Compressible & thermal energy

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

 August 12, 2013, 02:56 Compressible & thermal energy #1 Member   Marco Join Date: Jul 2013 Location: Italy Posts: 36 Rep Power: 5 Hallo Everybody I'm trying to simulate a simple compression of a closed domain due to increasing temperature of the fluid. I'm using CFX The fluid is air perfect gas, total energy model The domain has one wall at fixed temperature. The solution does't show any variation of pressure, Why ??? There are several tutorials that show the buoyant behavior of the fluid but the models use air at 25° and thermal energy model. These condition make the fluid incompressible and I don't whant this. Any advice ???

 August 12, 2013, 06:24 #2 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,707 Rep Power: 98 Can you post an image of what you are modelling and the CCL?

August 12, 2013, 06:37
#3
Member

Marco
Join Date: Jul 2013
Location: Italy
Posts: 36
Rep Power: 5
Hallo Glenn
here the ccl with the domain:

There is a simple closed cilinder with one wall at 900K
My opinion is that the fluid should increse temperature and pressure with time
Attached Files

 August 12, 2013, 06:47 #4 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,707 Rep Power: 98 How big is the chamber? Is 60s long enough to get significant heat in there anyway?

 August 12, 2013, 06:52 #5 Member   Marco Join Date: Jul 2013 Location: Italy Posts: 36 Rep Power: 5 The camber is 80mm long with 80mm diameter I think that is common sense that you have a wall at 600°C in a camber like this for one minute some variation should be happen....

 August 12, 2013, 07:49 #6 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,707 Rep Power: 98 Sounds like you are right. Don't forget that you had not stated the size previously - if the chamber was 1km square then you definitely were not heating for long enough. Can you post an image of what the temperature does look like in the post processor and your output file?

August 12, 2013, 10:41
#7
Member

Marco
Join Date: Jul 2013
Location: Italy
Posts: 36
Rep Power: 5
The results immage are at 6 sec of the solution,
while I'm writing the solution is going on.

Temperature in the contour you see stratified and pressure with full color.
You see the temperature vary very little and only near the wall

The pressure is uniform and it is realistic.

But on my opinion the wall at 900K should tranfer heat by conduction and by radiation, the convective contribution is disabled by settings (buoyant).
So due to radiation the temperature of the gas should be increased also far from
the wall at 900K and the most important thing is that 6 second increase more the temperature than we see in the simulation.....
Attached Images
 untitled.jpg (95.4 KB, 9 views)

 August 12, 2013, 10:43 #8 Member   Marco Join Date: Jul 2013 Location: Italy Posts: 36 Rep Power: 5 for the output file I'm running inside ansys and I don't know exactly what is the file you mean, sorry, if you can say me the extention I will find it....

 August 12, 2013, 18:27 #9 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,707 Rep Power: 98 Heat transfer occurs by conduction, convection and radiation. You have disabled buoyancy so convection will not happen. Unless you have used a radiation model then radiation will not happen either. So the only heat transfer mechanism you are modelling is conduction. Air has very low conductivity - so I would expect your chamber to heat up very slowly if that is all which is heating it. So if you want this model to be more realistic then enable buoyancy. This will be the primary heat transfer mechanism in a flow like this. If the gas is transparent (and air is generally assumed to be so) then radiation will not heat the gas - so why do you say radiation will affect things?

 August 13, 2013, 03:06 #10 Member   Marco Join Date: Jul 2013 Location: Italy Posts: 36 Rep Power: 5 You are right, the radiation is disabled, I've seen some tutorials that expain this. I thought the raiation of a wall at fixed temperature was calculated automatically, I was wrong. So, this simulation should be an experiment to understand external heating excage for a colsed volume like a Stirlig motor. You advice to enable buoyancy, and I will do, but, I've another question. Immage to have only one heated wall like this example, the radiation of this wall will not affect air because it is transparent, but will be absorbed from other wall. I can assume an emissivity of 0.5 for example. The other wall will be heated by radiation, how can I model this behavior ??? Will CFX calculate this automatically setting a value of diffuse fraction ???

 August 13, 2013, 03:22 #11 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,707 Rep Power: 98 There is no heat transfer to a transparent gas. Or is there particles in the gas to absorb radiation? Or is the gas not transparent? You could model the radiation to heat up the chamber walls. You will then need to model them as solids. This is pretty easy to do, use the discrete transfer radiation model. Also have a think about whether you need to model radiation at all, you could just replace it with a heat flux - provided you know the heat distribution accurately enough.

 August 13, 2013, 03:23 #12 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,707 Rep Power: 98 But I suspect you will find the key heat transfer mechanism will be convection. So it is essential that you include gravity and any other fluid flow which is present.

 Tags cfx, cfx & air content

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Herold CFX 7 June 20, 2012 18:36 Joseph CFX 14 April 20, 2010 15:45 vijeshjoshi23 Main CFD Forum 0 October 8, 2009 02:29 prayskyer CFX 2 June 19, 2006 19:52 Arnold Free Main CFD Forum 0 August 10, 1999 10:18

All times are GMT -4. The time now is 14:16.