CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

Table or polynomial boundary condition

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 15, 2019, 11:33
Default Table or polynomial boundary condition
  #1
New Member
 
Luka Vincekovic
Join Date: Mar 2019
Posts: 6
Rep Power: 2
lvincek is on a distinguished road
Hi all,
I am trying to insert flow direction as boundary condition via table. As far as I realised this can't be done. It is either value or expression, right?

So my question is, if I have a table which for example, describes some boundary condition what is the best way to import it as an expression?
Can someone please explain the procedure?

Let's say that we start from 100x100 values x-y table which describes total pressure. How do you get polynomial and import it in CFX? I attached how the pressure looks like when you plot it in MATLAB.

Thanks, Luka

Attached Images
File Type: png Capture.PNG (47.9 KB, 10 views)
lvincek is offline   Reply With Quote

Old   March 15, 2019, 11:38
Default
  #2
Senior Member
 
Join Date: Jun 2009
Posts: 962
Rep Power: 17
Opaque is on a distinguished road
In ANSYS CFX, a table is an expression via a function. Check the documentation for how functions work in expressions.
Opaque is offline   Reply With Quote

Old   March 15, 2019, 11:41
Default
  #3
New Member
 
Luka Vincekovic
Join Date: Mar 2019
Posts: 6
Rep Power: 2
lvincek is on a distinguished road
Yeah, I managed to get an expression working but it doesn't show what I want.
Do you have an idea how to describe attached contour with polynomial that would work?

Thanks
lvincek is offline   Reply With Quote

Old   March 15, 2019, 18:03
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,628
Rep Power: 120
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
You could use a 3D interpolation function, a polynomial which describes the function as a CEL expression or a user fortran routine to define it. CFX has lots of ways to do it.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   March 18, 2019, 11:34
Default
  #5
Senior Member
 
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 837
Rep Power: 16
evcelica is on a distinguished road
Yes, there are lots of ways to do it.

Easiest would be the 3D interpolation function that uses your 100x100 table directly.
Make it a function of (x,1,z)
format your table with 4 columns, using:
x, 1, z, PressureValue.
Then make an expression for P_inlet which would be a call to the function: PressureFunction(x,1,z).


To make a polynomial, you will have to develop an equation for a 2D surface, which is difficult, and usually not very accurate for complex surfaces.
evcelica is offline   Reply With Quote

Old   March 19, 2019, 04:30
Default
  #6
New Member
 
Luka Vincekovic
Join Date: Mar 2019
Posts: 6
Rep Power: 2
lvincek is on a distinguished road
Thank you all for the help, just a quick update.

I managed to import all the data as a table at the end. It is possible to import also the velocity direction as a table. I did a bit of reverse engineering. So in CFX Post you can see what data you can export from your boundaries and all these data can be imported as a table into CFX Pre.
So I took a table from CFX Post and just changed the values with what I needed and put it into CFX Pre.
lvincek is offline   Reply With Quote

Old   March 20, 2019, 12:15
Default
  #7
Senior Member
 
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 837
Rep Power: 16
evcelica is on a distinguished road
Yes you can import velocity as a table, or just about anything else you wish.
evcelica is offline   Reply With Quote

Reply

Tags
cfx, polynomial bc, polynomial eqn.

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Problem in setting Boundary Condition Madhatter92 CFX 12 January 12, 2016 04:39
sliding mesh problem in CFX Saima CFX 45 September 22, 2015 10:53
Radiation in semi-transparent media with surface-to-surface model? mpeppels CFX 10 June 16, 2015 15:48
several fields modified by single boundary condition schröder OpenFOAM Programming & Development 3 April 21, 2015 05:09
Error finding variable "THERMX" sunilpatil CFX 8 April 26, 2013 07:00


All times are GMT -4. The time now is 13:24.