Large Plastic Deformation

[qwicker]

Hello.

I am modeling a 3D part (can only be done in 3D). I am applying a large tensile load which I know will exceed the yield point of the material(AlNiBr). I want to plug in the data points for the stress-strain curve in the mat'l properties as "nonliner multilinear elastic". However, the solution won't run with my selected element type. I was trying to use bricks (Solid 186) or tets (Solid 187).

What kind of element should I be using for this? Am I going about the plastic deformation the correct way by wanting to input the stress-strain data?

Thank you!

 

[Transient1]

The best way to get a good answer is to pose a good question. You have left out a lot.

Here are my questions:


If you know the tensile load will exceed the yield point of the material, what is the purpose of the analysis?

Are you working in ANSYS classic or ANSYS workbench?

Have you succesfully run a linear, non-yield stress case?

You have stated my solution won't run with my selected element type. What does that mean? It fails to solve or it won't start? What are the error messages ANSYS gives you?


Here is my response:

SOLID187 will work for plasticity.

For plasticity if you have the stress-strain curve data then you have all you need. You need to implemenet a plasticity law such as MISO (Multilinear Isotropic Hardening). You have to turn on non-linear effects using nlgeom,on or in workbench selecting the same option in the details box for the material and analysis setting.

The help documentation has plenty of information about non-linear analysis. Look at the Basic Analysis Guide and the Structural Analysis for procedures/theory.

 

[qwicker]

Hi, thanks for the response because I believe you have already pointed me in the right direction. To answer your questions:

-I am pulling a part in a tensile load via a steel pin inserted. Basically the pin is going through a hole and then being pulled while holding the opposite end of the part. The stressed developing at the hole (in a linear, non-yield case) is extreme, nearly 1million psi. Thus I have deduced that the part is going to yield plastically. I need to know by how much.

This is how I was setting up my problem.
Material Model: Linear Elastic & Multilinear Elastic (I am using both, should I be?)
Elements: SOLID95 (I tried SOLID 186,187 but both failed to start the solution. The error was immediate and said these elements cannot be used with TB,MISO)

Just to give a brief overview, I am basically pulling a 3D part made of Steel and I want to see how it plastically deforms since loading will be beyong yielding point.

 

[Transient1]

You left out if your working in workbench or classic. Also, you have left out the purpose of this analysis.

Your geometry is basically a brick with a hole in it. A pin is inserted in the hole. The pin is pulled in one direction and the brick is constrained in the opposite direction.

How are you modeling the contact between the pin and the block? Are you meshing the two geometries with a uniform mesh (vglue in classic, parts created from Design Modeler in workbench).

Your question about material model is a first principles type question. Does your material go through elastic deformation? Does it then go through plastic deformation? I think you can deduce the answer about which material models to use from those questions.

Have you refined the mesh (made it smaller) around the area of highest stresses to see how the stresses change?

If you look up SOLID187 in the element reference, you will see MISO is an allowable option.

 

[qwicker]

Sorry, Classic interface

The purpose of the analysis is to find out why some parts are failing in this tensile test that is being performed at our factory. We switched material specifications slightly and now some of the parts are deforming or breaking.

I have modeled the contact between pin and part as Bonded. The parts are meshed using smart size with the mesh tool. The geometry of the part is more complex than a brick with a hole in it, but thats the general idea.

My material is Beryllium Copper. I have the full stress/strain data available.

I am trying to decide which material model to use. Based on the GUI, I was going to use Nonlinear>elastic>multilinear elastic. However, after reading some documentation, I may want to go with nonlinear>inelastic>rate_independant>kinematic_hardening_plasticity>mises_plasticity>multilinear(general)

I think the latter is more appropriate based on what I have read in the Ansys Structural analysis guide.

 

[qwicker]

Just as an update, I am using SOLID187 (tets) with the multilinear (general) kinematic hardening (KINH). I set the time as 100 with 20 substeps. It is running now, but is bisecting the loadstep alot. I hope it finishes properly. Any thoughts on this, especially if I cannot reach convergece?

 

[Stringmaker]

If it's bisecting often then that would mean that you have lots of plastic strain going on. My first suggestion would be to use brick elements as this will reduce the DOF count significantly. If you still have a large number of nodes you may want to use the PCG solver to speed things up if the sparse solver is slow on your system. I've had large plasticity models run on good solvers for days...so I'm not surprised. If you're seeing 1E6 psi elastic stress then obviously you have a problem. Perhaps your analysis is a bit overkill for this situation.

 

[qwicker]

Well when I returned this morning It had given me the error that one of more of my elements had become highly destorted. It had already gone through 35 substeps too.

What would happen if the load that I am applying to the part is too much and will cause failure? How does Ansys handle that (other than just giving an error)?

I am going to remesh in SOLID185.

 

[Transient1]

If the material is deforming to the point of rupture, ANSYS will in all likelyhood not complete the solution and give you the type of error you are dealing with. Using the nonlinear inelastic, KISO or MISO options is a more accurate representation of your situation than using a multi-linear elastic.

Part of your error could be coming from the bonded contact around the perimeter of the pin, since as the part is deforming the area around the pin is being constrained to the circumference of the pin. Is this accurate for your model? Is the hole larger than the diamter of the pin?

Non-linear convergence can be a pain staking process. Try things like mesh refiement, and increasing the number of sub-steps, etc.

 

[qwicker]

Ok I got convergence! I used KINH as opposed to KISO. I changed the pin from bonded(always) to just bonded. I am going to play around with a few more options to see what the different solutions look like. Thank you!

 

[Transient1]

Glad to hear it.

Since you have failed pieces, does the analysis match the test results in terms of failure forces and location?

 

[qwicker]

Well I dont have the data on hand, but I hope to find out!