|
[Sponsors] |
August 11, 2013, 23:47 |
Heat transfer CHT in ansys CFX
|
#1 |
New Member
Shaheen
Join Date: Aug 2013
Posts: 8
Rep Power: 12 |
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. |
|
August 12, 2013, 02:47 |
|
#2 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,695
Rep Power: 143 |
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. |
|
August 12, 2013, 06:21 |
|
#4 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,695
Rep Power: 143 |
You will also need solid to solid interfaces. Did you put them in too?
|
|
August 12, 2013, 16:38 |
|
#5 |
Senior Member
Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 361
Rep Power: 14 |
You also need to enable conservative interface flux at the interfaces.
|
|
August 12, 2013, 23:30 |
|
#6 |
New Member
Shaheen
Join Date: Aug 2013
Posts: 8
Rep Power: 12 |
I have put solid to solid and fluid to solid interfaces and enabled conservative heat flux between them.
|
|
August 12, 2013, 23:32 |
|
#7 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,695
Rep Power: 143 |
Can you post an image of the temperature distribution you do get (from the post processor) and your CCL?
|
|
August 12, 2013, 23:48 |
|
#8 |
New Member
Shaheen
Join Date: Aug 2013
Posts: 8
Rep Power: 12 |
|
|
August 13, 2013, 00:00 |
|
#9 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,695
Rep Power: 143 |
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. |
|
August 13, 2013, 00:08 |
|
#10 |
New Member
Shaheen
Join Date: Aug 2013
Posts: 8
Rep Power: 12 |
Thanks for the nice explanation .I will recheck every input and get back asap.
|
|
August 13, 2013, 03:29 |
heat flow calculation
|
#11 |
Member
|
[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 |
|
August 13, 2013, 05:51 |
|
#12 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,695
Rep Power: 143 |
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.
|
|
August 14, 2013, 00:01 |
|
#13 |
New Member
Shaheen
Join Date: Aug 2013
Posts: 8
Rep Power: 12 |
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. |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
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 18:58 |
STAR, Fluent, CFX and conj. heat transfer | star-user | Main CFD Forum | 8 | January 21, 2003 00:07 |