the solution is not converging

[Showkat Ahmad]

I am trying to validate a corrugated web girder as shell element having different web and flange properties. But the solution is not converging.The web and flange are are glued together. please suggest me how i can over come the same. I get the error message" Solution not converged at time 1.E-02 (load step 1 substep 1).
thank you

 

[FEA way]

Please provide more information about the analysis. Especially tell us which software you use. There are many possible reasons of convergence issues. Usually the problem is caused by wrong BCs, contact or high nonlinearity. Can you attach pictures of your model showing boundary conditions, interactions ad so on ? If not please described these settings.

 

[Showkat Ahmad]

I am using ANSYS APDL version 18.
the material model used is multi linear. the beam is modeled as shell 181 element
the beam has two constraints at one end (in x and y direction) and one constraint at other end ( in y direction) i.e; the beam is simply supported.

 

[Erik Panos Kostson]

Is it a beam mesh, or are you using 3D elements (say solid186). If it is a beam then this model is not well restrained (it will start spinning about a long. axis)
Can you attach the input file (all the commands to generate and solve the model), and will have a look.

 

[FEA way]

It’s a 3D shell model, right ? It seems that you don’t have any constraint in the Z direction. All rigid body motions should be eliminated.

 

[Showkat Ahmad]

thanks FEA Way .
Its is a 3D model and I have constrained in z direction also but the same problem persists.

 

[FEA way]

To make sure that you model is not underconstrained for some reason you can perform modal analysis. But if rigid body modes are not the problem here then you should carefully examine another settings of the analysis. Units (especially in material data), shell thickness, interactions and so on.

 

[Erik Panos Kostson]

Showkat Ahmad, if possible attach the log/command file and I will have a look for you.

- If you can not then check:

1 Elements
2 Loads Restraints
3 Connections
4 Material and section Properties
5 Solver settings
6 Solver Logs

- Also as FEAway suggested run a modal analysis to see that everything is connected (that will address point 1, 2 and 3)
Deactivate non-linearity.
- If it solves without material non-linearity, but with NLGEOM,ON then it is something to do with nonlinear properties in combination with a high load causing a lot of yielding say. If is taht one need to have a fine mesh and use many cuts (load scaled), until the limit load is reached
- If it solves for NLGEOM,off and material on, then it is something like instability that could be happening (doubt it though since it is bending). Try then to use stabilisation, that might help.
- If it does not solve for the above then deactivate that (NLGEOM, and material) and see how it solves.
- If it does no then reduce the force to see that it solves for something small. If it is solves for something small it could be that the force was too large or the stiffness too small.

Try that otherwise attach the log file or the solver output

 

[Showkat Ahmad]

actually i have generated a MACRO for the same.
the log file is given below

 

[Erik Panos Kostson]

can not see the macro - use the feature at the bottom of the page (Attachment) to a attach a file.

 

[Showkat Ahmad]

sorry here is the log file

 

[Showkat Ahmad]

I have performed the modal analysis. the modes are not as expected. the mode shape is given below.why the beam is lifting up at the right end since it is constrained there?

 

[Erik Panos Kostson]

Hi

Unfortunate in the log file there is no mesh or geometry areas and so on. Do you have an iges file (you can export from ansys), or did you create the geometry in apdl using K, L and A commands?
In that case you can include the commands or save the iges and attach. As for the mode it is good that parts seem attached. For the constrain how do you constrain it (command or GUI)?

 

[FEA way]

That’s why modal analysis is used in sich cases. If first modes show some unexpected motion of parts that should be constrained or tied to other parts then something is wrong in the analysis setup. In this case probably the model is still underconstrained. Check BC definitions carefully again. Do the remaining few modes seem to be correct ?

 

[Showkat Ahmad]

I had a look at the geometry of the model and I updated the things as suggested by the experts . Now the mode shapes are as expected and the results are converging .
Thank you everyone for the help

 

[Showkat Ahmad]

I have done modal analysis and the modes are as per expectations. But the problem is after UPGEOM command I want to do non linear static analysis but the solutions are not converging. Please suggest some tips.

 

[FEA way]

So you want to perform non-linear buckling analysis of this beam, right ? Convergence problems are common in this case sonce it’s a highly non-linear problem and the solver may not be able to pass the bifurcation point without some help. Try arc-length method. It’s designed for simulations like that.

 

[Showkat Ahmad]

THANK YOU, I TRIED ARC LENGTH METHOD I THINK IT IS WORKING.

 

[Erik Panos Kostson]

The ansys arclen method is not that great, I normally recommend to use the ansys stabilisation for models that include instabilities.

 

[Showkat Ahmad]

Thank you Erik for your suggestion. Will try it