Union model and Bonded Model

[Anonymous]

Dear all,

While importing the a 3D model from autocad with more than 3 parts, is it required to union command it those models in autocad itself and to import in simulation mechanical or just to import as separate elements and specify as bonded contacts in simulation software.

Find the attached model.

Regards,

Giridharan S

[marwan_azzam]

Hello @Anonymous

Either way is fine.  You can combine the models in Autocad and import the model as one part or you can leave it as an assembly.

The only two reasons why Simulation Mechanical would need separate parts is for different element types (brick, beam, plate, etc...) or a different material properties.  Otherwise the entire model can be all be one part.  Modifying the CAD model to combine the parts into one part could be unnecessary work.

In certain situations where the geometry is complex is is easier to mesh the model if it's one part but the is definitely not the case in your model.

Regards,

Marwan Azzam

[Anonymous]

Hi Marwan,

Thanks for your prompt response. Thinking the same I have tried using two options of importing (AutoCAD union and Simulation Bonded), but the end results are not matching between these two procedures. What should be followed then ? Which is correct method for ? What basis simulation working with this kind of input models. Kindly find the attached results and model.

Regards,

Giridharan S

[marwan_azzam]

Hello Giridharan,

Are you getting the same displacement from both models?

If not, you need to find out why and address that.  There is no sense in comparing the stresses if the displacements are different.

Also, when you have a multi-part model, the way the stresses at the interface between parts is calculated is is different.  Please see this section of the documentation.  In specific, the Smooth Results section.  For the multi-part model, you'd want to Smooth Results Across Part Boundaries.  This is found under Results Contours.

PS:  If you want to send out a model, the *.fem file is not enough.  You need to create and send the archive (*.ach file).

Regards,

Marwan Azzam

[Anonymous]

Dear Marwan,

Displacement results also not matching, 2mm vs 3.3mm.

This time I have attached the arch converted model for your reference.

Regards,

Giridharan S

[John_Holtz]

Hi Giridharan,

There is something wrong with the archive files (.ACH). The files are only 22 bytes and do not contain anything. Did you use the "app button > Archive > Create" command to make the archive files?

You can also compare the two models to determine why the results are different. For example,

1. Is the mesh finer in one of the models? A finer mesh usually gives more accurate results (which are usually larger and with a coarse mesh).
2. Have you done a mesh convergence study on both models? That is, have you made the mesh finer and finer until the results no longer change? This is necessary to know whether the mesh size is causing a difference.
3. Are the sum of the reaction forces the same? If not, the loads are not the same.
4. If the legend is set to the same minimum and maximum for both models, are the results "the same" except for a certain region? What is different about that area where the results are different?
5. Is the high stress occurring at a corner? Does the stress continue to rise when a finer mesh is used? Such situations are mathematically difficult for FEA to solve. (If the mesh gets larger and larger as the mesh is made finer and finer, the result is a mathematical issue and should be ignored.)

______________________________________________________________

If my post answers your question, please click the "Accept as Solution" button. This helps everyone find answers more quickly!

[Anonymous]

Hi John,

Thanks for reply. Kindly find the attached re-archived model.

Regards,

Giridharan S

[AstroJohnPE]

Hi @Anonymous

What are the results of the mesh convergence tests that you were supposed to do on both models? Do you get similar results when you use the same mesh size on both models?

What are the answers to the other questions (3, 4, and 5)?

[Anonymous]

Hi john,

These are results of iteration.

Cad Combined -
Iteration 1 - 297 MPa
2 - 379
3 - 431
4 - 666

Bonded -
Iteration 1- 1060 MPa
2- 1101
3- 832
4- 727
5- 513

Model crashed. Further details I cannot retrieve.

Let me check with other simple model.

Regards,

Giridharan S

[AstroJohnPE · Accepted solution]

Hi Giridharan,

"Iteration 1", "iteration 2", etc have no meaning. You need to record your results based on the mesh size. Likewise, you need to be specifying the absolute mesh size (in mm for example) and not percentage. (The mesh size by percentage changes from one model to another, so "100%" in one model does not equal 100% in another model -- even when the overall geometry is the same as in your case.) Set the absolute mesh size from "Mesh > 3DMesh Settings > Options > Surface > Type > Absolute mesh size".

When I ran both models at 5 mm mesh size, the stress results were 575 and 585 MPa and the pattern was identical in both models. In other words, the results were the same. (10 MPa out of 600 is insignificant in FEA. Differences in the pattern or differences of 5% to 10% are significant.)

As Marwan indicated, the next difference that you need to be aware of is that the model with one part will smooth the result between the fins and the column because they are one continuous part. The model with separate parts will smooth the results within each part, but by default they will not smooth the results across the part boundaries. To have a valid "apples to apples" comparison, you should turn the "Results Contours > Settings > Smoothing Options > Smooth across Part Boundaries" on. This will help to reduce any high stresses that occur in the corners of the fins.

The next thing that you may find as you make the mesh smaller and smaller is that the stress continues to increase. In the real world, the stress would level off at the theoretical value as the mesh becomes finer and finer. This does not happen in some models, especially at corners. You can think of corners as "0 radius fillets" which would have a stress concentration factor of infinity. The same thing happens mathematically in some models. The stress will continue to increase as the mesh gets smaller. If you see the stress go from maximum to a much smaller value over 1 element is an indication of this type of problem. When you see this occur, you have to ignore those high stresses. You can extrapolate the stress from nearby nodes to the corner to get a more reasonable estimate of the stress at the corner.

[Anonymous]

Hi John,

Thanks a lot for your detailed explanation. Let me do the same type of analysis from my side.

1. But for solid elements can we give surface mesh option.
2. As stress increases continuously upon reducing the element size, which stress value should be taken for design purpose. Is there any specific element size for which the stress to be taken for design.

Regards,

Giridharan S

[John_Holtz]

Hi @Anonymous

1. The mesh size is the mesh size. There is no difference between the size of the mesh on the surface and the size of the solid elements. One drives the other.

Also, the only setting in Simulation Mechanical for the size of the mesh (whether it is on the surface or inside the volume) is the control that I mentioned: "Mesh > 3D Mesh Settings > Options > Surface > Type > Absolute mesh size".

That is not entirely true because you can add mesh refinement to selected areas of the model as well. But without specifying the mesh size of the model, there can be no mesh refinement.

2. What I would do is extrapolate the stress from nearby nodes to the corner to get a more reasonable estimate of the stress at the corner. There is no "magic" mesh size that will give the correct result.