|
[Sponsors] |
![]() |
![]() |
#1 |
New Member
Thomas
Join Date: Dec 2016
Posts: 10
Rep Power: 10 ![]() |
Hello,
Im very new in Ansys Fluent and I wont to try some easy tutorials on YouTube. I found a very interesting one about an axial fan: Link: https://www.youtube.com/watch?v=KFrZoDWUC5s I try this with my own model since 2 days but without succes. ![]() The Blade is rotating, I mean the mesh is moving but there is no velocity or change of the pressure. Can someone help me please and tell what mistake I made? I uploadet a short Video which explain my problem better. Link: https://youtu.be/1GE5LoVIkjw For you guys this shoud be very simple. Thanks, Tom |
|
![]() |
![]() |
![]() |
![]() |
#2 |
Senior Member
Have a nice time!
Join Date: Feb 2016
Location: mech.eng.ahmedmansour@gmail.com
Posts: 291
Rep Power: 11 ![]() |
Hello dear Thomas...the problem is that you used the aluminium as a material and this is not right...here we simulate the fluid (air) and you have to select the air when you define the material of the cell zones....Only air....and you have to define only 2 cell zones "the enclosure and this is the fixed domain" and the rotating domain and here you check "mesh motion" and set the rotating speed...nothing more...you defined 3 zones with the wrong material.....Tell me your progress please...Thanks...I have a VAWT 2D simulation using the same sliding mesh technique and I showed that it it...It may help you sir...also there is a 3D tutorial about wind turbines using the enclosure "Ansys Fluent- Wind Turbine" it also may help you and it is uploaded on another youtube channel...Thanks
|
|
![]() |
![]() |
![]() |
![]() |
#3 | |
Senior Member
Join Date: Feb 2011
Posts: 496
Rep Power: 18 ![]() |
Quote:
|
||
![]() |
![]() |
![]() |
![]() |
#4 |
Senior Member
Have a nice time!
Join Date: Feb 2016
Location: mech.eng.ahmedmansour@gmail.com
Posts: 291
Rep Power: 11 ![]() |
If he follow what I said, the interfaces "contact regions" will be automatically detected by Fluent...This is not like the 2D simulations, the 2D simulations require defining the interfaces manually..And his tutorial shows 2 interfaces but with wrong definition due to the additional cell zone and the wrong material .Thanks
|
|
![]() |
![]() |
![]() |
![]() |
#5 | ||
New Member
Thomas
Join Date: Dec 2016
Posts: 10
Rep Power: 10 ![]() |
Thanks for the reply.
Quote:
And what I still dont understand is, why only 2 Zell Zones. I take this tutorial as an exercise. Later I would like that the fan "blow/cool down" another object (for example a pipe or somthing similar). It must be possible that the simulation has diffrent materials included. Quote:
best regards, Tom |
|||
![]() |
![]() |
![]() |
![]() |
#6 |
Senior Member
Have a nice time!
Join Date: Feb 2016
Location: mech.eng.ahmedmansour@gmail.com
Posts: 291
Rep Power: 11 ![]() |
Dear Thomas, like I said...If you wanna study the rotation of the fan, you have to define the materials as air without any solids...Fluent in this simulations will consider the air tries to rotate the rotor and you will get good results such as the tutorial of Eng. Raef...To study the heat transfer..I think it will be different setup or you may use Transient heat transfer package or also fluent but if you use fluent you have to set the temperature and check the energy equation...Also, if you have 2 fixed zones and 1 rotor, you will define 3 zones to tell fluent that the rotor will slide on 2 fixed zones..no problem..Also, if you import the rotor into ansys, it has to be add frozen not add material to run sliding mesh simulations..
Thanks |
|
![]() |
![]() |
![]() |
![]() |
#7 |
New Member
Thomas
Join Date: Dec 2016
Posts: 10
Rep Power: 10 ![]() |
Dear Ahmed,
I will try it tomorrow and report. I dont understand why, but well. Thanks |
|
![]() |
![]() |
![]() |
![]() |
#8 |
Senior Member
Have a nice time!
