Ansys 12 Plasticity 1

[krs2ball]

Distinguished members:

I have found myself troubled by ANSYS. I'm trying to perform a nonlinear analysis in order to observe its plastic behavior (the structure i'm developing, it's a steel stack, or pipe)

The problem is that so far, ANSYS 12 only allows me to perform this analysis by aplying a displacement. But what really interests me, it is to be able to perform a load-based analysis to acchieve plasticity, with different types of loads (wind, earthqueake, whatever)

If anyone can help me with this, you would make me the happiest man alive.

Best regards!

 

[seymours2571]

What error are you receiving? I have performed plasticity studies in WB before with no problems having a mixed bag of constraints and loads.

Steve

Stephen Seymour, PE
Seymour Engineering & Consulting Group

http://www.seymourecg.com

 

[krs2ball]

Thanks for responding

I have encountered convergence problems. I can not check its behavior post yielding point, perfect plasticity.

A simple analysis of a steel pipe, with a load of 1(whatever unit) on its top.

My main problem is to succesfully acchieve perfect plasticity. Which i have been able to do performing a displacement-based analysis.

 

[seymours2571]

How much of the stress vs. plastic strain curve do you have entered into WB? Reason being, Ansys assumes that the stress remains constant for any additional strain after the last data point on your stress vs. plastic strain curve. Therefore, large strains in very localized areas became unstable.

This may be one place you might be having issues at. Another is you may want to introduce more load steps to ensure stability.

Steve

Stephen Seymour, PE
Seymour Engineering & Consulting Group

http://www.seymourecg.com

 

[krs2ball]

I am using a bilinear isotropic curve, with these numbers:

yield strenght: 3.55E+08 Pa
Tangent Modulus: 5E+08 Pa (I'm still figuring out the tangent modulus)

And I am using 50 load steps. That part is the one I can not acchieve, that the stress remains constant and the strain continues.

I will keep trying though, thank you again mr Steve.

 

[seymours2571]

Hmm...plenty of load steps...so that is probably not the issue.

What Young's modulus do you have?

The issue I spoke of in my previous post regarding the stress remaining constant after the last data point on your stress vs. plastic strain curve pertained to the multi-linear isotropic hardening model. Using the bilinear is much easier.

Are there any singularities in the model? Such as point loads or point constraints?

Steve

Stephen Seymour, PE
Seymour Engineering & Consulting Group

http://www.seymourecg.com

 

[krs2ball]

Mr Steve

I'm so sorry I took so long to reply (I was away, no internet, almost in the middle-age)...
My model does not have any singularities that could cause a problem related to that. In fact, I am keeping it simple in order to go slowly testing it so it can work.

Actually (after several tests this last week) I was able to acchieve plasticity, but only using a displacement based method.

Now I am facing another kind of trouble in which I hope someone can help me out.

New Challenge:

My chimney has a Tuned mass damper(TMD) on its top. I'm trying to model this TMD in order to get lesser vibrations.

If you Mr Steve have come across such problem in the past, I would appreciate your help on this new challenge.

Best regards!

 

[juzz]

Hello, krs2ball!

Can you send (put on eng-tips) the input file for plasticity problem?

I will try to help you but I can do this only after I see the input file.

Kind regards,

juzz

 

[krs2ball]

Mr Juzz

Here I attached the .x_t file that is the basic geometry i am using. My main problem was that i have only acchieved in a different model on a displacement-based method, but never with a load-based method.

And the other problem I am working on, it is to design a Tuned mass damper on its top (or something that can reproduce its function).

Best regards, thank you for interesting.

 

[juzz]

Hi, Krs2ball!

First, the input you put there is only for geometry (I presume, seems a transfer from Parasolid). Anyway, I need to have the mesh and the boundary and loading conditions because the solver use these information and not the geometry.
When I asked for an input file I meant a file that can be loaded in ansys via command "read input file from....".

