|
[Sponsors] |
How to define a specific valume of domain in CFX-post? |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
May 12, 2019, 05:33 |
How to define a specific valume of domain in CFX-post?
|
#1 |
Member
Hamda
Join Date: Jul 2018
Posts: 80
Rep Power: 7 |
Hi,
As you see in the following picture, there are several spheres and I want to select one of them to investigate Temperature, velocity and pressure distributions. How can to select this specific sphere in CFD-post? Thanks in advance |
|
May 12, 2019, 07:04 |
|
#2 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,710
Rep Power: 143 |
The easiest way is to define that sphere as a mesh region (in meshing), and then you can simply refer to it as a locator.
If you have not done that and you have to post process an existing run you have to define a function which isolates the sphere. This is not too hard for a sphere as it can simply be all points less than the radius from the centre point of that sphere. I will leave the maths of defining that function up to you for your enjoyment
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
May 25, 2019, 13:07 |
|
#3 | |
Member
Hamda
Join Date: Jul 2018
Posts: 80
Rep Power: 7 |
Quote:
Thank you for your response. could you explain me how to define such a function? it means an expression? or I should insert volume ? I already inserted volume and got some contours. |
||
May 25, 2019, 19:04 |
|
#4 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,710
Rep Power: 143 |
Define a variable in CFD-Post of the form x^2+y^2+z^2. Then draw contours of that function, and make an volume out of the contour which defines your sphere.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
May 26, 2019, 07:38 |
|
#5 | |
Member
Hamda
Join Date: Jul 2018
Posts: 80
Rep Power: 7 |
Quote:
I wrote an expression of the form of x^2+y^2+z^2 and then used it for a variable (called sphere) and then drew contour of that variable. I got the following pic. But my problem is that when I use the defined variable I can't draw contours of Nu, temperature .... |
||
May 26, 2019, 08:34 |
|
#6 |
Senior Member
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,832
Rep Power: 27 |
Don't create a function. And especially not a function of a sphere around (0,0,0). That is what you did.
You should create a volume around the center of your sphere of interest. Go to pull down menu, Insert, Volume, select sphere, add the center of your sphere select the radius of your sphere and select below intersection, to obtain a volume containing all elements inside your sphere. Simple. But this is all work afterwords. As Glenn mentioned, it is best to give names beforehand during meshing. Then it is easier to find them back in the postprocessing. |
|
May 26, 2019, 08:47 |
|
#7 | |
Member
Hamda
Join Date: Jul 2018
Posts: 80
Rep Power: 7 |
Quote:
Thank you for your response. As mentioned before I already did that: I inserted a volume and got some contours. |
||
May 26, 2019, 08:57 |
|
#8 |
Senior Member
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,832
Rep Power: 27 |
I don't know what you did because I can't see it.
- In the picture I can see that you defined 2 volumes, but they are not visible. So I can't see if you did the correct thing............. - I see a contour of Variable 1, which probably is your expression. And you plot this on your interface which is part of your existing geometry. And the center is at the bottom, probably (0,0,0) I repeat: You should create a volume around the center of your sphere of interest. Go to pull down menu, Insert, Volume, select sphere, add the center of your sphere select the radius of your sphere and select below intersection, to obtain a volume containing all elements inside your sphere. Simple. |
|
May 26, 2019, 09:23 |
|
#9 | |
Member
Hamda
Join Date: Jul 2018
Posts: 80
Rep Power: 7 |
Quote:
I already inserted a volume. and did what you said.Please look at the pic. |
||
May 26, 2019, 09:50 |
|
#10 | |
Senior Member
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,832
Rep Power: 27 |
Quote:
Briljant, than you initial question is answered, not? Here you can investigate its volume average temperature and outisde pressure distribution. |
||
May 26, 2019, 09:58 |
|
#11 |
Senior Member
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,832
Rep Power: 27 |
If you want to evaluate heat transfer, then you need this volume average temperature.
But for outside variables you need a surface just outside each sphere, not? Then, as Glenn already mentioned, take a step back and define unique names. The easiest way is to go back to your meshing, and give unique names to each sphere surface. Then in Post, create a user surface with "Offset From Surface" as input. This allows you to create a spherical surface around your each sphere at, as an example, 1mm from the surface. |
|
May 26, 2019, 10:25 |
|
#12 | |
Member
Hamda
Join Date: Jul 2018
Posts: 80
Rep Power: 7 |
Quote:
yeah But now I have another question. I wrote some expressions for Nu and htc and when I drew contours I got negative values for them. these are my expression Myhtc=Wall Heat Flux/(T-780[K]) Nu=Myhtc*0.06[m]/0.31[W m^-1 K^-1] But as you see in the pic. I got negative values for Nu. Is there any problem related to the expressions? |
||
May 26, 2019, 10:37 |
|
#13 |
Senior Member
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,832
Rep Power: 27 |
Nu must be positive indeed. But I cannot evaluate your equations exactly since I don't know what you are doing. Cooling, heating?
But isn't it just a matter of sign/direction/normal/definition? |
|
May 26, 2019, 11:16 |
|
#14 | |
Member
Hamda
Join Date: Jul 2018
Posts: 80
Rep Power: 7 |
Quote:
It is so weird to me too. Each sphere is fuel and generates heat(I already wrote an expression for energy source) and through the spheres , Helium moves and collects heat from fuel spheres. Are my expressions correct? I also checked wall heat flux on "domain interface 1 side 2" and it is negative too!! |
||
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Velocity in porous domain in CFX post | Chander | CFX | 5 | May 20, 2015 04:12 |
Missing math.h header | Travis | FLUENT | 4 | January 15, 2009 11:48 |
CFX Solver Memory Error | mike | CFX | 1 | March 19, 2008 07:22 |
Proper output of angle of attack in CFX post | Kevin | CFX | 3 | October 18, 2006 12:18 |
Two-Phase Buoyant Flow Issue | Miguel Baritto | CFX | 4 | August 31, 2006 12:02 |