Join Date: Feb 2016
Location: mech.eng.ahmedmansour@gmail.com
Posts: 291
Rep Power: 11 ![]() |
Read the modified reply please
![]() |
|
![]() |
![]() |
![]() |
![]() |
#9 | |
New Member
Thomas
Join Date: Dec 2016
Posts: 10
Rep Power: 10 ![]() |
Quote:
|
||
![]() |
![]() |
![]() |
![]() |
#10 |
Senior Member
Have a nice time!
Join Date: Feb 2016
Location: mech.eng.ahmedmansour@gmail.com
Posts: 291
Rep Power: 11 ![]() |
I think, yes..Try it because I think that you defined the aluminium and it did not work properly...You showed that in the tutorial...we study the air that rotates the turbine...try what I said and what the others did and tell me please..Then we can analyze the next step...Do not worry dear Thomas
![]() Thanks |
|
![]() |
![]() |
![]() |
![]() |
#11 |
Senior Member
Have a nice time!
Join Date: Feb 2016
Location: mech.eng.ahmedmansour@gmail.com
Posts: 291
Rep Power: 11 ![]() |
When we run 3D simulations on centrifugal pumps, we do not import the pump model that was created by solidworks or inventor..We draw the fluid path inside the pump and define the 2 interfaces and the material for the 3 zones is water...we can set the temperature of the water to study the heat transfer of the water....If you wanna study the heat transfer of the CAD model of the pump...we make another different scenarios
![]() Thanks |
|
![]() |
![]() |
![]() |
![]() |
#12 |
New Member
Join Date: Dec 2016
Posts: 5
Rep Power: 10 ![]() |
Hey Thomas!
As far as I can tell, there are some problems in your design modeler and fluent setup. First of all, if you are only interested in the flow field arround your fan, you do not need to include any solid (non fluid) body in your Simulation. You do need the the fan and the stator in the design modeler, in order to substract them from the fluid domain. Before meshing however the fan and the stator must be suppressed. To create a vaild simulation setup, try the following steps: 1) Create a cylindric enclosure (using the enclosure tool) that closly covers your fan. And surpress the rotor itself. Through this you created a fluid domain for the fan featuring a gap with the shape of your fan. 2) Arround this enclosure create a second enclosure (box or cylinder). From this enclosure, substract the first enclosure and the stator (a cylindric hole should be visible). The second enclosure represents the non rotating fluid zone. Surpress the stator. 3) Go to the meshing. You should see two parts: The inner cylindric enclosure and the outer one (with the cylindric hole). Create the mesh. 4) Open the mesh in Fluent and define the inner enclosure as rotating and the outer one as stationary. Make sure that there is a Interface defined between both enclosures. Set the boundary conditions (your ones were correct). Run the calculation. The issue with your setup was, that you tried to rotate the rotor itself. In this approach to rotor simulation (called a sliding mesh approach) however instead of the rotor itself, a fluid part arround the rotor is rotated. I hope this advise helps you. Regards, Georg Sent from my SM-G920F using CFD Online Forum mobile app |
|
![]() |
![]() |
![]() |
![]() |
#13 |
Senior Member
Have a nice time!
Join Date: Feb 2016
Location: mech.eng.ahmedmansour@gmail.com
Posts: 291
Rep Power: 11 ![]() |
Dear GeorgeD....God bless you
![]() ![]() ![]() Viel Spaß ! |
|
![]() |
![]() |
![]() |
![]() |
#14 |
New Member
Join Date: Dec 2016
Posts: 5
Rep Power: 10 ![]() |
||
![]() |
![]() |
![]() |
![]() |
#15 |
Senior Member
Have a nice time!
Join Date: Feb 2016
Location: mech.eng.ahmedmansour@gmail.com
Posts: 291
Rep Power: 11 ![]() |
I know the information you typed....The problem is with the simulation of Eng. Thomas, I hope it works with him.....
Thank you and him... ![]() |
|
![]() |
![]() |
![]() |
![]() |
#16 |
New Member
Join Date: Dec 2016
Posts: 5
Rep Power: 10 ![]() |
Maybe a time saver for Thomas Simulation: Instead of starting the simulation in transient mode with a rather small timestep, try to calculate a steady solution first using the moving reference frame model.