Anyway, open your model in Ansys, be sure that everything is selected, that all loads are applied and all boundary conditions set. After that type in the command line window from Ansys the following command:

cdwrite, db, model,

It will generate a file in your folder called "model.cdb". Provide this file, please.

Regarding the tuned mass damper, basically this is a mass connected to the chimney by a spring and a damper. Probably you try using this for damping vibrations excited by vortex shedding (wind dynamic effect). My advice is to represent the chimney as a 2-D bar (BEAM3 element) and connect the mass (MASS21 element) by intermediate of some combination of spring and dashpot (COMBIN14 for example).
With this model setup you will have to perform a harmonic response analysis (see Structural Analysis Guide from ANSYS help for procedure).

Kind regards,

Juzz

 

[krs2ball]

Hey Juzz

I'm sorry about that. I thought of that, because i use ANSYS 12.1 and it works with this system of modules. I know there must be a way to export to a .cdb file, but I'm not really sure how to. The .wbpj is too large to attach it here.

Anyhow, i performed on that same model a simple mesh with a max. size of 380mm. I tried by using multiple forces just on the top of it: 5tonnef, 15 tonnef...and the problem is that at some point it does not converge into a solution.

My question are these:

- can i perform a load-based non-linear analysis? will I acchieve plasticity?

-I have to run a couple of earthquakes on my chimney, do you know any tutorial about this? I have used different softwares (SAP, etabs, etc) to perform this task, but I am kind of new on ANSYS, and actually i started off using ansys 12, never used the ones before this.

Thank you again for your time and fine will.

 

[Pawel27]

Hmmm.. I am wondering about your tangent modulus. Why it is so big? It can cause convergence problem... Please use smaller... like 1-5MPa.

 

[krs2ball]

Thank you Pawel, I will try with that tangent modulus. I'm having an awful time trying to get my model to converge.

 

[kan123]

Displacement-controlled loading is easier for a finite element code because those are the degrees-of-freedom of the solution. It is usually harder to get nonlinear convergence with a force load than a displacement load, especially if your tangent modulus is low. As you get past the knee of the stress-strain curve, a small change in force causes a huge change in displacement. You need to apply the load up to the point just before plasticity, then change to a very small load increment through the transition. You may be able to then change to somewhat larger increments. However, if the yield zone increases to the point that you have full section yielding, then your structure would be unstable and you probably wouldn't get a converged solution.

You can do a sensitivity study where you start with a tangent modulus only slightly less than the elastic modulus. Then see how the solution changes as you do runs with progressively smaller tangent moduli.

As for dynamic analysis (such as harmonic response), most of the those solutions can only be done with a linear model. If nonlinear effects are important, then you would have to do something like a direct (full) transient solution.

 

[FahimJavid]

Hi All,

 

[FahimJavid]

I am working on my thesis and in a part of it, i have to model a beam traversed by a moving load and a TMD attached to the beam.
I tried different methods to model the moving load, i think that part work pretty well; but the problem is TMD doesnt work.

In fact, it works when I do the Harmonic analysis on the system, but when it comes to transient analysis (moving load), tmd doesnt work.

Ive been fooling around for 2months. im stuck!
so, if you can help me through this, it would be REALLY appreciated.

Cheers,
Fahim

 

[cloa]

FahimJavid- you should start a new thread and krs2ball you should start a new thread for a new problem (TMD)

 

[krs2ball]

Fahim,

How do you check wheter is working the TMD or is not?
Please tell us more about your problem.

 

[flash3780]

Have you tried turning on stabilization? If your part is buckling, stabilization should help ANSYS converge on a solution.

 

[mgage]

Once you get yielding through the entire cross section of your pipe the analysis will fail. This is due to the fact that any more load will result in an infinite displacement because you are perfectly plastic. I've done this exact type of analysis before by using time steps to "sneak" up to the point where it will no longer converge.

Marcus