Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here


the solution is not converging

the solution is not converging

the solution is not converging

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

RE: the solution is not converging

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.

RE: the solution is not converging

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.

RE: the solution is not converging

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.

RE: the solution is not converging

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.

RE: the solution is not converging

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

RE: the solution is not converging

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.

RE: the solution is not converging

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

RE: the solution is not converging


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

RE: the solution is not converging

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

RE: the solution is not converging


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)?

RE: the solution is not converging

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 ?

RE: the solution is not converging

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

RE: the solution is not converging

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.

RE: the solution is not converging

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.

RE: the solution is not converging


RE: the solution is not converging

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

RE: the solution is not converging

Thank you Erik for your suggestion. Will try it

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members! Already a Member? Login


White Paper - A Guide to 3D Printing Materials
When it comes to using an FDM 3D printer effectively and efficiently, choosing the right material at the right time is essential. This 3D Printing Materials Guide will help give you and your team a basic understanding of some FDM 3D printing polymers and composites, their strengths and weaknesses, and when to use them. Download Now

Close Box

Join Eng-Tips® Today!

Join your peers on the Internet's largest technical engineering professional community.
It's easy to join and it's free.

Here's Why Members Love Eng-Tips Forums:

Register now while it's still free!

Already a member? Close this window and log in.

Join Us             Close