3D Fan Zone

DRiver · August 20, 2016, 20:03

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.

The King · September 12, 2016, 04:46

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!

Jay Sudani · November 30, 2016, 00:47

Quote:

Originally Posted by DRiver

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.

Dear Daniel Riveros.

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 ?

The King · November 30, 2016, 00:58

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!

Jay Sudani · November 30, 2016, 01:13

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?

The King · November 30, 2016, 01:49

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.

Jay Sudani · November 30, 2016, 01:52

Thank You. I will try it.

Jay Sudani · November 30, 2016, 02:20

Dear,
Do you have any tutorial of 3D fan zone model ?

The King · November 30, 2016, 02:27

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...)

1994bm · December 2, 2016, 02:16

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.

DRiver · December 17, 2016, 09:28

Quote:

Originally Posted by Jay Sudani

Dear Daniel Riveros.

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 ?

Dear Jay Sudani.

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.

shIxx · January 23, 2017, 09:57

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

chujeh2020 · January 7, 2020, 05:36

https://drive.google.com/open?id=1Hs...NOvH28ymq-fkgs

August 20, 2016, 20:03	3D Fan Zone	#1
DRiver 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.

November 30, 2016, 00:58	3D Fan Zone	#4
The King 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!

January 7, 2020, 05:36	3D fan zone tutorial case file	#13
chujeh2020 New Member Chu Yung Jeh Join Date: Mar 2012 Posts: 7 Rep Power: 14	https://drive.google.com/open?id=1Hs...NOvH28ymq-fkgs

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

September 12, 2016, 04:46		#2
The King 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, 01:13		#5
Jay Sudani 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
The King 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
Jay Sudani 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
Jay Sudani 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
The King 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
1994bm 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.

January 23, 2017, 09:57		#12
shIxx 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