Boundary type not appropriate to determine initial pressure

A subforum specific to the development of the OpenFoam-based workbenches ( Cfd https://github.com/qingfengxia/Cfd and CfdOF https://github.com/jaheyns/CfdOF )

Moderator: oliveroxtoby

Post Reply
poulmack
Posts: 12
Joined: Tue Nov 07, 2017 7:17 pm

Boundary type not appropriate to determine initial pressure

Post by poulmack »

Hi all,

I am running a simple simulation with an inlet of 0.1 kg/s and an outlet as open boundary (attached file). The mesh runs ok with cfMesh, but when trying to write the case, the following errors appear

Code: Select all

0.0: Error writing case:
0.0: RuntimeError: Boundary type not appropriate to determine initial pressure.
0.0: Write case setup file failed

Code: Select all


OpenFOAM v2206
cfMesh for V2206

Any help will be really appreciated.

OS: Windows 10 Version 2009
Word size of FreeCAD: 64-bit
Version: 0.20.29177 (Git)
Build type: Release
Branch: releases/FreeCAD-0-20
Hash: 68e337670e227889217652ddac593c93b5e8dc94
Python 3.8.10, Qt 5.15.2, Coin 4.0.1, Vtk 8.2.0, OCC 7.6.2
Locale: English/Canada (en_CA)
Installed mods: 
  * CfdOF 1.17.2
  * Help 1.0.3
  * ProDarkThemePreferencePack 1.0.0
Regards,
Paul
Attachments
Room split.FCStd
(35.76 KiB) Downloaded 35 times
Budahn
Posts: 15
Joined: Fri Jul 01, 2022 9:56 pm

Re: Boundary type not appropriate to determine initial pressure

Post by Budahn »

Go to initialize fields and put the pressure with specify value and it should work
poulmack
Posts: 12
Joined: Tue Nov 07, 2017 7:17 pm

Re: Boundary type not appropriate to determine initial pressure

Post by poulmack »

Thanks for your answer @Budahn ,

I did that and there is another error.

Code: Select all

Continuity error cannot be removed by adjusting the outflow.
Please check the velocity boundary conditions and/or run potentialFoam to initialise the outflow.
Total flux              : 1e-300
Specified mass inflow   : 0.083333333
Specified mass outflow  : 0
Adjustable mass outflow : 0
I understand that potential flow helps to converge easily, so that shouldn't be a problem/solution
Attachments
Room split.FCStd
(35.78 KiB) Downloaded 35 times
User avatar
oliveroxtoby
Posts: 810
Joined: Fri Dec 23, 2016 9:43 am
Location: South Africa

Re: Boundary type not appropriate to determine initial pressure

Post by oliveroxtoby »

poulmack wrote: Sun Jul 17, 2022 8:23 pm Hi all,

I am running a simple simulation with an inlet of 0.1 kg/s and an outlet as open boundary (attached file). The mesh runs ok with cfMesh, but when trying to write the case, the following errors appear

Code: Select all

0.0: Error writing case:
0.0: RuntimeError: Boundary type not appropriate to determine initial pressure.
0.0: Write case setup file failed
The problem is you have selected 'inlet' as the boundary to copy pressure from (in InitialiseFields). Since pressure isn't specified in that boundary type, it can't be used. Choose your 'open' bounary instead.
User avatar
oliveroxtoby
Posts: 810
Joined: Fri Dec 23, 2016 9:43 am
Location: South Africa

Re: Boundary type not appropriate to determine initial pressure

Post by oliveroxtoby »

poulmack wrote: Mon Jul 18, 2022 2:57 am Thanks for your answer @Budahn ,

I did that and there is another error.

Code: Select all

Continuity error cannot be removed by adjusting the outflow.
Please check the velocity boundary conditions and/or run potentialFoam to initialise the outflow.
Total flux              : 1e-300
Specified mass inflow   : 0.083333333
Specified mass outflow  : 0
Adjustable mass outflow : 0
The 'open' boundary isn't being picked up since that face doesn't exist on the object you are meshing. Changing the Part property of your mesh object from 'Body' to the 'BooleanFragments' object sorts it out. It should have given you a warning that the boundary is not matched though - I'll look into that.
Post Reply