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

Modelling a gas-gas heat exchanger

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

Like Tree1Likes
  • 1 Post By ghorrocks

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   January 30, 2023, 03:05
Default Modelling a gas-gas heat exchanger
  #1
New Member
 
Hossein Sheykh
Join Date: Jan 2023
Posts: 6
Rep Power: 3
Ho_Sh is on a distinguished road
Hello,

I am modelling a gas-gas heat exchanger to find the outlet pressure and temperature for hot and cold fluids. The known parameters are:

Hot and cold inlet mass flow rate
Hot and cold inlet temperature
Hot and Cold Inlet Pressure

As the outlet pressure is unknown, I want to use the pressure at the inlet BC and the mass flow rate of the fluids at the outlet BC to find the total pressure of the outlets through the simulation. In this way, I can calculate the pressure drop of the fluids.

Also, I leave the outlet temperature blank to get overwritten by the software.

I wonder if this setting is sensible in CFX?

Thanks
Hossein
Ho_Sh is offline   Reply With Quote

Old   January 30, 2023, 03:51
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,748
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Please read the section in the CFX documentation on well posed boundary conditions.

If the flows can be considered incompressible then you can model the inlet and outlets as mass flow inlets and a zero pressure outlet. This will give the pressure drop over the system at that flow rate.

If the flows are considered compressible then things get a bit more complex. We would need to know what Mach numbers it is operating at.
Ho_Sh likes this.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   January 30, 2023, 10:32
Default
  #3
New Member
 
Hossein Sheykh
Join Date: Jan 2023
Posts: 6
Rep Power: 3
Ho_Sh is on a distinguished road
Thanks, Glenn; I have run the simulation with mass flow rate to get the pressure drop but I was getting non-zero exit code: 25 and non-zero exit code: 2 and no result was achieved.

Changed the setting to the following and got some results eventually:

Hot Inlet:
Mass flow rate = 0.007
Total temperature 1040K

Hot outlet:
Opening pressure and direction
Relative pressure = 101325 pa
Opening temperature (In heat transfer section) 445K

Cold inlet:
total pressure(stable) = 286000 pa
Total temperature (in heat transfer section)= 455K

Cold outlet:
Opening pressure and direction (relative pressure = 1 atm (101325 pa))

Opening temperature = 970K

This boundary condition gave me the Maximum Mach number of 1.66 and Y+ of 649.

Can I ask if this setting sounds right? as the Mach is above 1, shouldn't I change it to supersonic?


Many thanks
Hossein

Last edited by Ho_Sh; January 30, 2023 at 12:07.
Ho_Sh is offline   Reply With Quote

Old   January 30, 2023, 15:45
Default
  #4
Senior Member
 
Join Date: Jun 2009
Posts: 1,825
Rep Power: 33
Opaque will become famous soon enough
In general, static pressure inlet conditions are not stable; therefore, I would not use it.

My advice is:
1 - Use mass flow outlet for both streams
2 - with the mass flow you can estimate the dynamic pressure at the inlet since you already know; therefore, an estimate for your total pressure inlets
3 - Similar to the total temperature condition, and I think you already estimated them in your previous simulations.
4 - compute those solutions, and verify how far the static pressures at the inlet are with respect to your known values. Once you feel comfortable with the solutions, your pressure drop is there.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
Opaque is offline   Reply With Quote

Reply

Tags
heat exchanger two fluids, heat exchangers, pressure drop

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
Modelling Heat transfer between stack and gas in Thermoacoustic Chirag2302 FLUENT 3 July 31, 2021 17:23
Fluent Heat exchanger model gimson FLUENT 0 May 10, 2021 04:30
how to set the heat transfer of the wall for compressible gas case IronLyon CFX 3 March 7, 2019 04:32
a possible substitution of heat exchanger module in fluent?! Sadegh.A FLUENT 0 September 25, 2017 15:49
Compression stoke is giving higher pressure than calculated nickjuana CFX 62 May 19, 2015 13:32


All times are GMT -4. The time now is 21:57.