CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Problem in coupling CFX and Ansys for fluid-thermal sim. (http://www.cfd-online.com/Forums/cfx/76336-problem-coupling-cfx-ansys-fluid-thermal-sim.html)

Jordi May 22, 2010 11:13

Problem in coupling CFX and Ansys for fluid-thermal sim.
 
I'm trying a coupled multiphysics simulation and have wasted about one week trying to simulate a heat transfer with convection, using Fluid Flow (CFX) and Steady-State Thermal (ANSYS) systems coupled.

My system has a solid body with internal heat generation surrounded by an air stream. My aim is to simulate the convection, not to use any data for this transfer coefficient.

At the beginning everything goes apparently ok, system linkages, geometry, meshing, set-up of systems, etc. up to the set-up cell in the thermal system. It remains with a question mark, so if I launch the solver from the Fluid system almost immediately fails.
I have tried many different choices but didn't succeed, I'm quite sure is a huge nonsense I miss once and again.

I have revised a Fluid System Interface tutorial but it's a little different from this case, it's the mechanical system that calls CFX but I have the reverse case (CFX invokes ANSYS).

I think my mistake is in the thermal (mechanical) set-up. I set the heat generation condition and then I'm not sure how to say the solver to catch data from CFX (temperature) to the solid surface. I tried:
- coupling - didn't work
- imported loads > ansoft - didn't work
- temperature - didn't find what file to retrieve data from, if any.

ghorrocks May 23, 2010 18:44

There is no need to use FSI if the body does not move. If it is coupled only with heat transfer then do it entirely in CFX using a conjugate heat transfer approach (CHT). Have a look at the heating coil tutorial example.

Jordi May 24, 2010 01:45

Yes, I know my problem does not involve FSI, I only had a look at that tutorial to learn how to set up the interaction.

I also had a look at the heating coil tutorial but (if we are talking about the same) there the convection coefficient is imposed, and that is just what I want CFX/Ansys to simulate and calculate.

ghorrocks May 24, 2010 06:49

Quote:

Yes, I know my problem does not involve FSI, I only had a look at that tutorial to learn how to set up the interaction.
I have never done FSI in ANSYS/CFX but I understand heat transfer FSI is trickier and more buggy than motion FEA.

Quote:

I also had a look at the heating coil tutorial but (if we are talking about the same) there the convection coefficient is imposed, and that is just what I want CFX/Ansys to simulate and calculate.
You cannot use a convection coefficient on the interface between a fluid and solid domain. The heat transfer is calculated as part of the simulation.

Jordi May 24, 2010 07:36

Quote:

Originally Posted by ghorrocks (Post 259955)
You cannot use a convection coefficient on the interface between a fluid and solid domain. The heat transfer is calculated as part of the simulation.

This is indeed what I want!! Not to impose any figure and get the real phenomenon simulated.

But my problem is about some tricky hidden point in the Mechanical set-up for the Steady-State transfer analysis... it remains with the question mark in the workbench. My idea is that the Thermal Analysis get the temperatures of the fluid (from CFX), calculates heat fluxes and return interface data (heat flux) to CFX where the fluid simulation updates too, but something is missing and really can't find where to look for.

ghorrocks May 24, 2010 07:50

Quote:

This is indeed what I want!! Not to impose any figure and get the real phenomenon simulated.
I don't have the heating coil example at hand, but the convection coefficient must be applied to a wall. The interface boundary condition between a fluid and solid domain by default already uses the interface condition (ie no convection coefficient) so the heating coil will be an example of how to do it.

Is there a reason you are doing this using ANSYS Mechanical? Is there something ANSYS Mechanical can do which CFX cannot with a CHT body? I don't understand your logic of using ANSYS Mechanical at all.

Jordi May 24, 2010 09:13

My aim is to simulate with FEA tools at the university (they have Ansys, all modules) a natural convection from different geometries (plates, tubes, etc. at diferent angles) to extract data and create generical correlations.
Somewhere I read a coupled multiphysics Fluid-Thermal analysis is done this way (CFX and Steady-State Thermal) but I'm not constrained to it.

