|
[Sponsors] |
June 11, 2015, 06:39 |
Patching initial conditions
|
#1 |
Member
mike
Join Date: Jun 2011
Posts: 42
Rep Power: 14 |
Dear All;
I have created a single domain in my mesh, but now I want to initialize a particular region different with other cells. In other words, I want to know if there is an option in CFX 14.5 or 15 to mark a region (with coordinates) and patch it with different values as initialization (just like Fluent), without need to create two distinct zones in the primary mesh. Cheers J.M |
|
June 11, 2015, 08:09 |
|
#2 |
Senior Member
Join Date: Jun 2009
Posts: 1,804
Rep Power: 32 |
You can use CEL to bound the region you want to initialize.
If the region you want to initialize is already a mesh region, i.e. there is name to group all the element in such space, you can easily use the "inside()@mesh region" function. For example, Pressure = 10 [Pa] * inside()@Front Pipe + 20 [Pa] * inside()@Back Pipe where inside()@Front Pipe = 1 within Front Pipe = 0 outside Front Pipe inside()@Back Pipe = 0 outside Back Pipe = 1 within Back Pipe If you want to use coordinates, you can use the CEL "step( expression )" function.. You can search the forum for several examples using "step" (similar to inside but "expression" can be nearly anything you want) May I ask why do you need specific initialization per region ? Multiphase free surface flow ? Recall that ANSYS CFX and ANSYS Fluent have different behaviors and some practices do not translate directly, and may not be needed when switching codes. |
|
June 12, 2015, 14:23 |
|
#3 |
Member
mike
Join Date: Jun 2011
Posts: 42
Rep Power: 14 |
Thanks Opaque;
I am going to simulate discharge phenomenon of a pressurized vessel into ambient. I wanted to know if I can patch vessel pressure in its' coordinates without creating two different zones and applying interfaces. |
|
June 13, 2015, 06:14 |
|
#4 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,703
Rep Power: 143 |
In fact you definitely should use an initial condition which defines the flow and not use multiple domains.
There are many ways you can do this. if(x>4[m],1[bar],0[bar]) step((x-4[m])/1[m])*1[bar] Or you can use 1D interpolation functions with X, Y or Z or some function of XYZ as the input variable. |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[OpenFOAM.org] Compile OF 2.3 on Mac OS X .... the patch | gschaider | OpenFOAM Installation | 225 | August 25, 2015 19:43 |
Wrong fluctuation of pressure in transient simulation | caitao | OpenFOAM Running, Solving & CFD | 2 | March 5, 2015 21:33 |
Orifice Plate with a fully developed flow - Problems with convergence | jonmec | OpenFOAM Running, Solving & CFD | 3 | July 28, 2011 05:24 |
Error while running rhoPisoFoam.. | nileshjrane | OpenFOAM Running, Solving & CFD | 8 | August 26, 2010 12:50 |
OpenFOAM on MinGW crosscompiler hosted on Linux | allenzhao | OpenFOAM Installation | 127 | January 30, 2009 19:08 |