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

Heat transfer CHT in ansys CFX

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 11, 2013, 23:47
Default Heat transfer CHT in ansys CFX
  #1
New Member
 
Join Date: Aug 2013
Posts: 8
Rep Power: 4
shaheen is on a distinguished road
Hi,

I have modelled a pipe in which oil is flowing at 85 deg C with 1m/s speed.There is a heater cable on the pipe to heat the oil as it flows.The heater provides 100 W/m output.The pipe and heater cable is insulated with additional layer of rockwool.

I have created seperate domains to represent fluid and solids and also verified the domain interface properties.

The problem is the oil is not heated and temperature at inlet and outlet is same.But in actual system the oil gets heated to 120 deg C.

Please can any one share their thoughts on this.
shaheen is offline   Reply With Quote

Old   August 12, 2013, 02:47
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,959
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Have you put interfaces to connect the solid and fluid domains? Also if you have multiple solid domains?

How have you modelled this? Can you show a picture which shows how you have modelled the heating cable.
ghorrocks is offline   Reply With Quote

Old   August 12, 2013, 04:22
Default
  #3
New Member
 
Join Date: Aug 2013
Posts: 8
Rep Power: 4
shaheen is on a distinguished road
Hi Glenn,

I have put interfaces to connect the solid and fluid domains with heat transfer option set to conservative heat flux.

1.JPG

2.JPG

3.JPG

I have attached images of the geometry for your viewing
shaheen is offline   Reply With Quote

Old   August 12, 2013, 06:21
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,959
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
You will also need solid to solid interfaces. Did you put them in too?
ghorrocks is offline   Reply With Quote

Old   August 12, 2013, 16:38
Default
  #5
Senior Member
 
RicochetJ's Avatar
 
Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 291
Rep Power: 6
RicochetJ is on a distinguished road
You also need to enable conservative interface flux at the interfaces.
RicochetJ is offline   Reply With Quote

Old   August 12, 2013, 23:30
Default
  #6
New Member
 
Join Date: Aug 2013
Posts: 8
Rep Power: 4
shaheen is on a distinguished road
I have put solid to solid and fluid to solid interfaces and enabled conservative heat flux between them.
shaheen is offline   Reply With Quote

Old   August 12, 2013, 23:32
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,959
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Can you post an image of the temperature distribution you do get (from the post processor) and your CCL?
ghorrocks is offline   Reply With Quote

Old   August 12, 2013, 23:48
Default
  #8
New Member
 
Join Date: Aug 2013
Posts: 8
Rep Power: 4
shaheen is on a distinguished road
The temperature distribution of oil.
4.jpg

The ccl file output
PipeHeater.txt
shaheen is offline   Reply With Quote

Old   August 13, 2013, 00:00
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,959
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
So it looks like heat is being transferred to the water, just less than you think is correct.

From your CCL I see you have a large pipe flowing water at 1m/s. This is quite a lot of water. And your heat is 100W/m. That is not much heat. My kettle at home is 2.4kW and it takes a couple of minutes to boil 0.5 litres of water. So it does not surprise me that 100W/m does not heat things up much.

Are you sure you have your geometry, flow rate and heat input correct? You really need to do some back of the envelope calculations to check you are in the right direction.

For instance, a 0.5m diamater pipe at 1m/s is 0.196m^3/s or 196 kg/s. At 4.2 kJ/kgK that works out to be 1e-4 K temperature difference averaged across the flow. That looks about what you got with CFX . So I think the simulation is accurately showing what you asked it to model.
ghorrocks is offline   Reply With Quote

Old   August 13, 2013, 00:08
Default
  #10
New Member
 
Join Date: Aug 2013
Posts: 8
Rep Power: 4
shaheen is on a distinguished road
Thanks for the nice explanation .I will recheck every input and get back asap.
shaheen is offline   Reply With Quote

Old   August 13, 2013, 03:29
Default heat flow calculation
  #11
Member
 
Karthick Selvam
Join Date: Oct 2012
Location: Germany
Posts: 48
Rep Power: 4
selvam2487 is on a distinguished road
Send a message via Skype™ to selvam2487
[For instance, a 0.5m diamater pipe at 1m/s is 0.196m^3/s or 196 kg/s. At 4.2 kJ/kgK that works out to be 1e-4 K temperature difference averaged across the flow. That looks about what you got with CFX . So I think the simulation is accurately showing what you asked it to model. ]

Dear Glenn,

Can you please tell me which formula you used to calculate the 1e-4 K temperature difference across the flow. I am interested in knowing how you included the power input value of 100 W/m in the calculation.

Regards,
Karthick

Last edited by selvam2487; August 13, 2013 at 03:30. Reason: Mistake
selvam2487 is offline   Reply With Quote

Old   August 13, 2013, 05:51
Default
  #12
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,959
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Your thing looks about 1m long so at 100W/m that is 100W. Then you have a power input, a mass flow rate, a specific heat and that defines the temperature rise.
ghorrocks is offline   Reply With Quote

Old   August 14, 2013, 00:01
Default
  #13
New Member
 
Join Date: Aug 2013
Posts: 8
Rep Power: 4
shaheen is on a distinguished road
Yes.In the actual system the pipe is long continous and oil is maintained above 85 deg and at intermediate lengths there is a supporting structure to support the pipe which is also partially insulated.At the support due to ambient conditions the oil temp drops.

The heater cable has output of 100 W/m and in operating condition the heater temperature is 92 deg.
shaheen 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
Question about heat transfer coefficient setting for CFX Anna Tian CFX 1 June 16, 2013 06:28
An error has occurred in cfx5solve: volo87 CFX 5 June 14, 2013 17:44
heat transfer in a box in ANSYS CFX 10 Igor Di Varano CFX 2 November 24, 2006 19:58
STAR, Fluent, CFX and conj. heat transfer star-user Main CFD Forum 8 January 21, 2003 01:07


All times are GMT -4. The time now is 18:16.