CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

Temperature rises with timestep

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   February 5, 2013, 12:09
Default Temperature rises with timestep
  #1
Member
 
Daniel Ceglarski
Join Date: Sep 2012
Location: Essen, Germany
Posts: 49
Rep Power: 4
Daniel C is on a distinguished road
Hallo,

a brief introduction to my CFD-Model:

I am investigating an enclosed rotating disc at Re-Numbers above 2E 8. The setup consist of one fluid (CO2) and two solid domains (Rotor,Stator). The Rotor-Fluid 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 20C and a Heat Transfer Coefficient of 5 W/(mK).

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.
Attached Images
File Type: jpg Convergence History.jpg (27.1 KB, 18 views)
Daniel C is offline   Reply With Quote

Old   February 5, 2013, 14:36
Default Real Gas properties?
  #2
Member
 
Daniel Ceglarski
Join Date: Sep 2012
Location: Essen, Germany
Posts: 49
Rep Power: 4
Daniel C is on a distinguished road
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.
Daniel C is offline   Reply With Quote

Old   February 5, 2013, 18:23
Default
  #3
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,929
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.cfd-online.com/Wiki/Ansys...gence_criteria
ghorrocks is offline   Reply With Quote

Old   February 7, 2013, 09:16
Default
  #4
Member
 
Daniel Ceglarski
Join Date: Sep 2012
Location: Essen, Germany
Posts: 49
Rep Power: 4
Daniel C is on a distinguished road
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:
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?
I assumed 20C outside temperature and a Heat Transfer Coefficient of 5 W/(mK). Even though the Heat Transfer Coefficient is pending on temperature this setup should come up to a steady state somewhere along the way.

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:
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.
Do you mean that I should change Domain Models\Domain Motion to Stationary for the Rotor Domain and set Boundary: Interface...\Boundary Details\Option to No Slip Wall with Wall Velocity (Rotating Wall)?

What is the difference between the two setups? Is it less expensive in terms of simulation runtime?
Daniel C is offline   Reply With Quote

Old   February 7, 2013, 19:56
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,929
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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?
ghorrocks is offline   Reply With Quote

Old   February 8, 2013, 03:50
Default
  #6
Member
 
Daniel Ceglarski
Join Date: Sep 2012
Location: Essen, Germany
Posts: 49
Rep Power: 4
Daniel C is on a distinguished road
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 90C 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?
Attached Images
File Type: jpg Cavity.jpg (82.7 KB, 10 views)
Daniel C is offline   Reply With Quote

Old   February 8, 2013, 05:34
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,929
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   February 8, 2013, 05:54
Default
  #8
Member
 
Daniel Ceglarski
Join Date: Sep 2012
Location: Essen, Germany
Posts: 49
Rep Power: 4
Daniel C is on a distinguished road
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.
Daniel C is offline   Reply With Quote

Old   February 8, 2013, 06:05
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,929
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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 non-uniformity 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.
ghorrocks is offline   Reply With Quote

Old   February 8, 2013, 06:21
Default
  #10
Member
 
Daniel Ceglarski
Join Date: Sep 2012
Location: Essen, Germany
Posts: 49
Rep Power: 4
Daniel C is on a distinguished road
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.
Daniel C is offline   Reply With Quote

Old   February 8, 2013, 06:57
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,929
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   February 8, 2013, 07:27
Default
  #12
Member
 
Daniel Ceglarski
Join Date: Sep 2012
Location: Essen, Germany
Posts: 49
Rep Power: 4
Daniel C is on a distinguished road
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.
Daniel C is offline   Reply With Quote

Old   February 9, 2013, 06:08
Default
  #13
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,929
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   February 9, 2013, 06:30
Default
  #14
Member
 
Daniel Ceglarski
Join Date: Sep 2012
Location: Essen, Germany
Posts: 49
Rep Power: 4
Daniel C is on a distinguished road
The outside is still air at 20C. Do I have to model the surrounding air to? Thought that 20C and 5 w/(mK) 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?
Daniel C is offline   Reply With Quote

Old   February 9, 2013, 07:07
Default
  #15
Member
 
Daniel Ceglarski
Join Date: Sep 2012
Location: Essen, Germany
Posts: 49
Rep Power: 4
Daniel C is on a distinguished road
I have an internal physical flow boundary that provides my wall temperature Tw. The outside temperature is T0 = 20C. From the Ansys Help I extracted that the total heat flux qw is calculated with qw=hc*(T0-Tw) = 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/(mK). 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 thought-provoking 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 CHT-Simulation, because Tw is taken from the inner solid domain edge and not from the fluid domain edge.
Attached Images
File Type: jpg Ansys Help.JPG (51.3 KB, 7 views)

Last edited by Daniel C; February 9, 2013 at 07:28.
Daniel C is offline   Reply With Quote

Old   February 10, 2013, 05:14
Default
  #16
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,929
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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:
since qrad is probably insignificant because of probably low temperatures in the solids.
That does not sound very confident. You need to estimate the order of magnitude of the radiative heat flux and be SURE it is insignificant.

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.
ghorrocks is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Problem with zeroGradient wall BC for temperature - Total temperature loss cboss OpenFOAM 10 March 5, 2015 07:57
Calculation of the Governing Equations Mihail CFX 7 September 7, 2014 06:27
Is wall ajacent temperature equal to conservative temperature of the wall? shenying0710 CFX 8 January 4, 2013 05:03
Inlet won't apply UDF and has temperature at 0K! tccruise Fluent UDF and Scheme Programming 2 September 14, 2012 06:08
monitoring point of total temperature rogbrito FLUENT 0 June 21, 2009 17:31


All times are GMT -4. The time now is 13:59.