CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Post-Processing

pressure drop using chtMultiRegionFoam

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

Like Tree3Likes
  • 1 Post By simrego
  • 2 Post By amdk136

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   November 30, 2018, 06:12
Default pressure drop using chtMultiRegionFoam
  #1
New Member
 
Arthur
Join Date: Oct 2018
Location: Glasgow
Posts: 20
Rep Power: 7
amdk136 is on a distinguished road
Hi,


I am trying to get the pressure drop between 2 different patches (inlet and outlet). In my controlDict I have included "#includeFunc patchAverage", and I have tried to use the postProcess -func patchAverage tool, however it tells me that I don't have a pressure field.

Code:
Reading fields:

Executing functionObjects
surfaceFieldValue patchAverage write:
--> FOAM Warning : 
    From function virtual bool Foam::functionObjects::fieldValues::surfaceFieldValue::write()
    in file fieldValues/surfaceFieldValue/surfaceFieldValue.C at line 807
    Requested field p not found in database and not processed


Time = 39.75
Within my simulations, I have a pressure difference as I have a pressure gradient (around 5 or 6). When I run the patchAverage on the outlet, I get the attached result (surfaceFieldData attached below).


I am using OpenFOAM 6, and I am unsure why it is not working. Is there a way to do this for specific patches within paraView instead of just OF? Can anyone help? Any help is appreciated!


Thank you,
Arthur
Attached Files
File Type: zip surfaceFieldValue.dat.zip (576 Bytes, 7 views)

Last edited by amdk136; November 30, 2018 at 06:22. Reason: adding info
amdk136 is offline   Reply With Quote

Old   December 2, 2018, 14:29
Default
  #2
Senior Member
 
anonymous
Join Date: Jan 2016
Posts: 416
Rep Power: 14
simrego is on a distinguished road
Hi!
In chtMultiRegionFoam you have regions. So you have to add the "-region regionName" switch to your command, where regionName is the name of the region where you have that patch.
simrego is offline   Reply With Quote

Old   December 3, 2018, 10:22
Default
  #3
New Member
 
Arthur
Join Date: Oct 2018
Location: Glasgow
Posts: 20
Rep Power: 7
amdk136 is on a distinguished road
Quote:
Originally Posted by simrego View Post
Hi!
In chtMultiRegionFoam you have regions. So you have to add the "-region regionName" switch to your command, where regionName is the name of the region where you have that patch.
Hi Simrego,

thank you for your reply! I have also tried with the "-region <region>", but when i do that I don't get a data file generated. After I posted this I tried just about every possible combination I could to no avail haha.

I'll assume it's a deeper rooted problem. Thanks for the help though!

Arthur
amdk136 is offline   Reply With Quote

Old   December 3, 2018, 10:38
Default
  #4
Senior Member
 
anonymous
Join Date: Jan 2016
Posts: 416
Rep Power: 14
simrego is on a distinguished road
Ooo sorry. Maybe I know your problem.
You just ran "postProcess -func patchAverage", right?
Try with "chtMultiRegionSimpleFoam -postProcess -func patchAverage -region <regionName>",
or you can use directly like:
chtMultiRegionSimpleFoam -postProcess -func "patchAverage(name=<patchName>, p)" -region <regionName>


I've just tried. This is working perfectly for me:
chtMultiRegionSimpleFoam -postProcess -func "patchAverage(name=inlet, p)" -region fluid -latestTime
amdk136 likes this.
simrego is offline   Reply With Quote

Old   December 4, 2018, 08:01
Default
  #5
New Member
 
Arthur
Join Date: Oct 2018
Location: Glasgow
Posts: 20
Rep Power: 7
amdk136 is on a distinguished road
Simrego,

Thank you again for your reply! I have tried that exactly how you have stated it, including the 'chtMultiRegionFoam' & also the 'region <region>' [as well as both with the "(name=patchName, field)" and without too], however no field data file is being created still.

Seems to be a very odd situation. I don't even get a post processing folder when I include the 'chtMultiRegionFoam' part.

Would it be possible for you to upload your case directory, please? So that I can see how you have it organised etc. And to see what I'm missing! (I understand if you'd rather not as well)

Thank you again,
Arthur
amdk136 is offline   Reply With Quote

Old   December 4, 2018, 15:41
Default
  #6
Senior Member
 
anonymous
Join Date: Jan 2016
Posts: 416
Rep Power: 14
simrego is on a distinguished road
Sorry, I can't share that case with you, but you can try it on any tutorial case. If it's not working I think the problem will be in your OF.
Maybe you are using an old version with a bug? Or had you any problems during the compilation? Or just a typo in the command? Or try with a different function, ie. patchIntegrate (just for a try).
simrego is offline   Reply With Quote

Old   December 5, 2018, 07:09
Default
  #7
New Member
 
Arthur
Join Date: Oct 2018
Location: Glasgow
Posts: 20
Rep Power: 7
amdk136 is on a distinguished road
Quote:
Originally Posted by simrego View Post
Sorry, I can't share that case with you, but you can try it on any tutorial case. If it's not working I think the problem will be in your OF.
Maybe you are using an old version with a bug? Or had you any problems during the compilation? Or just a typo in the command? Or try with a different function, ie. patchIntegrate (just for a try).

Simrego,



I have just run my case again and used the command you gave above (adapted for my case):
Code:
chtMultiRegionFoam -postProcess -func "patchAverage(name=cyclicFluidInlet, p_rgh)" -region water -latestTime

I was running the postProcess tool without "-latestTime" which was my problem as I didn't notice it on my phone. Posting again incase anyone else has the same problem as me



Thank you very much for your help again,
Arthur
wyldckat and hdotyao like this.
amdk136 is offline   Reply With Quote

Reply

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
Fluent cyclone pressure drop mkal FLUENT 1 February 20, 2020 01:55
How to plot pressure drop with Periodic BC? bigfans FLUENT 7 November 8, 2016 12:28
Pressure drop using Fan type BC Alexis Sack OpenFOAM Running, Solving & CFD 2 September 22, 2014 10:18
How to study pressure drop of continous phase in VOF model sajeesh FLUENT 4 February 5, 2014 23:01
Pipe Flow - Pressure Drop Daniel L FLOW-3D 2 December 10, 2010 05:23


All times are GMT -4. The time now is 04:56.