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

How to define Energy source in solid region ?

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

Like Tree6Likes
  • 2 Post By ghorrocks
  • 1 Post By ghorrocks
  • 1 Post By Rajaero
  • 1 Post By Rajaero
  • 1 Post By Rajaero

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   July 29, 2018, 11:50
Default How to define Energy source in solid region ?
  #1
Member
 
Hamda
Join Date: Jul 2018
Posts: 80
Rep Power: 7
Hamda is on a distinguished road
Hi,

In my projects, spheres (solid) are fuel element and I want to define energy source in solid region. But in CFX, unlike Fluent, there is no option to do that.

in Fluent, we can specify ONE energy source in solid region but in CFX, I have to use source point in CFX?



Thanks in advance.
Attached Images
File Type: jpg Screenshot (89).jpg (85.2 KB, 22 views)
Hamda is offline   Reply With Quote

Old   July 29, 2018, 18:30
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,703
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Yes, you can define a source in a volume region in CFX. Define the volume region as a subdomain and you will be able to define sources on it.
Светлана and Hamda like 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   July 30, 2018, 13:23
Default
  #3
Member
 
Hamda
Join Date: Jul 2018
Posts: 80
Rep Power: 7
Hamda is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Yes, you can define a source in a volume region in CFX. Define the volume region as a subdomain and you will be able to define sources on it.

Thanks a lot. As mentioned before my geometry consists of solid (spheres)and fluid (the space between spheres)domains, and I named the whole geometry, "Core". Now in "Default domain" in "location" I have 3 locations; Core, Primitive 3D (solid), Primitive 3D A (fluid). I was wondering If I am able to change the names? I want to change primitive... to fuel , etc.


Also, when I want to define fluid and particles,.. For fluid, I should choose its location (Primitive 3D A) and for solid (Primitive 3D )? I mean can I choose location, Core and then just change "domain type" and define materials for fluid and solid?
Many thanks
Hamda is offline   Reply With Quote

Old   July 30, 2018, 19:13
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,703
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
I would recommend against changing the names of the mesh regions. If you change the mesh it means it cannot update the links easily. If you change the names in the meshing software then the names will flow through to CFX - that is a better way of doing it. Alternately, when you define the domains you can call the domains whatever you like.

As for defining the regions to be fluid and solid - this is shown in the CFX tutorials. There are a few which cover CHT (conjugate heat transfer) modelling, so look to see how they set it up.
Hamda 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   July 30, 2018, 23:39
Default
  #5
Member
 
Taiwan,new north city
Join Date: Aug 2017
Location: Taiwan
Posts: 74
Rep Power: 8
Rajaero is on a distinguished road
Hi,
i agree with Glenn,
i think it is better to give name selection in the meshing itself.

Setting heat source:
1. split domain in to two parts (solid and fluid domain)
2. right click solid domain and select subdomain
3. in sub domain you can give total heat source.

Note: You should have solid-fluid interface for your problem
Thanks...
Hamda likes this.
Rajaero is offline   Reply With Quote

Old   August 5, 2018, 12:37
Default
  #6
Member
 
Hamda
Join Date: Jul 2018
Posts: 80
Rep Power: 7
Hamda is on a distinguished road
Quote:
Originally Posted by Rajaero View Post
Hi,
i agree with Glenn,
i think it is better to give name selection in the meshing itself.

Setting heat source:
1. split domain in to two parts (solid and fluid domain)
2. right click solid domain and select subdomain
3. in sub domain you can give total heat source.

Note: You should have solid-fluid interface for your problem
Thanks...
Thanks for your reply.

you say split domain to 2 parts i.e. I should define 2 domains? solid domain and fluid domain. I already did that
in sub domain I can define heat source but i have a problem with its unit! I mean my unit is (w/m3) but in CFX (W). In fluent I didn't have such problem because in it the unit was (w/m3). I should write an expression for it?

Also How can I sure that I have a solid-fluid interface for my problem? I mean I should define it in meshing stage?

Many thanks in advance
Hamda is offline   Reply With Quote

Old   August 5, 2018, 19:18
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,703
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Have a look in the CFX documentation on sources. There are a few different ways of specifying them.

