Temperature rises with timestep
1 Attachment(s)
Hallo,
a brief introduction to my CFDModel: I am investigating an enclosed rotating disc at ReNumbers above 2E 8. The setup consist of one fluid (CO2) and two solid domains (Rotor,Stator). The RotorFluid Interface is a Frozen Rotor Interface with No Slip Walls. The disc is rotating with an angular speed of 5000 rev/min. The CO2 is assumed to be an ideal gas at 40 bar. I used a general wall distance of 0,01 mm. This yields to y+ values from approx. 10 to 100. For the outside surfaces of the stationary housing (Stator), I assumed a temperature of 20°C and a Heat Transfer Coefficient of 5 W/(m²K). I included the Viscous Work Terms and used the SST turbulence model with Curvature Control and Automatic Wall Treatment.  From correlations, it is expected that the friction based torque is about 88 kW. The CFD simulation seems to represent physical correct flow conditions (Core Rotation Factor near 0,4) and estimates the torque with 86 kW. But the solution has not converged yet. I changed the timestep to 0,1s to speed up the convergence, this leaded to a temperature gain from 430K to over 515K. The temperature still increases. But if I shorten the timestep to 0,001s the temperature seems to be stable. Maybe the assumption of a constant Heat Transfer Coefficient for the outside walls is inaccurate and there is probably to less heat leaving the inner fluid domain. I have no idea, maybe anybody can give me a hint. 
Real Gas properties?
Maybe I can't Assume an ideal gas, because the CO2 is in a supercritical state, but at least I should get an finite temperature.

If CO2 is supercritical then you cannot use ideal gas. Need a better properties model then that.
You need to correctly set up the heat so it can reach a steady state. The heat is generated by friction, so where does it go? Until you model that you have no hope. Also, a disk spinning in a fluid region does not need rotating frame of reference. This can be done simply with a tangential velocity on the wall. This would simplify things quite a bit. But your general question seems to be an FAQ: http://www.cfdonline.com/Wiki/Ansys...gence_criteria 
Thank you ghorrocks.
Yes, it is mentioned in the FAQ that I also have to check the physics. It also seems to me, that the biggest source of error is the fluid property model. Quote:
I actually get temperatures above 1000 K! At this point, it is clear that my simulation is erroneous, but I am curious if it reaches a steady state. Quote:
What is the difference between the two setups? Is it less expensive in terms of simulation runtime? 
If you do not need a rotating frame of reference then your simulation will be much simpler to set up and a reasonable amount faster to run.
Can you post an image of what you are simulating? 
1 Attachment(s)
I am using different hexa meshes interconnected via interfaces. Then I prefer to resume with a stationary domain and set the boundary condition to No Slip Wall with Wall Velocity.
Please find the picture of my simulation case study below. As you can see, I have to simulate a whole 90°C segment, because later there will be a cooling duct on both sides of the stationary housing. At the moment I want to simulate the free convection. The question is: How can I set up the heat correctly? 
Some questions:
* Why are you modelling the solids? Do you want the heat transfer in the solids? Do you need to model both the housing and the rotor? * If you do not need to model heat transfer int he rotor then this can be modelled as a single stationary frame of reference model. No need for rotating domains. Replace the rotor with a tangential velocity on the walls of the rotor. * I presume the outer surfaces are convective and the rotor generates heat. So the thing should dissipate heat to the convection boundary. 
Yes, I want to simulate the heat transfer. Therefore I have to model the housing and the rotor as a solid. The flow is driven by the rotor, that generates heat that is tranfered into the fluid domain. The surfaces are convective. The temperature distribution in the rotor is also important for me.

Just because you want to model heat transfer does not mean you have to model the housing and rotor. You would only model the housing and/or rotor if there was a nonuniformity in the heat transfer in that body which meant a simple heat transfer BC on the surface is inadequate.
OK, so if the heat distribution is important then you definitely need to model the rotor. In that case you will need CFX V14 as that is the first version which supports convection of heat in a solid due to rotation. As as for your original question  the temperature is defined by the balance of heat in and heat out. Heat in is due to viscous drag  you will need a reasonable fluid model for that. Heat out is due to convection on the outsde  you will need an accurate heat transfer condition on the outside. This is pretty obvious, but until these two fundamental parameters are correct you will never be accurate. 
I am currently using V14. Is there any new option that I can tick on in my simulation model?
My first aim is to achieve an initial result without taking account on accuracy. So the ideal gas approach is definitely wrong, but about what inaccuracy we are talking about? Maybe + 20 kW on friction torque power for instance, I don't know. The outside surfaces will be cooled later on. But for the moment I want to know, what Temperatures will be created in the solids without cooling them. 
I have never used the solid rotating domain option. You wil have t figure that one out.
Also I have no idea about what accuracy using an ideal gas rather than a real gas would be. It depends on how far you are from an ideal gas. You will need to specify some sort of external temperature condition as otherwise the temperature will just keep on rising forever. 
So I need more accurate Boundary assumptions:
1. Fixed Temperature > What temperature level? 2. Heat Flux > No reference values available 3. Heat Transfer Coefficient and outside Temperature > Outside temperature known but Heat Transfer Coefficient unknown I have no idea at the moment. 
You have to know what is going on outside the housing. Is it mounted in something which would take heat away? Is it hot enough that radiation is important? Is it still air? Air conditioning? Forced air cooling?
You can estimate the appropriate heat transfer boundary when you know what is there. If you don't know then you have no hope  unless you know what temeprature the rotor is meant to be and just try a range of settings until you get one which looks about right. 
The outside is still air at 20°C. Do I have to model the surrounding air to? Thought that 20°C and 5 w/(m²K) would be good initial approach, but cannot get a steady state with that.
If I apply a fixed temperature of 14 °C on the walls (that is, I cool down the housing with water for instance) I get a steady state. But how can I simulate free convection to the sourroundig area? 
1 Attachment(s)
I have an internal physical flow boundary that provides my wall temperature Tw. The outside temperature is T0 = 20°C. From the Ansys Help I extracted that the total heat flux qw is calculated with qw=hc*(T0Tw) = qrad + qcond.
I am interested in qcond, since qrad is probably insignificant because of probably low temperatures in the solids. For the external heat transfer coefficient hc I assumed 5 w/(m²K). From my understanding, there is a significant delta T that should lead to a heat flux that is directed towards the outside faces. But I find it thoughtprovoking that Ansys states that the wall is not modelled in full domain. If I understood it correctly then I cannot use this type of boundary condition for a CHTSimulation, because Tw is taken from the inner solid domain edge and not from the fluid domain edge. 
5W/mK is a reasonable estimate for still air. But note you could easily have an error of 50% here as it is just an estimate and heat transfer can vary widely. That will affect your final temperature significantly.
The difficulty in getting convergence with a convective BC is probably just due to it being a less constrained boundary (you still have a temperature degree of freedom at the boundary). But it should not be too difficult to fix this and you should be able to get it to converge easily enough. Quote:
This diagram is not applicable to your case. The diagram shows how a convective boundary is put on a fluid domain. You are putting it on a solid domain. So in your case the wall is modelled. 
All times are GMT 4. The time now is 01:26. 