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

HVAC Modeling Humans in Room

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 21, 2009, 17:41
Default
  #21
New Member
 
David
Join Date: Apr 2009
Posts: 13
Rep Power: 9
LilBort is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Hi,

"The inlets and outlets have fixed velocities, and the room should pressurize." - this sounds like rubbish to me. The room will just keep increasing in pressure as time progresses. If you want to want to pressurize the room you need to specify the inlet and outlet flow curve and any leakage paths. Then the room will naturally find its pressure level between the inlet and outlet.

"I am considering turning radiation off all together" - work out the radiation heat fluxes. If they are insignificant compared to the convection and conduction fluxes then yes, turn them off.

"Once I get my model to run correctly I will increase the number of loops" - this is not a good way of quickly getting a starting point. You need the timesteps to come close to converging or you can get very misleading results. Use a max coeff loops of 10 or more right from the start.

"I increased the memory allocation because I was getting overflow errors" - then fix the overflow errors. This shows there is something seriously wrong with your model and you only been lucky that increasing memory allocation allowed it to continue. I doubt the results are sensible, you could get anything.

Glenn Horrocks

Glenn Horrocks

I have given your comments consideration, and I have chosen to set my return outlets with 0 Pa relative pressure to keep the room from constantly increasing in pressure.
LilBort is offline   Reply With Quote

Old   April 21, 2009, 17:47
Default
  #22
New Member
 
David
Join Date: Apr 2009
Posts: 13
Rep Power: 9
LilBort is on a distinguished road
Quote:
Originally Posted by Simulation Engineer View Post
Hi - a couple of thoughts and maybe you already have these:

Did you set up Domain Interfaces of solid - fluid type between all the solid cylinders and air in the room?

did you use buoyancy and set gravity vector direction and ref density for fluid?

did you use Air Ideal gas model for air if it is natural convection?

- How do you set domain interfaces between solid and fluid domains?

I have since redesigned the mesh to include the humans and room all into one domain. I will not have a humans domain, just cylindrical indents in the floor of the room. And I will set a heat flux on the cylinder surfaces. But it would be nice to be able to add additional domains after the fact, so that I do not need to redesign the mesh every time I need at add people or equipment to the room.

- Yes, yes and yes. Displacement ventilation relies on the physics of buoyancy to stratify the room air into a temperature gradient. Cold air comes in near the floor and when it hits a heat source the hot air rises to the ceiling moving contaminants with it. This is why there is a noticeable temperature gradient from ceiling to floor.

- Yes I am using Air Ideal Gas
LilBort is offline   Reply With Quote

Old   April 21, 2009, 22:08
Default
  #23
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,397
Rep Power: 96
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Hi

You don't need to remesh. In CFX-Pre just delete the solid domains. You just won't use that bit of the mesh.

Glenn Horrocks
ghorrocks is offline   Reply With Quote

Old   April 22, 2009, 08:53
Default
  #24
New Member
 
David
Join Date: Apr 2009
Posts: 13
Rep Power: 9
LilBort is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Hi

You don't need to remesh. In CFX-Pre just delete the solid domains. You just won't use that bit of the mesh.

Glenn Horrocks

When I do this, I get the Isolated Fluid Regions Error.
LilBort is offline   Reply With Quote

Old   April 22, 2009, 20:23
Default
  #25
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,397
Rep Power: 96
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Hi,

The isolated fluid regions warning is saying you have two or more domains which are not connected in anyway. This means that you have not properly deleted the solid region. You can delete it either at the mesh level (on the top of the tree in CFX-Pre) or at the domain level by not specifying any domain to use the solid region, then deleting the default domain which is generated to use the solid domain.

Also - Don't use air ideal gas for buoyancy unless you have large temperature/pressure variations. Use an incompressible flow with the thermal buoyancy coefficient set instead.

Glenn Horrocks
ghorrocks is offline   Reply With Quote

Old   May 11, 2009, 05:29
Default
  #26
New Member
 
Join Date: Mar 2009
Location: Spain
Posts: 4
Rep Power: 9
pulgarcito is on a distinguished road
Hi to all,

I dont understand your interesting in simulate solid regions. Just simulate only fluid domain and represent human bodies as a wall using heat flux (total or convective deppending if you plan to simulate radiation or not). In my experience, displacement ventilation simulation works great with boussinesq aproximation for buoyancy. You will encounter more numerical stability using boussinesq rather than real gas state equation.

perhapls helps you to run calculations in transient mode, reducing g value to add an extra "relaxation" for momentum equations. Then increase g value untill the desired conditions.

Sorry for my english

Regards

Quote:
Originally Posted by ghorrocks View Post
Hi,

The isolated fluid regions warning is saying you have two or more domains which are not connected in anyway. This means that you have not properly deleted the solid region. You can delete it either at the mesh level (on the top of the tree in CFX-Pre) or at the domain level by not specifying any domain to use the solid region, then deleting the default domain which is generated to use the solid domain.

Also - Don't use air ideal gas for buoyancy unless you have large temperature/pressure variations. Use an incompressible flow with the thermal buoyancy coefficient set instead.

Glenn Horrocks
pulgarcito is offline   Reply With Quote

Old   May 29, 2009, 06:31
Default
  #27
New Member
 
Join Date: Mar 2009
Posts: 8
Rep Power: 9
Blob is on a distinguished road
Hi, maybe you've resolved all the issues by now, but I had a few thoughts. From your simulation screen shots, it seems like the stratification interface is a little low and there is too much mixing. Did you set the inlet volumetric flow rate correctly relative to the heat flux entering the room? Also, what kind of turbulence model are you using?
Blob is offline   Reply With Quote

Old   July 31, 2009, 11:08
Default asking the same problem
  #28
New Member
 
dss
Join Date: Jul 2009
Posts: 25
Rep Power: 8
flyingd is on a distinguished road
Quote:
Originally Posted by pulgarcito View Post
Hi to all,

I dont understand your interesting in simulate solid regions. Just simulate only fluid domain and represent human bodies as a wall using heat flux (total or convective deppending if you plan to simulate radiation or not). In my experience, displacement ventilation simulation works great with boussinesq aproximation for buoyancy. You will encounter more numerical stability using boussinesq rather than real gas state equation.

perhapls helps you to run calculations in transient mode, reducing g value to add an extra "relaxation" for momentum equations. Then increase g value untill the desired conditions.

Sorry for my english

Regards
I meet the same error,but if there is no free surface the model is ok.
why:
flyingd 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
HVAC modeling problem David CFX 4 April 21, 2011 09:00
modeling objects in room airflow ahmet FLUENT 2 February 21, 2007 21:41
Modeling Flow/Saturation/Absorption in Fibers Gene Dougherty Main CFD Forum 0 June 6, 2003 14:49
Contaminant Distribution in Air-Con Room Jules FLUENT 0 June 13, 2002 10:57
Contaminant Distribution in Air-con Room Jules Main CFD Forum 0 June 13, 2002 10:55


All times are GMT -4. The time now is 11:06.