|
[Sponsors] |
August 20, 2016, 20:03 |
3D Fan Zone
|
#1 |
New Member
Daniel Riveros
Join Date: Nov 2015
Location: Genoa, Italy
Posts: 14
Rep Power: 10 |
Hi!
I am simulating the behavior of a refrigerator's fan, I have already ran a MRF Sliding Mesh simulation with the fan geometry, but I would like to use the 3D Fan Zone model, because this option could reduce the computational time. Could you tell me: how the geometry should be define? I created a toroidal shape with a square as its base and I meshed it. The user's manual says to define its boundaries as interior, but I cannot do it becuase Fluent only gives me the option of interface. When I try to run the simulation, it shows an error of segmentation fault. I hope you can help me. Thank you. |
|
September 12, 2016, 04:46 |
|
#2 |
Member
Arnout
Join Date: Nov 2010
Posts: 46
Rep Power: 15 |
Hi,
Check if you have a inlet plane and a outlet plane, of type interior, splitting the fan zone with the other fluid zone. Good luck! |
|
November 30, 2016, 00:47 |
|
#3 | |
New Member
Jay Sudani
Join Date: Nov 2016
Posts: 4
Rep Power: 9 |
Quote:
I am also facing the same issue while using 3D Fan Zone model in ANSYS Fluent. Can you help me to resolve the error of segmentation fault ? |
||
November 30, 2016, 00:58 |
3D Fan Zone
|
#4 |
Member
Arnout
Join Date: Nov 2010
Posts: 46
Rep Power: 15 |
Hi, I had the same mesh on both sides of the interface and had set the interface initially to wall (in the mesher). Then I could change it to interior in fluent. If you're mesh is not matching on both sides of a face, fluent defines it as interface. Good luck!
|
|
November 30, 2016, 01:13 |
|
#5 |
New Member
Jay Sudani
Join Date: Nov 2016
Posts: 4
Rep Power: 9 |
But how can we define any boundary as wall in the Ansys mesher itself? We usually do that in the "setup". Also is it necesaary to have a torrid shape as the 3D Fan ? Can we have hollow cylinder instead?
|
|
November 30, 2016, 01:49 |
|
#6 |
Member
Arnout
Join Date: Nov 2010
Posts: 46
Rep Power: 15 |
In the ansys meshed, you can give the inter face a name. wall_in and wall_out for example. Select the face, right click and choose named selection. I had a cylinder shape.
|
|
November 30, 2016, 01:52 |
|
#7 |
New Member
Jay Sudani
Join Date: Nov 2016
Posts: 4
Rep Power: 9 |
Thank You. I will try it.
|
|
November 30, 2016, 02:20 |
|
#8 |
New Member
Jay Sudani
Join Date: Nov 2016
Posts: 4
Rep Power: 9 |
Dear,
Do you have any tutorial of 3D fan zone model ? |
|
November 30, 2016, 02:27 |
|
#9 |
Member
Arnout
Join Date: Nov 2010
Posts: 46
Rep Power: 15 |
Hi, no. But it was straight forward. Meshing: Give the fan zone a different name, define inlet and outlet plane as wall. Fluent: Change faces from wall to interior, select the fan fluid zone, switch on fan zone. Type dP and rotor speed. Define blade parameters from blade design. Select the faces as in and outlet. (Wrote it down from my memory...so it can be a little different...)
|
|
December 2, 2016, 02:16 |
|
#10 |
New Member
Bhaskar
Join Date: Feb 2015
Posts: 7
Rep Power: 11 |
Why are you not using the lumped parameter model of fluent ? Since you just need the fan flow as per the fan curve, and not other stuff such as fan noise or stall points.
Just create a cylindrical zone, which is the same dimensions of your fan structure(dia and depth). Make sure it has hex mesh, because the node direction of the mesh will determine the fan direction. You can also select to reverse the flow direction as per your convenience. |
|
December 17, 2016, 09:28 |
3D Fan Zone
|
#11 | |
New Member
Daniel Riveros
Join Date: Nov 2015
Location: Genoa, Italy
Posts: 14
Rep Power: 10 |
Quote:
I solved my problem following the next steps: 1. In DesignModeler you create a hollow cylinder and create the inertial zones around this cylinder. 2. Step 1 gives you at least 2 bodies, so you have to put together the hollow cylinder and the bodies around it in a New Part (this create a group of bodies, but in Meshing create a continuos mesh for all bodies in the group) 3. In Meshing you mesh all your bodies and walls between the bodies from the new part are defined as interior. 4. Just follow the steps that ANSYS Help give about defining a 3D Fan Zone in Fluent. I hope this can help you. Have a nice day, Jay. |
||
January 23, 2017, 09:57 |
|
#12 |
New Member
Thomas
Join Date: Dec 2016
Posts: 10
Rep Power: 9 |
Dear Daniel,
have the same problem. Its is a contact region (interface) istead of a wall. And if I delete this contact region, I cant make it interior just wall or intake_fan or exhoust_fan. Can you please upload your project file? Greets, Tom |
|
January 7, 2020, 05:36 |
3D fan zone tutorial case file
|
#13 |
New Member
Chu Yung Jeh
Join Date: Mar 2012
Posts: 7
Rep Power: 14 |
||
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[Commercial meshers] Mesh conversion problem (fluent3DMeshToFoam) | Aadhavan | OpenFOAM Meshing & Mesh Conversion | 2 | March 8, 2018 01:47 |
Possible Bug in pimpleFoam (or createPatch) (or fluent3DMeshToFoam) | cfdonline2mohsen | OpenFOAM | 3 | October 21, 2013 09:28 |
[Commercial meshers] fluentMeshToFoam multidomain mesh conversion problem | Attesz | OpenFOAM Meshing & Mesh Conversion | 12 | May 2, 2013 10:52 |
Problem in running ICEM grid in Openfoam | Tarak | OpenFOAM | 6 | September 9, 2011 17:51 |
Problem in IMPORT of ICEM input file in FLUENT | csvirume | FLUENT | 2 | September 9, 2009 01:08 |