Mixed-Dimensional Coupling

[Anonymous]

I am trying to build an analysis for a model that mainly consists of thin plates.

However, the time of calculation is too long for a complete solid analysis and therefore I decided to use midplanes and plates.

My main issue is one plate bending over another under loads.

By building the whole model with midplanes, two of them, that have a face to face connection lose contact.

So I changed their mesh to solid. Now, the next problem was a face to face contact between one of the solids and another midplane part of the model. A solution with minibeams had neither a good result nor was it very practicable to implement.

My current solution is to split the plate that bends over the other into a midplane and a solid part. Here it works that all the parts keep contact, but it puts out an incorrect deflection curve that looks like some kind of a ball joint effect, where the contact does not take any moments.

I guess this is because of different degrees of freedom between the solid and the plate elements.

Is there a standard contact provided in Autodesk Simulation to solve this or is it possible to implement constraint equations?

[S.LI]

You must be very experienced on ASIM model setting.

After thinking a while, I couldn't find any better methods than what you did, such as mini-beam, shell+solid etc.

To transfer rotational DOF constraints between different element types is a tough problem generally in FEA. I don't think there is a good way to do this in ASIM by constraint equations or contact elements.

Not sure if you know there is a kind of composite shell element in ASIM MES, which allows multiple layers in one shell element.

If the difference of materials in your thin part is only the material orientation, it might worth a try on this element.

[John_Holtz]

Hello,

Can you elaborate on your "current solution"? Maybe attach an image or two. Are you saying that one part in Inventor (or whatever CAD app you are using) is represented by 2 parts in Simulation: one part is solid, and 1 part is plate? What is the "second" part in the CAD app that this first part contacts: plate? solid? plate and solid?

The plate to plate contact should be solvable using the "Nonlinear > MES" analysis type. Surface to surface contact lets the user define what the separation is between two parts when contact occurs. In your case, that distance would be half the sum of the two plate thicknesses. Try a test model first to make sure MES will accept such a large contact distance since it is usually expecting very small gaps when contact occurs.

[S.LI]

To correct one thing about composite shell in my previous post, different layer could be assigned different material.

But it might not work in your case, since it only counts the whole contributions from all layers, and doesn't distinguish the positions of layers (top or bottom). For example, bimetallic strip thermometer could not be simulated by composite shell, I think.

About the method with a plate attached to solid elements,

1.) how about finer mesh? Will it reduce the error?

2.) do you use mid-side nodes for solid parts? Usually, mid-side nodes are helpful in bending problems.

3.) what's the exact meaning on "ball joint"?

Thanks.

[Anonymous]

Thank you very much for your answers.

Attached you can find two images of the described problem. In the "mesh.jpg" you can see how the midplane and the solids work together.

On the right hand side there are the two solid plates. As you can see the lower one is fixed by boundary conditions.

Actually the purple-colored midplane is a part of the upper solid plate. In Inventor I designed two different parts so that I could define them seperately in ASIM.

The second image shows the same section in the results.

As one can see here, the midplane does not behave correctly. In my opinion the derivation of the deflection curve should be (more or less) zero close to the contact zone.

I already read about the MES-Solution. Isn't it too much to use a nonlinear analysis for a "simple" static case? Besides, unfortunately in my version nonlinear stress is not available (or I couldn't find it until now). Does it belong to an extra part that has to be installed seperately?

[John_Holtz]

Hi again.

I looked at your images but could not understand anything that I was looking at. I am also confused between what you are calling a plate, solid plate, plate elements (the midplane), and brick elements (solids). If a "solid plate" is something that is made with brick elements, then another term would reduce the confusion. (Maybe call it wall? sheet?)

And since it may be that the edge of the plate elements are contacting the side of the brick elements (as if the plate is normal to the solid?), most of the previous suggestions are probably invalid.

