sequentially coupled analysis

[mvp23]

In a sequentially coupled thermal stress analysis , once the thermal part is complete , should the temperatures be fed into the structural analysis using a predefined field in the ' Initial Step ' ? I just wish to clarify .

thanks

 

[corus]

Yea, or within the step.

Tara

http://tinyurl.com/4ydjg7m

 

[mvp23]

Thank you

 

[mvp23]

corus ,

this is with reference to another thread that I had started. (

http://www.eng-tips.com/viewthread.cfm?qid=300206&page=1)

In simulating a uniform radially outward heat flow through concentric tubes (snug fit ) , I find that the values HFL1 and HFL2 vary which cause small oscillations in the HFL magnitude as well. I haven’t performed the stress analysis after transferring these values as I know the varying directional heat fluxes will cause the directional stresses and contact pressures to vary as well .
Could this be due to the elements being used ? I tried various element combinations
- hex mesh , quad elements for heat transfer
- hex mesh , linear elements for heat transfer
- tet mesh , quad elements for heat transfer
- tet mesh , linear elements for heat transfer
- inner tube – tet mesh quad heat transfer elements
- outer tube- hex mesh quad heat transfer elements
But none of these seem to iron out the directional HFL ‘noise’ on the surfaces. I’ve run extremely huge meshes as well , but it doesn’t seem to make any difference .

I learnt that quad elements model curved surfaces accurately , but at times give problems in transmitting loads due to a force acting in the opposite direction ( to the applied load ) in the corner nodes. However , when I just take a single tube , use quad elements , the results are perfect with uniform values .
This also makes me think that the contact might be causing issues. If you could look at my contact definitions in the cae file I have posted on the other thread it would help me iron out possible problems.

Here is an attached pic of the HFL1 contours of the assembly which I’m pretty sure is wrong . Also , if you notice in Figure 1 and Figure 2 that there isn’t much of a difference after the coordinate transformation. I don’t know if the transformation is being done as it should considering my temperature values are constant throughout and hence the heat flux values should be constant as well . Figure. 5 shows a similar trend as Figure 2. However the plot becomes better with the transformation . Again , is Abaqus unable to transform surfaces that are in contact or is there a special way to do this. I guess I’m looking at this issue from all angles .

 

[mvp23]

Here is the picture just in case you are unable to open the previous one.

 

[corus]

From memory your problem should be modelled as 2D axisymmetric. I'm not sure why you've chosen to model the whole 360 degree cylinder, unless you have to apply some asymmetric loading to the cylinder at some later stage. Use 2D axisymmetric geometry first, and use a finer mesh to get good results, before comparing the results to the 3D model. You can always rotate the contour plots from a 2D axisymmetric job so that they appear as coming from a full 360 degree cylinder. This is useful for showing results to management who have problems leveraging their brains out of their backside.

With contact problems I've always found it better to use linear elements, and never to use tet elements unless there is no other way out of it. Never ever use linear tet elements, unless it's for pure thermal analyses. Which ever elements you use it's better to have similar mesh densities on both contact faces.

Tara

http://tinyurl.com/4ydjg7m

 

[mvp23]

Yes , you had mentioned before that I use a 2D axisymmetric approach. The reason behind doing a full blown 3D analysis is two fold
1. These cylinders , once assembled , are welded at the ends. The stresses at the weld is included within the scope of the analysis. This would give us an idea of the type of weld required.

2. In another analysis I will be including a foil between these cylinders and it's geometry can be best described as a 270 degree revolved object. Hence I decided to go with a 3D model as it would make things easier later on.

Also , do you think that using a 3D revolution would be a better option to create my cylinders rather than a 3D extrusion ? Could that be the cause of asymmetric directional heat fluxes?
Anyway , I will try out the axisymmetric approach and fill you in .

Thanks for the help

 

[mvp23]

Yeah I did the 2D axisymmetric analysis and was looking to do a symmetric model generation to convert it to 3D , but the user's manual states that the symmetric model generation cannot be used for models defined in terms of an assembly of part instances.
So I guess this option is ruled out ?