Model Conduction as Convection

[Lurg]

Hello, I am having trouble with the meshing of a model to which I want to apply a thermal load and make a transient analysis.
I thought of simulating only one part of the whole model adding a convection boundary condition in the edges that will act as a substitute of the material that I have not modelled and the conduction it implies.

I will try to explain again in case it is not clear.

I have a circular model to which I want to apply a termal load.
Since the mesh I need is too small and i can't use more tan 260K elements/nodes i thought of modelling only a small segment.
To simulate the rest of the model i would like to apply in the edges a convection boundary condition equivalent to the conduction of the material.

My question is, Is this posible? to add a convection boundary cindition that is equivalent to the conduction of the material.
Also, How can i calculate the film coefficient equivalent to the conduction?

Thanks in advance.

 

[L_K]

Better option would be to use either symmetry boundary condition or
create an axisymmetric analysis. Of course this requires both the geometry and loads to be symmetric.

 

[scheah]

Instead of trying to manually define conduction/convection to substitute non-modeled parts, cyclic symmetry is perhaps what you're after. Assuming you are working in workbench, these links may help:
[URL unfurl="true"]https://www.simutechgroup.com/tips-and-tricks/fea-articles/246-fea-tips-tricks-ansys-cyclic-symmetry[/url]
[URL unfurl="true"]https://www.youtube.com/watch?v=EBa7_R6cVxc[/url]


Best regards,
Jason

 

[Lurg]

Thank you both for your answers, I will answer you in order.

L_K (Structural) 20 Jun 17 12:16

Better option would be to use either symmetry boundary condition or
create an axisymmetric analysis. Of course this requires both the geometry and loads to be symmetric.

A symmerty boundary condition would be great. As far a as I know it means that in the elements where you define this symmetry boundary condition ANSYS will supose the same conditions un both sides of the symmetry boundary in every time step.
I would like to apply this but I can't find any info in the ANSYS guides nor in google. An explanatory link would be very helpful but i will try to look for it myself too.
FYI my model is totally symmetric but the loads are not necesarily symmetric and also they move every load step.
I will add some captures to ilustrate. In the images only half of the model has been Meshed and the mesh is a lot coarser tan the one I would need.

sk_cheah (Structural) 20 Jun 17 12:53

Instead of trying to manually define conduction/convection to substitute non-modeled parts, cyclic symmetry is perhaps what you're after. Assuming you are working in workbench, these links may help:

https://www.simutechgroup.com/tips-and-tricks/fea-articles/246-fea-tips-tricks-ansys-cyclic-symmetry

https://www.youtube.com/watch?v=EBa7_R6cVxc

Best regards,
Jason

I have already tried the Cyclic symmetry but unfortunately the ansys guide that explains it says specifically that with the termal DOF is not posible to apply cyclic symmetry.
Thank you anyway, this would have been a perfect solution. What I am trying to do is the Cyclic symmetri but manually.

 

[scheah]

...but unfortunately the ansys guide that explains it says specifically that with the termal DOF is not posible to apply cyclic symmetry.

I was surprised by this statement. The help document seems to say thermal DOF is possible. I was able to run a simple thermal transient cyclic symmetry model by applying a small heat flux on a small area on the inner diameter.

Best regards,
Jason

 

[Lurg]

Okey, thanks for the clarification.
I will try to do it in my model.
Anyway i just want to explain myself by saying that i saw that statement in an ANSYS guide, specifically the ANSYS Mechanical APDL Advanced Analysis Guide.

I hope I will be able to do it in APDL.

Thanks again for the interest!

 

[Lurg]

Hello again.
I have also made a simple model in ansys but I have recieved this two error messages.

I am using the Academic version of the ANSYS Mechanical APDL 17.2. This is the one I have available and maybe this is the problema, that the transien termal analysis is not available in this version.

Thank you anyway!
If I finally get to solve this I will post the solution I found.

 

[L_K]

If the loads are not either plane symmetric or cyclic symmetric you are forced to model
the whole geometry. In that case, in order to decrease element count, you could refine the mesh
where needed. If the nodal temperatures are of interest, good results (mesh convergence) can be achieved with
relatively large elements.

 

[scheah]

Lurg,

Instead of Ansys Classic, can you do it in Workbench instead? Attached is the ds.dat file generated by Workbench of the example created earlier. Note that it doesn't use any cyclic symmetry commands. Instead, it uses [tt]CP[/tt] to link the high and low side (pictured below).

A possible solution to explore is to have matching mesh between the two surfaces, then write a script to generate [tt]CP[/tt] pairs between the corresponding nodes.


Best regards,
Jason

 

[Lurg]

I finally got to make the cyclic symmerty in APDL with the CYCLIC command but unfortunately this is not suitable for me because my loads are not symmetric.

The thing I am trying now is the one I asked in the first comment.
I am trying to model the conduction to the rest of the piece as a boundary condition in the sides where should be material.
I saw in internet you can model the conduction to another body that is in contact with your workpiece as a a negative heat flux.

I think this can be an easy and simple solution.

 

[Lurg]

I am sorry, I meant the CP commands, not the CYCLIC command.

 

[L_K]

I would at least validate results this method yields by comparing with full geometry model (coarse mesh).

 

[scheah]

I am trying to model the conduction to the rest of the piece as a boundary condition in the sides where should be material.
I saw in internet you can model the conduction to another body that is in contact with your workpiece as a a negative heat flux.

In my mind, your proposed method is complicated because you have to somehow figure out before hand how much negative heat flux exists. Also, manually defining it as homogeneous at the interface may be an artificial constraint.

An alternative is submodeling. Start with a global coarse model to calculate the interface results that would be later used in your refined model. PADT wrote a good article here.


Best regards,
Jason