Thermal-stress and strain analysis in ANSYS. Element type question. 1

[Staszkinson]

Hello,

I am going to perform nonlinear analysis of some shell structures - gas ducts in ANSYS WORKBENCH. I would like to take into account:
1/ thermal conditions
2/ pressure
3/ material nonlinearity
4/ geometrical nonlineality (large deflections)


A) What is the best ANSYS finite element type for this type of analysis?
B) Can you recommend any good tutorials/articles about shells in thermal conditions?
C) What do you think about finite element analysis using solid elements (tetra/quad) in my case (gas ducts). Should I even think about it?
D) What type of objects should I use to perform analysis using shells and wires in one model? Can you recommend any ANSYS element type for wire elements?

Thanks!

 

[rickfischer51]

First, do you have temperature data to apply, or do you need to start with a thermal analysis? If the latter, you need to start with a thermal analysis system, then attach a static structural system to it.

Second, the question is sort of moot in that WB picks the element for you. You have very little control over which element WB chooses. It will always pick the newer technology elements and ignore the legacy elements.

If you have heat generation and/or nonlinear materials, I think you need either multiple solids through the thickness or shell elements. I think you will find that if you are analyzing to a code like the ASME BPVC, postprocessing is generally easier with shells. Plus, the element count will be way lower



Rick Fischer
Principal Engineer
Argonne National Laboratory

 

[Staszkinson]

Dear Rick,
1/ Temperature. In the future, probably I am going to perform some CFD analyses with a little help of different work groups of my company. At this moment I need simplified approach. I want to define quite uniform temperature field in at some parts of my ducts. Let's say that I will analyse ducts in 100/200/400 Celsius degrees with NLGEOM on, and material nonlinearity. What do you think about this approach?

2/ Elements. I have some habits according to using ABAQUS. In this software choice of finite element type is transparent and clear. Thank you for explanation about picking the latest finite elements.

3/ Standards. I am going to use Eurocodes (standards for structural engineering) but I will also try to use ASME standards. Thank you for information about ASME publicatons.

Thank you for your help. I really appreciate it.

 

[rickfischer51]

1 In between CFD and applying temperatures as structural loads is a thermal solution where you can apply thermal boundary conditions and loads and solve for temperature. You then attach a static structural sot it in the project window, and it automatically applies the temperatures as structural loads. If you know the working temperatures to an acceptable level of certainty, then apply them directly. Otherwise, consider running thermal first.

2 If you want control over the element choice, run the analysis in MAPDL, aka Ansys Classic, Blackscreen, etc.

3 Definitely read and understand your code requirements before you start modeling. It will save much pain, anguish and wasted effort.

Rick Fischer
Principal Engineer
Argonne National Laboratory

 

[Staszkinson]

Hello,
I decided to perform simplified analysis without CFD analysis.

I would like to ask about element type and modeling in WB.

I was going to model my structure using only surfaces (for shell element purposes), but I need to take into account thermal gradients (different temperatures on both sides of my shell).
1/ I thought about modelling my strucure using surfaces and SHELL131 finite element, but I'm not sure if I can in WB apply different thermal conditions as the structural loads on both sides of my shell elements.
2/ Otherwise, there is a second option - use solid elements and then apply thermal conditions on each surface. Am I right? What element type in this case should I consider?

 

[Staszkinson]

Correction 1/:
I mean SHELL181 element.

 

[rickfischer51]

Apply your Thermal Condition. In the details, note the line Shell Face says both. Click on both and adjust it to top or bottom. To determine which side of a surface is top, click on it. The green side is top. Once the thermal condition is set, clicking on the thermal condition in the tree will turn the chosen side red.

Rick Fischer
Principal Engineer
Argonne National Laboratory

 

[Staszkinson]

Thank you very much.