|
[Sponsors] |
Changing BC outlet with different BC from initival value |
![]() |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
![]() |
![]() |
#1 |
Senior Member
Daniel
Join Date: Feb 2017
Location: Germany
Posts: 165
Rep Power: 9 ![]() |
Hello,
kind of hard to find a right topic for this. I am currently trying to make a performance curve of a four-stage axial comrpessor. I have reference values of massflow rates which i need to achieve. The problem was that this setup has an average pressure at the outlet. So I needed to change the pressure and get hopefully the right massflow (kind of tricky but that should not be the focus right now). Now I want to start new with a massflow at the outlet (like recommended in the CFX guide). Is there a problem to use my current simulations with the ave pressure at outlet as initial value? Or does this only work when they both have the exact same BC? Cause last week when I started it quickly, there was an error. Do I need to interpolate something? Thank you very much ![]() |
|
![]() |
![]() |
![]() |
![]() |
#2 |
Senior Member
M
Join Date: Dec 2017
Posts: 692
Rep Power: 12 ![]() |
Why dont just run it without initial values and with the new massflow-BC and see what happens?
What was the exact error you got? It might not even be related to the BCs. |
|
![]() |
![]() |
![]() |
![]() |
#3 | |
Senior Member
Daniel
Join Date: Feb 2017
Location: Germany
Posts: 165
Rep Power: 9 ![]() |
Quote:
I got several Messages like the following: ______________________________________________ Parallel run: Received message from slave ----------------------------------------- Slave partition : 2 Slave routine : get_TWFTFC Master location : End of Continuity Loop Message label : 009100015 Message follows below - : +--------------------------------------------------------------------+ | ****** Notice ****** | | The non-dimensional near wall temperature (T+) has been clipped | | for calculation of Wall Heat Transfer Coefficient. | | | | Boundary Condition : S4 Hub | | T+ clip value = 1.0000E-10 | | | | If this situation persists and you are using the High Speed Model, | | consider enabling Mach number based blending between low speed and | | high speed wall functions. You can do so by specifying a Mach | | number threshold as follows: | | | | EXPERT PARAMETERS: | | highspeed wf mach threshold = 0.1 # default=0.0 (off) | | END | +--------------------------------------------------------------------+ +--------------------------------------------------------------------+ | Notice: The maximum Mach number is 4.325E+09. | +--------------------------------------------------------------------+ ================================================== ==================== OUTER LOOP ITERATION = 4 CPU SECONDS = 1.739E+03 ---------------------------------------------------------------------- | Equation | Rate | RMS Res | Max Res | Linear Solution | +----------------------+------+---------+---------+------------------+ +--------------------------------------------------------------------+ | ERROR #001100279 has occurred in subroutine ErrAction. | | Message: | | Floating point exception: Overflow | | | | | | | | | | | +--------------------------------------------------------------------+ |
||
![]() |
![]() |
![]() |
![]() |
#4 |
Senior Member
Daniel
Join Date: Feb 2017
Location: Germany
Posts: 165
Rep Power: 9 ![]() |
I guess i found a problem.
In my previous simulations I calculated the massFlow for the whole 360° model and set it as BC. Therefore the Mach-Number is damn high. But i needed to set only the massflow calculated for 1 passage I guess. |
|
![]() |
![]() |
![]() |
![]() |
#5 |
Senior Member
Join Date: Jun 2009
Posts: 1,850
Rep Power: 33 ![]() |
If you are building a performance curve using ANSYS tools, I advise you to use the "Exit Corrected Mass Flow" boundary condition for the whole range.
It will converge better than splitting the curve into a pressure outlet range, and a mass flow outlet range of simulations. The true physical mass flow is reported during the run; therefore, you can verify it is the intended mass flow for your plots. |
|
![]() |
![]() |
![]() |
|
|
![]() |
||||
Thread | Thread Starter | Forum | Replies | Last Post |
Strange Results at Tank Outlet with InterFoam | mgdenno | OpenFOAM | 18 | November 28, 2019 23:05 |
Generating water waves - backflow at the outlet | Luke92 | CFX | 1 | November 18, 2017 05:27 |
Volume fraction at outlet not known | Bisht | FLUENT | 8 | September 5, 2017 02:38 |
[PyFoam] Problems with the new PyFoam release | zfaraday | OpenFOAM Community Contributions | 13 | December 9, 2014 18:58 |
uncertain on model outlet definition | mactech001 | CFX | 0 | February 10, 2010 02:03 |