|
[Sponsors] |
November 2, 2013, 18:19 |
CFX a vibration fan at a shell space
|
#1 |
New Member
邱迪西
Join Date: Nov 2013
Posts: 8
Rep Power: 13 |
Hi all
I'm a Mechanical Engineering student from Taiwan And my English is not so good. So maybe I can't express what simulation i want to do so well. My reserch is put a vibration fan at a shell space. The size of shell space is 300*150*10(mm) And the size of fan is 30*30*0.3(mm) And the fan place in the center of shell space. Seniors tell me to give the fan an expression as "0.004[m]*(x/0.03[m])*sin(pi*Time/0.01)" (A fan with the tip amplitude as 8mm and frequency as 50Hz) If I run it for steady state the time of solve is very quick. And the results of stream line look so weird. My seniors run it for transient at that time. And he set Total time as 0.04s Time steps as 0.01s And add a Trn Results what program ask him to add. He set 1 at Output Frequency and he don't know why. but the results of stream line is also weird. all stream focus on fan and don't bring the air onward. and the velocity is very slow. I tried to set the total time for 0.04s and time steps as 0.001s but it will be error. The part of mesh. My senior teach me very simple. We only change the setting of sizing Use Advanced Size Funtion ON:Proximimity and Curvature Relevance Center Fine Smoothing High Span Angle Center Fine (P.S. He don't know why choose these) Min Size 0.0003m (the height of fan) Max Face Size 0.001m Max Size 0.005m And we do Face Sizing on fan Element Size 0.0003m I ask for helo from many people but nobody can help me. Then I found this forum so I ask for help here. Thanks. |
|
November 2, 2013, 23:46 |
|
#2 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,844
Rep Power: 144 |
I do not understand what you are trying to do.
Why does the fan have the vibration? Is the vibration known or is it coupled to the fluid flow? What is the purpose of doing this model? What effects do you expect this vibration will have on the fluid flow? |
|
November 3, 2013, 00:01 |
|
#3 |
New Member
邱迪西
Join Date: Nov 2013
Posts: 8
Rep Power: 13 |
The vibration is known
It's not a rotary fan It's an electromagnetic control swing blade blower Its movement pattern like piezoelectricity fan Because of modern electronic products more thinner now. We want to know whether this fan can cooling when it place in a shell box But it's builded recently so we don't think too much. At this stage we just want to see the fluid field and the velocity of air flow first. thank you for your response |
|
November 3, 2013, 00:06 |
|
#4 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,844
Rep Power: 144 |
So this sounds like a moving mesh application. Does the motion have any twisting or is it just vibration?
|
|
November 3, 2013, 00:20 |
|
#5 |
New Member
邱迪西
Join Date: Nov 2013
Posts: 8
Rep Power: 13 |
In reality we giving fan a sine wave from function generator
At the CFX we set Mesh Deformation Regions of Motion Specified Expression 0.004[m]*(x/0.03[m])*sin(pi*Time/0.01) boundry six faces of fan Specified Displacement x Component 0 y Component 0.004[m]*(x/0.03[m])*sin(pi*Time/0.01) z Component 0 No Slip Wall |
|
November 3, 2013, 00:34 |
|
#6 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,844
Rep Power: 144 |
This sounds simple - just a moving mesh simulation. You first post says the flow is not how you expect. I would not expect much (or even any) forward flow if you just vibrate a blade.
What flow do you expect from this? Do you have experimental data to support it? Are you absolutely sure the blade does not twist? Even a small twist of a few degrees will make the blade a much more effective airfoil and generate a flow larger than a straight blade. |
|
November 3, 2013, 00:45 |
|
#7 |
New Member
邱迪西
Join Date: Nov 2013
Posts: 8
Rep Power: 13 |
We use a trapezoid blade
And its material is aluminum because the blade is very thin only 0.3mm so maybe when it vibrate it twist a little When we use hot wire anemometer at experimental from the blade 5mm We get the velocity as 1.81m/s from hot wire anemometer sorry I can't response so quick because I need to use google translate to type these |
|
November 3, 2013, 06:00 |
|
#8 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,844
Rep Power: 144 |
Your translations are OK, I am starting to understand what you are trying to do.
