Sequentially coupled thermal-stress analysis in Abaqus

[GandalFEM]

Hi, I am getting a weird result where the part that has no temperature change is shrinking (drop in temperature).

The result from thermal analysis was spot on, but when the result was applied (ODB file to predefined field) to the static analysis the expansion of my part simply doesn't make sense at all.

However, when the temperature (NT11) result looked alright in the static analysis result. So I am confused even more.

I am using steady-state in the step for both thermal and stress analysis.

Did this happen to anyone? Please help..

 

[FEA way]

What is the reference temperature for thermal expansion ? Is initial temperature field also defined ?

 

[GandalFEM]

Hi FEA way,

Thanks for such prompt reply! I used predefined field to give initial reference temperature of 298K. My model is two parts: internal and outer part. Internal part has temperature of 50K (given by BC) and outer part is at 298K. The result from post-thermal static analysis show severe shrinkage and extremely high stress at outer part more than the internal part, which is what troubling me..

Please let me know if you need further explanation!

Thanks..!!

 

[FEA way]

By reference temperature, I meant the one specified in material properties for thermal expansion. By default, it's zero.

 

[GandalFEM]

Oh I see!! I gave it a try using 298K as a reference temperature but still no luck. However, I was able to get fairely reasonable result using coupled thermo-mechanical analysis with the same conditions.

I am using 1.15E-005 as thermal coefficient of stainless steel. I believe all the material property are accurate as well..

Please let me know if you have any idea or things for me to try!

Thanks!! I really appreciate your help sir.

 

[GandalFEM]

It seems like there is an error when sequencial thermo-mechanical analysis performed using shell model in Abaqus.

As shown in the pic below, the outer part that has no temperature change thus should show no displacement shows large displacement and extremely high stress.

Perhaps there is an error for retreving nodal temperature data in predefined fields...

 

[FEA way]

Can you share the file (possibly .cae) ?

 

[GandalFEM]

Yes, of course!

I had to quickly remake the example. Strangely, the result is slightly different because the inner part shrunk as it should instead of outer part (which was happening constantly). However, unreasonably high stress is observed even though they are free surface where the stress should be 0. Even if they are not free surface, outer part should be 0 since there is no temperature change..

Please see the CAE file in the attachment.

Thank you very much!!!

Link

 

[FEA way]

It should work if you:
1. Add an initial temperature of 298 K to the thermal analysis.
2. Specify all the active temperature degrees of freedom (11, 12, 13, 14, 15) in boundary condition definitions in the thermal analysis.
3. Remove both predefined temperature fields from the static analysis and define only one for the Initial step, setting the increment from which to read to 0.
4. Use the Predefined Field Manager to modify the aforementioned temperature field to specify begin increment = 1 and end increment = 1.

 

[GandalFEM]

Hi FEA way,

I can not thank you enough for your help!! Your method allowed only internal part to deform as it should! However, unreasonably high stress is observed in internal part even though its a free object where no stress should be formed due to thermal expansion or contraction.

Would you know any reason why?

I have attached the CAE file and ODB result for your reference.

Thank you so so much...!!!!!!!!!

 

[FEA way]

Instead of leaving the part completely unconstrained, try applying minimal constraints (just to remove rigid body motions without causing thermal stresses) such as symmetry on 3 orthogonal faces. This should help.