Temperature Displacement in Abaqus

[midnighttofurun]

I have a very thin part that I need to perform a thermal displacement on in Abaqus. I need to find the displacement of a point on the part due to temperature increase. I know the initial and final temperatures and the mechanical boundary conditions (the edges of the part are mechanically fixed).

I am familiar with most CAD softwares as well as a few FEA programs. However, Abaqus is the only program available to me.

Is there an easier way to perform this analysis in abaqus other than using the sequentially coupled thermal stress analysis?

 

[MNS747]

There are some other available such as Coupled-Thermal displacement anaylsis but this will be used when heat is being generated due to mechanical stresses. As you mentioned and i feel its a basic thermal displacement analysis I would say to have the Heat transfer analysis first and then read the temperature data into your Static-General analysis.

Regards

 

[corus]

I always thought 'sequential' meant performing the thermal analysis forst and then the mechanical second, which is the normal way of analysis. Coupled temperature displacement is used when the temperatures are dependent upon the shape, ie. when contact occurs and the bounday condition changes. Temperatures generated by mechanical stresses would be included in this too.
A simpler way is to just specify the temperatures at nodes, usually when you have a uniform distribution, or some other simple form. If you're using shell elements remember that you have the variables NT11..NT15 to specify temperatures for (depending on the number of section points through the thickness). Otherwise you'll specify a temperature at point 1 with 0 degrees at all other points through the section.

corus

 

[xerf]

If you know the temperature variation, you might not need a heat transfer analysis or thermal-displacement coupled analysis but just a static displacement analysis. You need to:
-define the thermal expansion properties of the material
-define the initial temperature field
-define the displacement boundary conditions
-prescribe variation of temperature field and other mechanical loads.