[kevin8843]

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.

[ghorrocks]

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?

[kevin8843]

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

[ghorrocks]

So this sounds like a moving mesh application. Does the motion have any twisting or is it just vibration?

[kevin8843]

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

[ghorrocks]

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.

[kevin8843]

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

[ghorrocks]

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.

[kevin8843]

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

[ghorrocks]

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.

[kevin8843]

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?

[ghorrocks]

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.

[kevin8843]

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

[ghorrocks]

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.

[kevin8843]

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

[ghorrocks]

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.