Please some advice and helps for my thermal stress analysis.

[Anonymous]

Hello. I’m writing from Japan.

I’m a beginner at English, so I’m sorry for my poor English..

This time, I tried to perform the thermal stress analysis of a three-layer cantilever.

There is a temperature difference between the first layer and the third layer.

When I analyzed it, a model was displaced in a horizontal direction.

Intuitively, the model is displaced in vertical direction because of the temperature difference between the first layer and the third layer. (Like below figure)

I think this result was not correct.

I just started simulation at Nastran In-CAD and using Inventor, so I want you to give some advice.

I’ll describe below what procedure I analyzed.

I used a “Mate constraints” with each part at "Inventor 2019", then I used a “Mate constraints” with YZ plane of the first layer and YZ plane of the second layer. I dittoed with YZ plane of the third layer and YZ plane of the second layer.

Lower figure is image of three plates before constraints.

At Nastran In-CAD, I analyzed as below like “Heat Transfer and Thermal Stress Analysis of an Exhaust Manifold” in tutorials.

Firstly, I chose the “linear steady state heat transfer and thermal stress”

Due to face constraints between the first layer and the second layer, and the third layer and second layer, I did “surface contacts" automatically. Then “Contact type” was bonded and “Penetration type” was symmetric.

A material of the first and third layer was “Aluminum 6061”, and a material of second layer was unique orthotropic material which was referred to “Aluminum 6061”

“Reference temperature” of the first layer was 353.15K, and “Reference temperature” of the third layer was 273.15K. I didn’t input the second layer’s “Reference temperature”.

All parts were solid elements.

The mesh element size was 0.01 and I selected “Liner” from “Element order”.

The load type was “temperature”, the first layer is 353.15K, and the third layer is 273.15K.

I had analyzed this, then I performed thermal stress analysis based on result of “Heat Transfer and Thermal Stress Analysis of an Exhaust Manifold”.

I did two below commands like tutorials.

1. In the tree view, right-click on Manifold Analysis, and choose Duplicate. This will create a copy of the analysis with the name as Manifold Analysis - Copy.
2. Now, Manifold Analysis - Copytree is in active mode. Under Subcases left-click on Subcase 1 to select the name, and rename it to Subcase 2. Remove the Initial Temperature load from Subcase 2 as it is not required for a thermal stress analysis.

The load type was “From Output”, and I selected  FNO file(result of “Heat Transfer and Thermal Stress Analysis of an Exhaust Manifold”) at “Result File” in the “Load Definition section”

The right end face was constraint because this model is a cantilever.

I analyzed these conditions.

Thank you very much for reading the message through to the end.

Please some advice and helps for my thermal stress analysis.

Kind regards,

Takaya Nakamura(7515085)

[John_Holtz]

Hi @Anonymous

Your post was too long for me to read . I think it will be easier for someone to determine the problem if you attach the model. (For In-CAD models, you need to zip, rar, or compress together the Inventor part and assembly files, .ipt and .iam. Then attach the .zip or .rar file.)

[Anonymous]

Hello. Jhon Holtz.

Thank you so much for your advice.

I reconsidered a condition of constraint and I analyzed again because the constraint of the right side face was insufficiency.

However, my analysis didn’t go well again.

Following your advice, I’ll attach the model.

Please check the model and give me some advice and help.

Sincerely,

7515085

[John_Holtz]

Hi @Anonymous

The results indicate that there are constraints applied to the "free end" of the beam. (See Figure 1 below.) I know that you did not apply any constraints there, so this indicates that the analysis is adding the constraints by mistake. My guess is the very thin strips on the top and bottom are causing the problems. (If you look at the mesh of the thin surface, you can see that the thickness was not preserved in the mesh, so it is wrong to begin with. The mesher just is not designed to create a solid mesh on a part that is so very thin.)

Figure 1. Original analysis with three solids

The overall model size is 125 by 1250 mm. My suggestion is to not model the thin strips (only 0.025 mm thick) on the top and bottom using a solid. In fact, you should not even include solids 0.025 mm thick in the model. The entire analysis can be created by using one solid with the dimensions 125 mm wide by 1250 mm long by t mm thick. (See Figure 2.)

1. create one idealization using solid for the solid aluminum core.
2. create another idealization using shells for top surface. The thickness of the shells is 0.025 mm which you enter on the idealization dialog. You will select the face on the top of the solid for this idealization.
3. create another idealization using shells for the bottom surface. (Actually, the two shells can be in the same idealization since the properties are the same.)

If you set the shell idealization to use triangular elements, then no contact is required between the shell and solid because the mesh will automatically match. (The same geometry is used by the solid idealization and shell idealization, so the mesh is the same.)

In other words, thin "solids" should be analyzed using shell elements instead of solid elements. Depending on the geometry, you can create the shell elements by creating surfaces in the CAD model, or converting solid parts to shells using the "Prepare > Offset Surfaces/Find Thin Bodies/Midsurfaces" command in In-CAD, or just by selecting faces of the model (as in this example).

Figure 2: Three idealizations

Let us know if you have any questions.

______________________________________________________________

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

[Anonymous]

Hello. Jhon Holtz.

Thank you very much for giving me advice.

I retried to this analysis and I have two question.

Firstly, I used “Offset Surfaces” and selected the upper strip and lower strip. (offset is 0.0125mm, thickness is 0.025)

I deactivate the Automatic Face Chain option.

At this time, material of offset surfaces became same material of core.

Although, material of core is Orthotropic 3D, is this appropriate for shell elements as well?

Secondly, when I performed the thermal stress analysis, I gave this error. ”Mesh does not contain any nodes or elements.”

Mesh size hasn’t changed from previous analysis. (mesh size is 0.01, element order is liner and I checked “Continuous Meshing”)

Why I was taken this error message?

I hope to hear from you soon.

Sincerely,

7515085

[John_Holtz · Accepted solution]

Hi,

For your first item (offset surfaces), you need to use the material that is appropriate for the analysis -- you know which material that needs to be. Of course, you can edit the idealization and choose the material that you need.

Is there a reason that you are making the analysis more difficult than it needs to be? Using an offset surface (which then requires contact) makes the analysis twice as difficult and less accurate than other options. For example:

• This is just a guess, but I think the offset of 0.0125 mm is insignificant compared to the 20 mm thickness of the entire structure. (Or the offset is insignificant compared to the accuracy of a typical simulation.) The method that I described in a previous post avoids the difficulties and inaccuracies of using offset and bonding.
• If the offset is important, you can still use my approach. Shell elements can be offset from the location of the mesh, so you can create the model with a matched mesh but the simulation is based on the shell at the proper offset location. Under the idealization for the shell, click the "Advanced Options" and change the "Bottom Fiber Distance".

For your second item (mesh does not contain any nodes or elements), the problem is not related to the mesh size. The problem is that you have a part in the model that is not assigned to any idealization. This is only a problem if you missed a part in the assembly that is required in the analysis. See the article Error: Mesh does not contain any nodes or elements with Nastran in-Cad (Idealization).

[Anonymous]

Hello. Jhon Holtz.

Thank you so much for your advice.

I followed your advice, I succeeded my analysis.

First item(offset surface)

I want to analyze three-layer cantilever so offset surfaces are important for me.

Thus I changed the material of two strips from the core material to surface material.

Second item(mesh does not contain any nodes or elements)

When I used “Offset surfaces”, I selected upper and lower strips, so I exclude upper and lower strips from Analysis.

Then the error was disappeared.

Thank you very much for your help.

I’m glad to succeed my analysis.

I will make further efforts in my analysis.

Best regards,

7515085

[rledger9EX5S]

edit