Help with Function Boudary Condition/Tabular BCs

[thanhvan]

Hello everybody,

Would you please tell me some ideas about Function/Table BCs in ANSYS. How to define a Function by using Command lines.
For example:

! Begin of equation: a*sin(omega*{TIME})
%_FNCNAME%(0,0,1)= 0.0, -999
%_FNCNAME%(2,0,1)= 0.0
%_FNCNAME%(3,0,1)= %_FNC_C1(1)%
%_FNCNAME%(4,0,1)= %_FNC_C2(1)%
%_FNCNAME%(5,0,1)= 0.0
%_FNCNAME%(6,0,1)= 0.0
%_FNCNAME%(0,1,1)= 1.0, -1, 0, 1, 18, 3, 1
%_FNCNAME%(0,2,1)= 0.0, -1, 9, 1, -1, 0, 0
%_FNCNAME%(0,3,1)= 0, -2, 0, 1, 17, 3, -1
%_FNCNAME%(0,4,1)= 0.0, 99, 0, 1, -2, 0, 0
! End of equation: a*sin(omega*{TIME})
(%_FNC_C1(1)%, %_FNC_C2(1)% are constants)

I could not understand the meaning of these above command. Is it a Function written in command lines?
You can refer them at section 3.6.4 of the ANSYS7.0/Help

Also, do you know how to apply a 2 Dimension Table as a boudary condition? If I want to apply a load which is vary versus time of the solution and the position of the nodes, what should I do?
Thank you very much for your consideration.
Best regards.

 

[mxr]

I'm having the same questions with this. The example makes absolutely no sense. I have to set up a similar boundary condition. Does anybody have a clue?

 

[Drej]

To set up a boundary condition based on a function of time (which is what I'm assuming you need), you need to set up tabular boundary conditions using the TABLE function in ANSYS. One way is to use the function editor. An easier (personal opinion) way is to use a simple series of commands.

To set up a function where the time t is:

0
0.1
0.2
0.3
0.4
0.5
...
...

and the value of the function is:

1
2
3
4
5
6
...
...

You need to first dimension the TABLE using:

*DIM,ENGTIPS,TABLE,6,1,1, , ,

Then, you can specify the t value above using:

*SET,ENGTIPS(1,0,1) , 0 
*SET,ENGTIPS(2,0,1) , 0.1 
*SET,ENGTIPS(3,0,1) , 0.2   
*SET,ENGTIPS(4,0,1) , 0.3   
*SET,ENGTIPS(5,0,1) , 0.4   
*SET,ENGTIPS(6,0,1) , 0.5

and the value of the function using:

*SET,ENGTIPS(1,1,1) , 1   
*SET,ENGTIPS(2,1,1) , 2 
*SET,ENGTIPS(3,1,1) , 3 
*SET,ENGTIPS(4,1,1) , 4 
*SET,ENGTIPS(5,1,1) , 5
*SET,ENGTIPS(6,1,1) , 6

Tables are used SPECIFICALLY for this function in ANSYS i.e. you must use a TABLE to specify TABULAR BCs. If you want, you can put all of the above into a text file and read this into ANSYS using FILE > Read input from... and choose the file.

Then you have to refer to the TABLE name in your loading. For example, if the value of the function is displacement in the x direction applied to node 1354:

D,1354,UX,%ENGTIPS%

or force:

F,1354,FX,%ENGTIPS%

Let me know how you get on with this.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[thanhvan]

Hi Drej,

Thanks for your sharing. Recently, I usually apply the tablular boundary condition by using Function Editor. It's is very easy to use and mentioned in the Ansys help. After building the function, use the Ansys Main Menu/Session Editor to copy the code of the function. It's look the same with my previous post. And though I could not understand all the number, this method works just well.

 

[mxr]

Thanks Drej and thanhavan...this was a great help and now the B.C. I want is working! I found that you can also go into the function file that's generated using the function editor and copy the part of the code that sets up the table.

Thanks again for the great help!