Thermal stress analysis

[shahir]

Hi frds,

I am using ABAQUS CAE 6.6-1

I am simulating a Shell subjected to a temperature change(for eg., 350 to 500deg C) and with some mech BCs.

I am able to do this in a static step ,by giving initial temperature field in initial step(for eg., 350deg in predefined field1 in initial step)and and in the static step have given final temp as field 2(500deg in predefined field2 in static step)with some mech BCs.

In my results i am obtaining the temperature distibution over the step time(350 to 500deg C)

Now I want to do this as Sequential thermal stress analysis

I have modelled two different Heat transfer models with Temperature BC in Heat transfer sterand obtained two odb files got distribution of initial and final temperatures respectively(for eg.,initial odb file contains 0 to 350 deg distributionand eg.,final odb file contains 0 to 500 deg distribution)

I modelled a static analysis model and getting initial odb file in initial step predefined field and final odb file in static step as predefined field 2 with mechanical BCs.

But i am getting different stress and displacement values for both(Static models simply with temperature field and Sequential analysis(Static models with the results of heat transfer models))

I dont know why, may b the element type chosen in Heat transfer and Static in sequential analysis(i hav also tried changing suitable elements but there is no change)
hope i hav explained it in detaillll

Is there anyother way to obtain the tempeature distribution in the static step?

thx for reading the long story

i am waitig for your suggestion thx

 

[xerf]

Though, I probably did not understand what exactly you
are doing, and I do not have yet v6.6, my comment is
that in the Static step, the heat trasfer problem is not solved for. The temperature fields are used only for computing the thermal strains. The temperature fields have a prescribed variation in the static step.

If you put an initial temperature field in a heat transfer step (transient or steady state), the heat flow will be accounted for .

 

[shahir]

Thx for ur suggestion xerf

will yos suggest me a suitable step for doing my analysis?

thx

 

[xerf]

You could try using a coupled temp-displacement step.

 

[corus]

Coupled temperature/displacement can be expensive and unnecessary unless there is significant movement of components. It's better to run a sequential thermal analysis and stress analysis as you have done. There should be no problem with the elements you choose in the static and thermal analyses. If the nodes don't match then there are interpolation options for when reading in the temperatures. I find it better to create and run a thermal model and then from that thermal model simply modify the element type to a structural type element so that the nodes will match exactly when importing the temperatures.

corus

 

[barrind]

I have a related problem to this. Due to the size of my model and the memory available on my pc I run the thermal model using linear elements and it runs ok. However when I changes the elements to quads I run out of memory in the pre phase. In my final model I am only interested in the stress in a part of the model and intend to delete unwanted elemnts from the input file before running the analysis. Is it possible to use the thermal .fil file generated by the linear elemenmt model, to import a temperature field for a copied model which has had its elemnts changed from linear to quads using the interpolation option you describe?

 

[xerf]

Have you tried to increase the memory allocated by the analysis input file processor (i.e. the pre_memory variable) from the default 256Mb to a higher value ?

(If quad=quadrilateral element then by linear elements you mean (bi-)linear quads and by quads you mean (bi-)quadratic quads, don't you ?)

 

[coucy]

I'm firstly simulating a plane strain problem under a uniforme thermal field at steady state. It is evident that this problem can be given in a closed-form, but I don't know how to introduce in Abaqus the thermal boundary conditions (ex, thermal-isolating wall at steady-state, T(left-side)=Tl, T(right-side)=Tr) or other treatments... Someone can help me?

I've read documentation: *COUPLED TEMPERATURE-DISPLACEMENT,steady state. ....but it seems that it not run.

Thank a lots.

 

[xerf]

Thermally insulated boundary implies zero heat flux on that boundary.

 

[coucy]

Thanks xerf, I'm in good sense.

 

[shahir]

hi frds

thx for all ur replies sorry for the late response

i found the solution

the problem was that the number of temperature points in thermal file does not match the mechanical files

i need to specify it as piece wise linear to the number of integration points. it will be done in the Section in advanced tab option.

thx for all ur comments

bye

sheriff