Apparently it should work this way... I start with CFX then I add Steady-State Thermal Analysis:
http://www.pheromone-seduction.com/project%201.png
http://www.pheromone-seduction.com/project2.png

to get this:

http://www.pheromone-seduction.com/project3.png

I delete solution cells from the mechanical system (CFX manages global solving - read somewhere):

http://www.pheromone-seduction.com/project4.png

Then I work with geometry, etc. up to this no-way-out point:

http://www.pheromone-seduction.com/project5.png

In the setup of the thermal system, I have a heat generation and then I should put somewhere that the interface surface has a computational connection to CFX, but I can't see how... I tried almost all possibilities from here:

http://www.pheromone-seduction.com/project6.png

ghorrocks May 24, 2010 18:28

I strongly recommend you do this model in CFX only. You are just making things hard for yourself by trying to use ANSYS Mechanical to do it. It is very easy to set up in CFX, you get far better control and it will run quicker and converge better. I recommend only going to ANSYS Mechanical for stress/strain FEA.

Jordi May 24, 2010 19:58

Yes, I did a quick test and I found I can set a subdomain with a heat generation. Apparently it works, with only CFX, no MFX necessary.
I'm really happy, I used CFX for a number of problems but only for fluid flow.

Jordi May 25, 2010 09:54

Yes, it seems to work. This is a model of a solar plate heated by sun's radiation and kept in thermal equilibrium by natural convection.
This is temperature distribution:

http://www.pheromone-seduction.com/CFX1.png

this is the streamline of airflow, with temp in color:

http://www.pheromone-seduction.com/CFX2.png

and this is the air temperature at the middle plane, beautiful!

http://www.pheromone-seduction.com/CFX3.png

thanks for your help!
http://www.pheromone-seduction.con/CFX1.png

Idiom_1 June 2, 2015 04:20

Quote:

Originally Posted by ghorrocks (Post 259910)
There is no need to use FSI if the body does not move. If it is coupled only with heat transfer then do it entirely in CFX using a conjugate heat transfer approach (CHT). Have a look at the heating coil tutorial example.

Hey,

I realize that topic is very old but i try...

i got a problem with one simulation so i find that topic:
- how can I make an simulation if i want to make a move to my object and also put him heat. I mean, one wire goes through tube which is higher temperature. How can i make analysis like this and which module should i use?

Thank you for help :)

ghorrocks June 2, 2015 07:57

If the motion can be defined within CFX then do it entirely in CFX. It is always easier doing it in a single package rather than coupling multiple packages together. But if the motion is too complex to define in CFX (for instance you need FEA to define it) then you have to couple to ANSYS.

Idiom_1 June 2, 2015 09:10

In fact i didnt make any simulation in cfx yet so my question is:
is it possible to make an simulation contain move/motion solid objects and trading temperature?

If you got time, i would be so pleased if you try to help solve my problem.
Of course im a bit amateur but well.. i try.
It looks like this picture:
http://wrzucaj.net/image/mE2

One wire inside is moving through tube which have temperature like 700K.
Can I make it using transient/steady state thermal analysis + transient structural or explicit dynamics as a coupled analysis?
I tried to make it by transient thermal and then to solution put a transient structural, but my with moving solution i can see only stresses etc, not temperature. I would like to see temperature in chosen time of simulation.
Only one way to make it is use to CFX? Is not problem to use there solid materials not fluids?

Sorry for so many questions as i guess very basic level but im going to learn ansys.

Mostly tnaks for help,
greetings! :)

ghorrocks June 3, 2015 08:21

It should be possible to do this. What makes the wire move?

Idiom_1 June 4, 2015 09:47

Im not sure i got right u'r question, but answer: not matter in fact, i just i want to put velocity to surface i mark in picture. There is not any complicated system to pull wire, just taken velocity to surface or whole model.
It's not about pull it by roll or something like that, move is given to wire directly.

ghorrocks June 6, 2015 00:45

If you know the velocity in advance then you can do this with moving mesh, or possibly even just tangential wall velocities. No need for FSI.


All times are GMT -4. The time now is 12:40.