Need what are the steps to follow for this “Isotropic plate subjected to thermal loading constrained at both ends”
Thanks in Advance!
Can you share more details about your desired setup ? Is purely mechanical analysis with temperature difference applied as a defined field for thermal expression sufficient ? Then see this: https://www.youtube.com/watch?v=_Bv_RD7DOtA
Aluminum plate of thickness 1 mm…for suppose 100 degree temperature was applied what are the thermal stresses on the plate when the model is constrained at both ends.
Like this ?
Plate thermal load.pmx (295.2 KB)
Almost the same. Thank you!
Plate becomes in compression and buckling mode should be checked.
Yes, you’re right.
In my case, I apply a prescribed displacement in the X-direction (a specific value in mm) to allow controlled deflection, while all other degrees of freedom are constrained.
The goal is to observe and compare the resulting thermal stresses in the X-direction for both isotropic and orthotropic materials under the same boundary and thermal loading conditions.
I’m planning to follow the approach I mentioned above. If there are any suggestions or corrections, I’d be happy to hear them.
Your file is PrePoMax v2.3.0 but it doesn’t open with that version. When closing it there is a new process running in the backwround.
FYI, i’m using the latest v2.3.6 dev…for me the file was opened
In Abaqus, thermal defined field (*TEMPERATURE) can be used with *BUCKLE. Unfortunately, CalculiX doesn’t support it: *TEMPERATURE doesn't work with *BUCKLE
I can open it back in v2.3.0, strange.
in my case i want to apply 100 degree temperature…
As shown in images 20 degree initial and 80 degree defined because of differential temp 100-20=80 degree…is this a correct way of representing 100 degree temp for the model?
This is 60 degrees of temperature increase. 20 deg is at the start of your analysis, then it reaches 80 deg at the end. So use 0 initial and 100 final or 20 initial and 120 final if you want to raise the temperature by 100 deg.
Also, notice the “Zero temperature” in the material thermal expansion definition. This is the temperature after which thermal expansion starts. So you can set it to the same value as your initial temperature if you want thermal expansion to start right after it.
Now you have a different initial temperature than the expansion reference temperature.
It will be easier in 2D (plane stress) and you don’t have to prescribe that displacement of 0.23 mm, let it occur naturally.
Plate thermal load 2.pmx (87.8 KB)
in your case the stresses are not matching right???..
Anyway i got what i am expecting…actually its the requirement to give displacement in x and check the thermal stresses.
Please refer this —
Iso_plate_thermal_Load.pmx (379.0 KB)
…next i want the same procedure to be done for orthotropic plate …for this case i think again material props should be define in calculix…how the thermal expansion should give?..any ideas will help my work..
Why ? They are exactly the same as in your SMath calculation:
PrePoMax doesn’t support orthotropic material properties yet. You will have to use the Keyword Editor for that. The syntax is:
- for orthotropic elasticity:
*ELASTIC, TYPE=ENGINEERING CONSTANTS
E_1, E_2, E_3, v_12, V_13, G_12, G_13,
G_23
- for orthotropic thermal expansion:
*EXPANSION, TYPE=ORTHO, ZERO=...
α_11, α_22, α_33
Yeah…got the stresses…i didn’t check the mises stresses..
i dont understand one thing in your model…how is this possible as the model is a shell section right?
"If possible whatever the method you have done where we got both displacement and stresses correctly..can you do the same procedure for my model which i have shared…as i am not getting the results which you got even i have modified like your model..
I used plane stress instead of 3D shell to get rid of the third dimension and simplify BCs. That’s why I applied a solid section.
The thing is that if you apply the displacement of 0.23 mm calculated from thermal expansion then you already have the displacement and stress (as it’s calculated from strain using Hooke’s law) that would result from temperature increase and you don’t need that temperature increase in an analysis anymore. Maybe run two simulations - one with prescribed displacement based on the analytically calculated thermal strain and one without it but with the thermal load.