You might need to run your simulation for many vibration periods before a flow starts up. A short simulation might not be long enough. Also a small amount of twist in the blade might make a big difference. I would look into this and see how much twist you are likely to have. You could do this experimentally or you could do analytical calculations or FEA. |
|
November 3, 2013, 09:56 |
|
#9 |
New Member
邱迪西
Join Date: Nov 2013
Posts: 8
Rep Power: 13 |
I have tried Total Time 1s
Timesteps 0.01s Dose it mean run hundred steps? It's velocity is more big but still too small (0.0003m/s) And the flow didn't go forward too (still focus on blade) I think whether my expression is wrong? or something else? I'm appreciate that you willing to listen to my question thank you |
|
November 3, 2013, 17:43 |
|
#10 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,844
Rep Power: 144 |
If you are modelling a 50Hz vibration you will need a time step much smaller than 0.01s. Try 1e-4 [s], that is closer to the size you will need.
But a better way of setting the time step size is using adaptive time steps. Make it home in on 3-5 coefficient loops per iteration and let it find its own time step. |
|
November 3, 2013, 18:14 |
|
#11 |
New Member
邱迪西
Join Date: Nov 2013
Posts: 8
Rep Power: 13 |
I tried to run your suggestion
and soon,a window pop-up say The ANSYS CFX solver exited with return code 1. No results file | has been created. And I found message in Slover manager as follows At least one highly skewed element has been detected on a wall boundary, leading to an unreliable near-wall distance calculation for the turbulent wall functions. The solver will continue to execute, but convergence and/or accuracy may be affected. Please consider improving the mesh quality. The coordinates of the element face are ( 0.2992E-01, 0.1383E-02, 0.1600E-01 ). I think I should set time step much smaller than 0.01s before too But when I tried to change time steps setting These massage appear often Only some specific set can run Like total time0.04 time steps 0.01 And I am no idea where is the problem is. And the adaptive have many entries I never use this before so I don't know what should I type in these entries I set Initial Timestep 0.001s Maximum Timestep 0.01s Minimum Timestep 0.001s Target Max.Loops 5 Target Min.Loops 3 others entries I didn't change Am I wrong for these setting? |
|
November 3, 2013, 18:20 |
|
#12 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,844
Rep Power: 144 |
Have a look at the options for mesh smoothing to stop the mesh folding error you are getting.
For adaptive time steps: Set the initial time step to 1e-4s Minimum time step size should be 1e-10s The other settings are OK. |
|
November 3, 2013, 19:15 |
|
#13 |
New Member
邱迪西
Join Date: Nov 2013
Posts: 8
Rep Power: 13 |
Sorry I didn't understand for the first sentence
Do you mean mesh > sizing > smoothing? that one i set high and in setup Output Control > Trn Results this part what should I set I don't know what is this part mean My senior set Output Frequency Option Timestep Interval1 before And he don't know why... And really thank you for your patience to teach me these |
|
November 4, 2013, 05:35 |
|
#14 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,844
Rep Power: 144 |
Mesh smoothing options for mesh motion. This is in CFX-Pre under domain options.
Output Control > Trn Results just does averaging and other statistical manipulation of the results. This is useful if you need things like the avergae flow field. I suspect this would be useful in your case. |
|
November 7, 2013, 22:23 |
|
#15 |
New Member
邱迪西
Join Date: Nov 2013
Posts: 8
Rep Power: 13 |
Sorry
I still can't find where is the first sentence you say Does it because of version? My version is V13 And sorry for reply so slowly I'm busy recently for something and thank you |
|
November 7, 2013, 22:42 |
|
#16 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,844
Rep Power: 144 |
I was talking about "Mesh Deformation" options under the domains tab.
There has been a lot of new things done in V14 and V14.5. You should upgrade to the latest version of CFX. |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Uniform pressue increase over fan | alxe | CFX | 4 | August 30, 2011 20:15 |
Pros and Cons for CFX, CFdesign, COMSOL | Val | Main CFD Forum | 3 | June 10, 2011 03:20 |
CFX or Fluent for Turbo machinery ? | Far | FLUENT | 3 | May 27, 2011 04:02 |
Propeller Fan Curve Simulation | Teng_YJ | FLUENT | 2 | February 16, 2009 20:37 |
CFX 4.4 installation problem | Pandu Sattvika | CFX | 1 | December 1, 2001 05:07 |