Learning Forum

[Venugopalb]

Hello all!

I am doing nonlinear buckling analysis in a shell. sometimes, workbench solves the model and give a converged solution. But, In some cases, it is converging up to yield point. After that, it shows a convergence error. How to resolve this problem?

Here I am using geometric imperfection of linear buckling modes 1 and 2.

Please give some guidelines.

Thanking you

[Sandeep Medikonda]

What specific error message is reported in the solver output?

What type of material behavior are you providing?

[Venugopalb]

Hello sir!

The complete error message is given below

Material property used is given below

I used the imperfection code,

/prep7

UPGEOM,0.5,1,1,file,rst,

UPGEOM,0.5,1,2,file,rst,

cdwrite,db,file,cdb

Thanking you

[Sandeep Medikonda]

So, you are adding the displacements from a previous analysis? what is the reasoning for that? Also how far into the simulation do you proceed and what does the force convergence look like?

In multi-linear plasticity, you need to specify Stress vs Plastic Strain....So at zero plastic strain, you would have to start at yield...this is one clear mistake.

Once you fix that, I would also look at the plastic strain in the model....It is very likely that you are exceeding what you are specifying here as the max. plastic  strain...beyond this point ansys does not extrapolate and your tangent stiffness might be zero which could be causing issues....I would use the slope of the last 2 points and add a dummy point with a very high plastic strain value or use a bi-linear elastic-plastic material model....

[Venugopalb]

Hello sir!

1. I added displacements of linear buckling analysis to introduce imperfection in the model.

2. We are feeding the stress-strain curve to Ansys to predict the behavior. but you stated that for 0 plastic strain it should start with a yield point of stress. I think there is no difference. How can I calculate the strain with respect to stress after a yield point?

3. Is it necessary to add yield and ultimate strength data when we feed multilinear Isotropic hardening?

 4. How do you say that plastic strain exceeded the maximum value?

[Venugopalb]

Sandeep sir!

As you said I have considered plastic strain at yield point is 0 and calculated subsequent plastic strain by subtracting the subsequent plastic strain values as shown below.

 

 

 

Is it correct?

[Sandeep Medikonda]

Yes, subtracting elastic strains is how I would do.

I am pointing out a typical problem with multi-linear plasticity models based on experience. I am not sure if it is the cause of the problem in your case.... But check for plastic strain and see if has exceeded the max value....because it is a buckling problem my guess is that it has...

Either way, Consider adding some stabilization and see if it helps with convergence....start with a small value such as 5e-02 or 0.1 even....

[Venugopalb]

Thank you, Sandeep!

yes. It is a buckling problem.

1. How can I check plastic strain exceeds the maximum value or not?

2. I have given material data as Young's modulus, Poisson's ratio, yield strength, ultimate strength, and Multilinear strain hardening. Is it enough?

3. As per your suggestion, If I add Stabilisation, it may affect the result. Right?

 

[Sandeep Medikonda]

Right-click on the solution and add an equivalent plastic strain

Yes, you need to check for the stabilization energy and make sure it is small enough.

[Venugopalb]

Yes sir.

I will try it.

/prep7

UPGEOM,0.5,1,1,file,rst,

UPGEOM,0.5,1,2,file,rst,

cdwrite,db,file,cdb

In the above mentioned imperfection code, what will be the maximum value as we can give? Give some commands regarding this.

Thanking you for our quick reply.