Too many increments needed to complete the step Help Please 1

[Rangatang]

Hi all

I am running a simple composite beam analysis but the job is continually aborted with the following error

Too many increments needed to complete the step

I have checked that the boundary conditions are defined and there is no contact surfaces.

I have attached the input file and the message file

I am a very new user to abaqus and any help would be greatly appreciated

 

[Rangatang]

sorry here is the input file

thank you in advanced

 

[amubashar]

In your step definition, I changed maximum number of increments to 1000 and initial increment size to 0.01 and the job completed in 242 increments.

 

[IceBreakerSours]

Static analysis with linear elastic isotropic material properties (and no contact etc.) should NOT take hundreds of increments!!

If you switch back to default settings in the analysis procedure:

*Static
0.1, 1., 1e-05, 1.

You must understand what the warnings and errors in the generated files mean. If you open the .msg file, here are some warnings:

"***WARNING: SOLVER PROBLEM. NUMERICAL SINGULARITY WHEN PROCESSING NODE PART-1-1.134 D.O.F. 2 RATIO = 61.3097E+09.
***WARNING: SOLVER PROBLEM. NUMERICAL SINGULARITY WHEN PROCESSING NODE PART-1-1.56 D.O.F. 2 RATIO = 213.310E+09.
***WARNING: SOLVER PROBLEM. NUMERICAL SINGULARITY WHEN PROCESSING NODE PART-1-1.1021 D.O.F. 2 RATIO = 7.94402E+09.
***WARNING: SOLVER PROBLEM. NUMERICAL SINGULARITY WHEN PROCESSING NODE PART-1-1.318 D.O.F. 2 RATIO = 4.96852E+09.
***WARNING: SOLVER PROBLEM. NUMERICAL SINGULARITY WHEN PROCESSING NODE PART-1-1.556 D.O.F. 2 RATIO = 54.9321E+09."

Open the ODB, go to Tools->Job Diagnostics, click on Job and on the right hand side, click on Warnings. You'll notice the same set of nodes reported as pointed out in the warnings in the .msg file. The warnings mean that ABAQUS believes that five nodes in the model are free to displace in the Y-direction.

Also, if you look at Tools->Create Display Group->select Elements, you'll notice warning elements. ABAQUS is NOT happy with the aspect ratio of the elements. They are very thin.

It is your job to figure out why those warning nodes are behaving the way they are and, if and how to fix the mesh. However, let me suggest a hint: Element sets _PickedSet23 and _PickedSet24 are assigned Platinum material property. However, these elements are the faces of continuum elements NOT membrane/surface/shell elements - which is what you should create. On the one hand, you are assigning PPY material property to the top and bottom layers of continuum elements, and PVDF to the middle layer, and on the other hand, you are assigning yet another material property to the faces of those very continuum elements some other material property.

Option 1: You need to create a surface (2D) of appropriate dimensions and assign membrane/shell/surface elements the Platinum material property.

Option 2: Learn how to make composites (Property module -> Composite -> Create) in ABAQUS/CAE. Use the documentation for examples and other help.

Some questions for you to think about:

"*Static
0.02, 1., 1e-07, 0.02"

On what basis did you switch the default settings of the static analysis procedure?

"*Element, type=C3D8R"

Why did you choose reduced integration elements?

Since you are a beginner, I'd recommend doing the cantilever test in 2D space and then in 3D space on 1D (like trusses), 2D (like membrane) and 3D elements (like bricks). Compare the results with analytical results. Then, you should move on to composites.

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083