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

Room Enclosure AC High Wattage

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   July 8, 2020, 20:36
Default Room Enclosure AC High Wattage
  #1
New Member
 
Join Date: Apr 2020
Posts: 12
Rep Power: 2
miniseeker22 is on a distinguished road
I am trying to simulate a vehicle enclosure that has a solar load, ac convection inside, and a shelf of different volumes containing heat generation.

These results show that at steady state, the room will be filled with 25C air, but some of the items on the shelf could still be 700C? Even items that have a source of 25W are showing 254C. Could this be true?

This makes me think that the boundaries aren't sharing thermal contact like they should although I have them enabled. I even enabled the appropriate internal heat generation at each interface (fluid fluid & fluid solid) under each domain (each item is a different domain. So I'm a bit confused why the air is a solid block for the most part besides the shell edges where there is impact from solar.?

Here is a very specific example.

One of the lower boxes has its own domain and has thermal energy heat transfer in the solid models. I do not have an initialization here because it only allows temperature.

Under that box domain I have a fluid solid interface and a solid solid interface. For both of those I have a boundary source where I can say the energy total source is 25 W. Is this the correct way to do this? If I haven't mentioned something it has been untouched.

For the overall model fluid to solid interface, I have heat transfer checked and a thin material of aluminum.

I have scoured youtube and boards, but it never goes into the specifics that are causing me problems. I can't find a replication of the environment at hand.

I would really appreciate your help. The official ansys boards act like they don't even want to help you.
miniseeker22 is offline   Reply With Quote

Old   July 10, 2020, 04:44
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,306
Rep Power: 125
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
If you are modelling a normal HVAC condition and are getting temperatures of 250C then it is quite likely an interface is not set up properly. Look at the "Non overlap fractions" in the output file and results file to see if you can identify the problem. it could also be that you did not set up heat transfer correctly at the interface. For instance you may need to have some special handling of radiation heat transfer at the boundary.

Alternately this could be caused by numerical divergence. This just means your simulation is not convergening. This FAQ has tips for that: https://www.cfd-online.com/Wiki/Ansy...do_about_it.3F
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   July 10, 2020, 20:03
Default
  #3
New Member
 
Join Date: Apr 2020
Posts: 12
Rep Power: 2
miniseeker22 is on a distinguished road
Hi ghorrocks,

Thank you for your reply and suggestions.

-I looked at my non-overlap fractions and they were all zero for my fluid solid interface and solid solid interface. I wasn't familiar with this metric, but I think this is correct since everything is overlapping? Nothing is not overlapping? Please correct me if this is supposed to have value.

-I looked over the FAQ you sent. Since I am using the student version I am limited to <512k nodes and am at that limit, so if all of this is a course mesh problem then I think I'm out of luck.

-I ran it again through double precision which was a new addition. This lowered the temperatures from the huge numbers prior, i.e. ~160C for the lower wattages. I know this is still higher than expected.

-I then lower the timescale to 0.3 and then raised it to 1.5 instead of the default 1. This made the results worse.

-At this rate, I think it has to be the heat transfer interface. Can you comment specifically on the best course for the box interfaces? I have the overall interfaces and then the sub-domain interfaces for each box. Both fluid fluid and fluid solid interfaces in sub-domain only have heat transfer enabled and a source to indicate the box's wattage. Then for the overall model interface I have inserted thin materials to have heat transfer. Does this sound correct? If it does, then perhaps I need to manually check my interface groupings list.

My RMS P-Mass is the one diverging around 1e-5 while my stated limit in the model is 1e-4. The rest converge at 1e-3. Not sure if this helps to find the error.

Thank you for your suggestions!! I really really appreciate the guidance.
miniseeker22 is offline   Reply With Quote

Old   July 11, 2020, 02:32
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,306
Rep Power: 125
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
That suggests your problem is that your solution is not converged. Have another look at the FAQ, the tips it suggests will help.

Here is a summary of what to look for:
* Improve mesh quality
* double precision numerics
* smaller time step, changing to larger as the solution proceeds

If you want us to look more closely post your output file.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   July 15, 2020, 09:25
Default
  #5
New Member
 
Join Date: Apr 2020
Posts: 12
Rep Power: 2
miniseeker22 is on a distinguished road
Hi ghorrocks,

I'm finally seeing normal-ish results ( less than 55C for boxes)!! Based on your recommendations:

- reduced the mesh as much as I could under student license
-enabled double precision
-changed to smaller timestep.

The timestep is what really made a difference this iteration. When I previously tried it, I still had it too large. I read online that hvac timesteps are usually around .01-.001 and that's what helped.

For some reason, it won't let me upload the output file through the gui here. It errors out. Is there some other way to distribute it? I have better results, but still would like to know if it's accurate.

Thank you thank you!!
miniseeker22 is offline   Reply With Quote

Old   July 15, 2020, 17:53
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,306
Rep Power: 125
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
If you compress the output file you should be able to post it on the forum.

Alternately, you can edit the output file down to only the setup information and the final few iterations. That should make it small enough to upload.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[blockMesh] Simulating a room superian OpenFOAM Meshing & Mesh Conversion 3 April 1, 2015 10:21
[GAMBIT] Object in room with that object being the purpose of investigation fluentgambituser ANSYS Meshing & Geometry 3 August 24, 2011 01:52
Salome and Code Saturne simulation of simple room and objects cristian.ocnarescu Main CFD Forum 0 June 21, 2010 10:19
HVAC Modeling Humans in Room LilBort CFX 27 July 31, 2009 11:08
Server Rack in a room jayantha CFX 3 July 20, 2009 18:43


All times are GMT -4. The time now is 08:58.