For the solid-fluid interface - if you are unsure you have this correct then do some tutorial examples to see how they are set up. And if you have not set them up correctly then the temperature of your fuel spheres will quickly increase to huge temperatures as nothing is cooling it down - so it will be easy to spot if you have it wrong.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   August 5, 2018, 23:43
Default
  #8
Member
 
Hamda
Join Date: Jul 2018
Posts: 80
Rep Power: 7
Hamda is on a distinguished road
Dear ghorrocks,
Thanks, I already read CFD tutorial but I didn't find anything related to my problem (heat source). As you know Software tutorials don't cover any thing and so I have to ask my questions here and other sites. The best way to me is to use other's experience.
Thanks
Hamda is offline   Reply With Quote

Old   August 5, 2018, 23:59
Default
  #9
Member
 
Taiwan,new north city
Join Date: Aug 2017
Location: Taiwan
Posts: 74
Rep Power: 8
Rajaero is on a distinguished road
Hi,
please follow the steps below,
1. In space claim you should select share options under properties
2. If you select share option then cfx will create fluid solid interface automatically when you split domain (fluid and solid domain) in cfx
3. For the interface boundary condition 3 types available. Generally people will select conservative heat flux across interface.
4. as you know in fluent you can give heat source as a volume heat generation rate (W/m^3). but in CFX it is only heat flow (W). so it is better to convert volume heat generation rate (W/m^3) to total heat source (W) (simple conversion)

Thanks...
Hamda likes this.
Rajaero is offline   Reply With Quote

Old   August 6, 2018, 04:44
Default
  #10
Member
 
Hamda
Join Date: Jul 2018
Posts: 80
Rep Power: 7
Hamda is on a distinguished road
Quote:
Originally Posted by Rajaero View Post
Hi,
please follow the steps below,
1. In space claim you should select share options under properties
2. If you select share option then cfx will create fluid solid interface automatically when you split domain (fluid and solid domain) in cfx
3. For the interface boundary condition 3 types available. Generally people will select conservative heat flux across interface.
4. as you know in fluent you can give heat source as a volume heat generation rate (W/m^3). but in CFX it is only heat flow (W). so it is better to convert volume heat generation rate (W/m^3) to total heat source (W) (simple conversion)

Thanks...
Thank you,
But where? in CFX or meshing stage? since in CFX I don't find "share option" and properties.
By the way, I asked it in other sites too and I was told that in Meshing stage, I should have one geometry with 2 parts (fluid and solid zones) then CFX itself will create solid-fluid interface but now I have 2 geometries.
Attached Images
File Type: jpg Screenshot (111).jpg (84.7 KB, 4 views)
Hamda is offline   Reply With Quote

Old   August 7, 2018, 04:58
Default
  #11
Member
 
Taiwan,new north city
Join Date: Aug 2017
Location: Taiwan
Posts: 74
Rep Power: 8
Rajaero is on a distinguished road
Hi,
sorry i did a mistake. Follow the steps below,
1.Left click your geometry/part file and select share option under analysis/share topology.
2. Refer the following link in YouTube (share topology)
https://www.youtube.com/watch?v=h43E1YO1LiM&t=65s

3. Did you enable automatic default interface in cfx. If not check the following link.
https://www.sharcnet.ca/Software/Ans...DialogPre.html

Thanks...
Hamda likes this.
Rajaero is offline   Reply With Quote

Old   August 7, 2018, 07:15
Default
  #12
Member
 
Hamda
Join Date: Jul 2018
Posts: 80
Rep Power: 7
Hamda is on a distinguished road
Thank you for providing me with links. I already defined interfaces in my mesh file and then in CFX , in interface section, I created 2 interfaces.. but now my problem is for inner spheres (4 spheres as you see in the pic) how can I define 2 interface sides? since as you know for each interface one side should be for solid and other side should be for fluid.



Thanks
Hamda is offline   Reply With Quote

Old   August 7, 2018, 07:59
Default
  #13
Member
 
Hamda
Join Date: Jul 2018
Posts: 80
Rep Power: 7
Hamda is on a distinguished road
"Did you enable automatic default interface in cfx. If not check the following link"


Sorry but when I right-click the Simulation object in the tree view there is no "Automatic Default Interfaces".
by the way , I see "interfaces" object below the "simulation" object.
Hamda is offline   Reply With Quote

Old   August 7, 2018, 08:17
Default
  #14
Member
 
Hamda
Join Date: Jul 2018
Posts: 80
Rep Power: 7
Hamda is on a distinguished road
the video is for Ansys mechanical and I created my geometry in CFX, so It didn't help me. By the way thanks.
Hamda is offline   Reply With Quote

Reply

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
[swak4Foam] swak4foam for OpenFOAM 4.0 mnikku OpenFOAM Community Contributions 80 May 17, 2022 08:06
Problem with chtMultiregionFoam radiation boundary condition baran_foam OpenFOAM Running, Solving & CFD 10 December 17, 2019 17:36
Laminar Kinetic Energy Model (Walters 2008) logoswort Fluent UDF and Scheme Programming 2 May 19, 2017 19:41
[Other] Adding solvers from DensityBasedTurbo to foam-extend 3.0 Seroga OpenFOAM Community Contributions 9 June 12, 2015 17:18
Trouble compiling utilities using source-built OpenFOAM Artur OpenFOAM Programming & Development 14 October 29, 2013 10:59


All times are GMT -4. The time now is 19:52.