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

Varying Interface Type for Same Side

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   October 18, 2017, 04:47
Default Varying Interface Type for Same Side
  #1
New Member
 
Join Date: Nov 2015
Posts: 4
Rep Power: 10
SKennedy_1 is on a distinguished road
Hello everyone,

My problem is: I have a rotor, which is partially contained by the bore walls, but also has a radial discharge port.

I normally simulate using a fluid-fluid interface between the rotor and discharge port, and assume adiabatic walls for the bore.

However I now want to include heat transfer between the gas and the bore walls, so now need to add a fluid-solid interface...this ultimately means the rotor side will have a fluid-fluid interface and a fluid-solid interface....and it's not possible to assign the same side of the domain to more than one interface.

Oh, I should also mention the rotor is moving, as the mesh changing I can't simply split the rotor wall.

Hope I've explained that Ok.
Any help appreciated.

Stuart
Attached Images
File Type: jpg Capture.jpg (62.4 KB, 10 views)
SKennedy_1 is offline   Reply With Quote

Old   October 18, 2017, 06:58
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,665
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
You do not need to model the solid to include heat transfer. You can simply assign a heat transfer boundary condition to the fluid domain face (eg convective) and it will have heat transfer.

The usual approach for modelling lobed impellers like this is using immersed solids. Are you using this approach? If not why not?
ghorrocks is offline   Reply With Quote

Old   October 18, 2017, 07:43
Default
  #3
New Member
 
Join Date: Nov 2015
Posts: 4
Rep Power: 10
SKennedy_1 is on a distinguished road
Hi ghorrocks,

Thanks for you response. I may be slightly misunderstanding what is required to undertake the simulation. I was applying similar principles of modelling a simple fluid flowing through pipe problem, in which I have modelled the solid and applied and HTC boundary condition to external wall - to eventually export to thermal analysis.

In my problem, I am modelling a screw compressor, so I was looking to replicate the above problem, except the gas being compressed isthe fluid and the casing is the pipe.

Regardless I will look to apply your suggestion.

Re immersed body - I understand this only to be used for incompressible fluids and any literature I have read indicates this is not suitable for screw compressor modelling.
regards,
Stuart
SKennedy_1 is offline   Reply With Quote

Old   October 18, 2017, 07:56
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,665
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
You can impose the HTC boundary on the fluid domain with no need for a solid domain. Do you need the solid domain for any reason? If it does not contribute significantly then do not model it.

Immersed solid - OK, sounds like immersed solid is not appropriate. So how are you modelling the motion of the rotors?
ghorrocks is offline   Reply With Quote

Old   October 18, 2017, 08:08
Default
  #5
New Member
 
Join Date: Nov 2015
Posts: 4
Rep Power: 10
SKennedy_1 is on a distinguished road
OK - cool. I included the solid domain as this will be used in the next stage of thermal and subsequently for structural. I understand the HTC to be a function of temperature, therefore if this is varying in the compression chamber, I was unsure if applying it as a BC would be appropriate.

I really need to get my head into a few more tutorials and HT theory!!

I create the deforming fluid domain in 3rd party software and import a new grid position via a user library at each time step. Quite neat - but takes a will to compute.

Cheers,
Stuart
SKennedy_1 is offline   Reply With Quote

Old   October 18, 2017, 08:13
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,665
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
OK, if you need the thermal profile for subsequent analysis then yes, you need to model the casing. But you can impose the same thermal conditions on a solid domain as a fluid domain, so keep that in mind for future analysis.

OK, so you are using the pre-defined mesh approach. Yes, this is likely to be very slow as it will need to do results interpolation every new mesh. If that is every time step then this simulation is likely to be extremely slow, and the interpolation is likely to significantly smear the variables. I would not be surprised if these problems make the approach unviable.

I think you will find CFX is not really a suitable CFD code for this analysis. You will probably have more luck with Fluent as it has overset mesh options and a few others which CFX does not have. Those approaches are likely to be better than what is possible in CFX.
SKennedy_1 likes this.
ghorrocks is offline   Reply With Quote

Reply

Tags
fluid-fluid, fluid-solid, interface

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
time step continuity problem in VAWT simulation lpz_michele OpenFOAM Running, Solving & CFD 5 February 22, 2018 20:50
Divergent temperature in chtMultiRegion(Simple)Foam akrasemann OpenFOAM Running, Solving & CFD 13 March 24, 2014 03:54
Problem with compile the setParabolicInlet ivanyao OpenFOAM Running, Solving & CFD 6 September 5, 2008 21:50
CFX Solver Memory Error mike CFX 1 March 19, 2008 08:22
Convective Heat Transfer - Heat Exchanger Mark CFX 6 November 15, 2004 16:55


All times are GMT -4. The time now is 10:38.