". In this case, with most softwares (Solidworks, Catia, UG NX,...) you can "promote" the surface to a "null-thickness" solid, then "add" it to the other bodies with a boolean operation. But this wouldn't help you in ANSYS, where the concept of "zero-thickness" is unknown for a solid (in fact, 3D Finite Elements with no thickness do exist, they are called... SHELLS!!!).
So, where is the solution? Manipulate the model in the CAD environment so that everything is united together, so that the "crossing lines" between the surface and the ribs, for example, do exist as model's entities. Then, in ANSYS, use shell elements for the surface and solid elements for the solids. Be careful of interface problems (or use SOLSH190 element).
I realize that what I've written is not so clear... I hope it will give you some ideas, though...
Regards