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

Circumferential average in CFD-Post

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   May 8, 2020, 11:43
Default Circumferential average in CFD-Post
  #1
New Member
 
Luca
Join Date: Jun 2017
Location: Italy
Posts: 5
Rep Power: 8
LuComet is on a distinguished road
Dear all,

I'm post-processing full annulus results of an axial compressor rotor in CFD-Post 16.1. Since the inlet conditions are not uniform, I want to export results for each blade passage. In particular, I want to export circumferentially-averaged spanwise profiles of inlet and outlet variables, in order to calculate for example the spanwise distribution of pressure ratio of one passage.

In the Turbo menu, I select the Turbo Regions of the domain considering the Mesh Regions of one passage, then I proceed with Initialize and Calculate velocity components. I set a Turbo Chart in order to generate the circumferential area-averaged spanwise profile of a variable (e.g. Total Pressure in Stn Frame ACA on Hub to Shroud Line). However, for different passages, the spanwise profiles of a variable are always the same, so I think that CFD-Post is averaging over the 360 and not over the domain that I specify

Any suggestions on how to calculate this circumferential average? Thank you for your time!
LuComet is offline   Reply With Quote

Old   May 14, 2020, 13:38
Default
  #2
New Member
 
Luca
Join Date: Jun 2017
Location: Italy
Posts: 5
Rep Power: 8
LuComet is on a distinguished road
After many trials I think I found the solution. Apparently the Hub to Shroud tool calculates the circumferential average of a variable over the entire domain, that is 360 for the full annulus case, regardless of what blade has been initialized, so I abandoned the idea of the separate initializations. Therefore, to export the spanwise trend of data (e.g. pressure ratio) pitch-averaged over a specified Theta interval (e.g. one channel between two blades) I scripted the following procedure:

1) create User Surface A on the INFLOW Mesh Region of one blade passage, and rotate it around the rotor axis in order to match the channel inlet between two blades (see channel1.png)

2) create a Contour of Span Normalized on surface A, with a certain number of levels

3) for each level i create a User Surface Bi (see channel1.png, green surfaces)

4) for each surface Bi define an expression: p0iCalc = areaAve(Total Pressure in Stn Frame)@User Surface Bi, and link it to a variable p0i

5) create a Turbo Line or any suitable location (maybe even a point would do, as the p0i are constants), go to File > Export, and select all the p0i. A spanwise distribution of total pressure, pitch-averaged over a blade channel, will be exported

6) create a Turbo Surface C at constant blade aligned, and place it at the channel outlet, i.e. at the blade TE (see channel1.png, red surface)

7) move the Contour on surface C. The surfaces Bi will move together with the Contour, and the variables will update accordingly

8) repeat the data export and perform the ratio between the two total pressure trends, in order to get the spanwsie distribution of pitch-averaged pressure ratio

I placed the second surface at the TE of the blades and not at the outlet of the CFD domain for the following reason. The rotor I'm studying is characterized by non-uniform inlet flow, so each channel has different inlet conditions. Downstream of the TE, fluxes coming from different channels are mixed together, and the periodicity principle is not standing anymore. So the control volume of a single channel has to be defined (see channel2.png), without intercepting streamlines coming from nearby channels.

I tested this method extending the Theta interval to the whole 360, and as expected I got the same results of the Hub to Shroud tool.

I will be happy of updating this procedure if anyone knows a simpler approach
Attached Images
File Type: png channel1.png (52.4 KB, 88 views)
File Type: jpg channel2.jpg (139.4 KB, 77 views)

Last edited by LuComet; May 15, 2020 at 13:09.
LuComet is offline   Reply With Quote

Reply

Tags
360, cfd - post, circumferential average, full annulus, hub to shroud

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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
y+ and u+ values with low-Re RANS turbulence models: utility + testcase florian_krause OpenFOAM 114 August 23, 2023 05:37
CFD Design...The CFD Future John C. Chien Main CFD Forum 20 November 19, 2015 23:40
Average Velocity in CFD Post amin.z CFX 10 July 7, 2015 18:57
static enthalpy calculation in CFD Post newbie384 CFX 2 March 22, 2014 07:28
CFD Post Streamlines better representation? Dr. Flow Squad CFX 2 January 20, 2014 13:48


All times are GMT -4. The time now is 22:28.