To do this, just switch to steady state and check the "frame motion" check box for the rotating zone (the inner enclosure) instead of "mesh motion" and define the same rotation settings. Once you reached convergence in steady state, switch to transient and hit "copy to mesh motion" button in the rotating zone setup and start the transient run. With this you avoid calculating many timesteps until the flowfield is developed. Sent from my SM-G920F using CFD Online Forum mobile app |
|
![]() |
![]() |
![]() |
![]() |
#17 |
Senior Member
Have a nice time!
Join Date: Feb 2016
Location: mech.eng.ahmedmansour@gmail.com
Posts: 291
Rep Power: 11 ![]() |
He can run many things because he is new in Fluent, so it will be good examples but he has to know that sliding mesh is designed for the unsteady simulations due to the unsteady nature of the flow..Some applications can be simulated firstly as steady....All the information about these models are included in Ansys theory guide and it is available on Google...
Thanks |
|
![]() |
![]() |
![]() |
![]() |
#18 |
New Member
Join Date: Dec 2016
Posts: 5
Rep Power: 10 ![]() |
Yes, you are right... Especially about the Theory/User Guide. This thing maybe looks like Windows 98, but usually you will find a good description of the models including examples on how to use them...
Sent from my SM-G920F using CFD Online Forum mobile app |
|
![]() |
![]() |
![]() |
![]() |
#19 |
New Member
Thomas
Join Date: Dec 2016
Posts: 10
Rep Power: 10 ![]() |
Hi all,
I tryed the steps from GeorgD´s post above and I hope that I have done it right. But it dont seem to be the case, because the result looks confusing. Well, at least ther is a result. Update: A detailed descrition of what I did: 1.) Import the model with 2 bodies (stator + rotor) 2.) Created an enclosure (rotating_enclosure) that covers the model. 3.) Created a boolean and substracted the rotor from the rotating_enclosure. 4.) Created a second enclosure (static_enclosure) wich represents the air-zone. 5.) Createt a second boolean and substracted the stator and the rotating_enclosure. 6.) Supressed the stator and the rotor in the bodie tree. 7.) Created the name selections outlet_1, outlet_2 and wall I uploadet a new video. Link: https://youtu.be/NCr8CLaT8mM It seems that the inner (rotating) enclosure is a like a invisible wall, but it isnt defined as wall, as seen in the video. Because the inner_enclosure includes the stator, it seems that the stator is also rotating. So first I treyed with the sketcher to draw a circle between stator and rotor an extruded it. but then I got this Error: "Divergence detected in AMG solver: pressure correction" Maby I shoud create another boolean between the steps 5 and 6 to add the stator again to the static_enclosure.... Ok the stator is rotating, or not... no matter at the moment. There must be another mistake on the boundery conditions or the cell zones. @Ahmed: Thanks for the tip about theory user guide, I will read and try some examples. @GeorgD: A steady simulation is really a time saver,.. thanks. But if I run a steady simulation, there are no results about the velocity, because in this case there is no inlet and at the time t=0s the air is not moving. For the pressure its Ok. Thanks for your efforts, Tom |
|
![]() |
![]() |
![]() |
![]() |
#20 |
Senior Member
Have a nice time!
Join Date: Feb 2016
Location: mech.eng.ahmedmansour@gmail.com
Posts: 291
Rep Power: 11 ![]() |
Try to follow eng Raef bolean methods..He talked about them...I think it is easy..
Good luck sir. |
|
![]() |
![]() |
![]() |
Tags |
bodie, fluent, rotating |
|
|
![]() |
||||
Thread | Thread Starter | Forum | Replies | Last Post |
Axial Fan is rotating - BC's at Inlet/Outlet? | SirIsaac90 | OpenFOAM Pre-Processing | 1 | September 8, 2016 14:17 |
Car external aerodynamic with wheel spinning issue | hokhay | FloEFD, FloWorks & FloTHERM | 2 | August 18, 2016 05:23 |
Interpreting streamlines of a rotating fan. | danbence | Visualization & Post-Processing | 1 | April 8, 2014 11:13 |
Simulation of Axial Fan Flow using A Momentum Source Subdomain | Liam | CFX | 28 | July 16, 2013 09:24 |
axial flow in counter rotating ducted fan | Vishu | FLUENT | 4 | January 13, 2004 18:52 |