Whether you need the complication of the nonlinear MES analysis depends on the physical arrangement and the capabilities of linear versus MES (and what steps you are willing to do if there is a linear solution). The option for nonlinear analysis is at the same place where you have defined the analysis for every model you have created, most likely right when you imported the CAD model. But without knowing what version you are using, we cannot say whether you should have it or not. ("Help > About" gives a written description of what you own and the long version number.)

I suggest you read the thread Create, Post, or Provide an Archive of your model and go from there.

[Anonymous]

Okay, I am sorry for the confusion.

I will try to describe the issue more clearly with better pictures :).

In the picture minibeams attached to this post, you can see a side view of Part 2, which is solid, part 1a which is a solid too and part 1b that is meshed by plate elements. Furthermore there are other members that don't have to be considered at the moment.

Part 1a and 1b originally belong to the same component, but I divided it into two parts in inventor. As one can see Part 1a is connected with one edge to the face of the solid Part 1b and bends downwards.

In my opinion the final picture should look like shown in picture "minibeams".

Without any further contact-definition one can see an incorrect deflection curve in picture "without minibeams". This is what I meant by "ball joint effect", because the connection between part 1a and 1b seems to have at least one rotational DOF that is not correct.

Now my question is if it is possible to define an appropiate contact without the effort of minibeams in Autodesk Simulation.

Regarding the version: At the moment I am using the Commercial Version of Algor Simulation 2011, but our IT is working on 2012. So if you can think of a solution only available in 2012, that would be okay, too.

[Anonymous]

I found a better description / solution for my issue in the wikihelp-pages Contact (section: bonded contact between plates and bricks)

Are those techniques automatically implemented by using smart contact? If yes, which of the solutions does it use? The additional plates at the solid surface or the inner connection?

[John_Holtz]

It looks like you are making progress. The answers to your questions are:

No, smart contact does not use either of the methods shown on the page Examples of Contact that you referenced. The only time that smart contact should be used for plate to solid connections is if the rotation (your d/dx) of the solid is 0. If the solid has rotated at the point where the plate connects, smart contact will give inaccurate ("wrong") results.

No, there is not an automatic way of connecting plates to solids without using a method like your "minibeams" or one of the methods on the examples page.

[Anonymous]

Hi John,

regarding your answers I have some further questions, since I am trying to understand the theory that is implemented:

1. If smart contact does not use one of the mentioned methods, what exactly does it do? Does it simply turn off the rotational DOF at the line of connection?

When I use it at least there is no hinge effect. I am only worried about the transfer of stresses from plates to solid (You can see it in the attached picture).

2. Referring again to the wikihelp-page examples of contact, how would you realize the first example shown in figure 2?

[John_Holtz · Accepted solution]

Hi,

1. For smart contact between plates and bricks, the translation of the plate nodes is "interpolated" from the translations of the brick nodes. This is done using Multi-Point Constraint equations (MPC). The rotation of the plate nodes is set to 0 in all three directions; that is, the result is the same as applying a general constraint of "No Rotation" (Rx, Ry, Rz all checked).

2. It would not be possible to embed the plate elements into the brick elements when the model comes from CAD unless the solid is split into two parts where it meets the plate. In the image, the top two layers of brick elements would be on part 1, the bottom two layers of brick elements would be on part 2, and the plate would be on part 3. Then the embedded plate elements can be created by selecting the lines on either brick part and duplicating them ("Draw > Pattern > Duplicate").

[Anonymous]

Thank you very much. That helps a lot!

[Anonymous]

After some more experience with my model, I think it would be reasonable to simulate the contact between the plates by deleting the lower one and using an elastic boundary condition.

But how do I use the stiffness correctly? Usually the stiffness is calculated by K=E*A/L for translational DOF and K=EI/L for rotational DOF, so I applied this as a surface boundary condition. However, it creates a better(-looking) result, if the stiffness has a lower value and I think that I made a mistake somewhere.

Do I maybe have to apply a stiffness of the plate divided by the amount of nodes or something?

[Anonymous]

Oh sorry, I mean the rotational stiffness is K=Eh^3/[12*(1-poisson^2)]. However, my issue stays the same.