Hi!

I simulated two-way fluid structure interaction running an ANSYS Multi-field (MFX) simulation with constant inlet velocity, now I try to set a inlet velocity which is variable with time step. I want to read a file which have the inlet velocity data variable with time step. How can I do this?

Thanks!

Dear Dorin,

Is it a function of time only, or a function of space as well? For the former, just type in a 1d CEL interpolation function..

For the latter, there are ways of achieving this but I advice you to contact the CFX help desk.

Opaque

Dear opaque,

Thanks for your help. It is a function of time only. I try to simulate a transient two-way fluid structure interaction running an ANSYS Multi-field simulation with inlet velocity have a different value for each timesteps , the timesteps is the same timesteps which I enter in Simulation Type tab. I have a file with two column, first column have timesteps value and the second has velocity value, I try to introduce this file as a inlet velocity. How can I do this?

Thanks!

Dorin

Dear Dorin,

Please search the documentation for "one dimensional interpolation" and it explain to you how it works.

At the end of that document, there is the explanation of "importing data from file"

Opaque

Dear Opaque,

Thanks for your help. I search in the documentation and I understood that Coordinate column accept coordinate axis dimensions (e.g., [m], [cm], etc.) and in the Value column I understood that I can put velocity value. This mean that the velocity is variable with coordinate. What I want is to set velocity variable with timesteps, in Coordinate column I want to have timesteps, for example I have a total time of the simulation 0.7 s and the timesteps 0.007 s and I want that inlet velocity(U) to have a value of 0.1 m/s at timestep 0.007, a value of 0.2 m/s at timestep 0.014, a value of 0.3 m/s at timestep 0.021, ..., a value of 10 m/s at timestep 0.7. I have this values in a file, when I Right-click in the window to import data from a file the value of timesteps are written in Coordinate column and the value of velocity are written in Value column. Please tell me if it is O.K, because I understood that in Coordinate column I can put only the coordinate axis dimensions (x, y, z).

Thanks!

Dorin

Dear Dorin,

It should be OK (at least for 1D interpolation)..

Unless your file is really large, I would input the data directly into the GUI..

Opaque.

Dear Opaque,

Thanks! In this case it is O.K to put in Argument units [s] and in Results units [m s^-1]? Please tell me how I set the velocity in inlet boundary?

Thanks!

Dorin

Dear Dorin,

Here is an example,

FUNCTION : MyVelFunc

Option = Interpolation

Result Units = [m s^-1]

Argument List = [s]

INTERPOLATION DATA :

Data Pairs = 0.00, 1.0, \

0.01, 1.0, \

......

Extend Min = True

Extend Max = True

END

END

Then, in you inlet you will type something like

MASS AND MOMENTUM:

Option = Normal Speed

Normal Speed = MyVelFunc(t)

END

Hope this helps,

Opaque

Dear Opaque,

Thanks a lot, that was really helpful!

Dorin

If your velocity profile is that simple, why don't you use an expression for the velocity? U = U0 * t/1[s] ? - Dr. Flow Squad

Hi Dr. Flow Squad!

Thanks! The velocity profile which I written in the message is a simple example and it is a good idea to use an expression, but I want to know, in case that the velocity profile is not that simple and it is hard to put in a expression, how to read a file with velocity data.

I search in archives and I found this address http://tinyurl.com/2gkjh8 and I see that you simulated cylinder in cross flow, please send me, if it is possible, the command file and the geometry file for this problem, it will be very helpful to me.

Thanks!

Dorin

It's not the best mesh I've made, but here it is: http://users.cybercity.dk/~ida3068/cfd/2dcylinder.zip - Dr F.S.

Hi Dr. Flow Squad!

Thanks!

I create a new simulation, I import gtm file after that I import ccl file and I have some errors:

Initial conditions are required for transient simulations (unless you select an Initial Values file from the Solver Manager).

There are 2d regions in boundary 'Domain Interface 1 Side 1' in domain 'Domain 1' that have already been used.

The parameter "Location" in "/FLOW/DOMAINomain 1" holds the following disallowed value: "Assembly 3". (Allowed values are: "Assembly 2, B30, B30 2, Assembly".)

The parameter "Location" in "/FLOW/DOMAINomain 1/BOUNDARY:in" holds the following disallowed value: "in". (Allowed values are: "Assembly 2, Default 2D Region 2, in 2, out 2, ...".)

The parameter "Location" in "/FLOW/DOMAINomain 1/BOUNDARY:symside1" holds the following disallowed value: "Default 2D Region". (Allowed values are: "Assembly 2, Default 2D Region 2, in 2, out 2, ...".)

Please tell me what happened, I did something wrong?

Thanks!

Dorin

Within pre I reflected the geometry (w. copy) to get the full domain. Maybe it has to do with that, I don't recall. Change the settings to stationary to get a start value that the transient simulation can start from. Good luck. otherwise contact me directly through email. this is not forum related any more.