|
[Sponsors] |
Strange Velocity in impeller of MRFSimpleFOAM |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
April 11, 2008, 03:17 |
The case is on its way!
/E
|
#21 |
Member
|
The case is on its way!
/E |
|
April 11, 2008, 04:09 |
Hi what is your dimension for
|
#22 |
Senior Member
|
Hi what is your dimension for omega? 620.823rad/s or 620.832rpm
|
|
April 11, 2008, 04:49 |
MRFZone require rad/s. (You ca
|
#23 |
Member
Niklas Wikstrom
Join Date: Mar 2009
Posts: 86
Rep Power: 17 |
MRFZone require rad/s. (You can easily check the correct rotation velocity by looking at the tip velocity of the impeller blades.)
/Niklas |
|
April 11, 2008, 05:11 |
Hi Eric:
i am not quit sure
|
#24 |
Senior Member
|
Hi Eric:
i am not quit sure about you boundary but aftre 100 and more step the inlet vector looks strange too: wayne |
|
April 11, 2008, 08:12 |
Looks strange indeed! I'm runn
|
#25 |
Member
|
Looks strange indeed! I'm running the case to make sure I haven't made any stupid alterations that prevents it from converging.
Maybe my collegue Niklas can send you one of his cases? /Eric |
|
April 11, 2008, 09:15 |
Hi Wayne,
The case runs jus
|
#26 |
Member
|
Hi Wayne,
The case runs just fine here. Just let it run for some 500-1000 iterations, and it will look much nicer. The mesh is so coarse that you'll need to relax k and epsilon substantially (0.01 or 0.001) during the first 200-300 iterations, but it's typical OF behaviour. Also, you can reduce the non-orthogonal corrections to 0 to prevent the solver from holding on to a bad solution. /Eric |
|
April 11, 2008, 09:59 |
Hi Eric
thanks for you help
|
#27 |
Senior Member
|
Hi Eric
thanks for you help.what i am do not know how to set the boundary in OF, what i always do in CFX is : inlet -> massflow inlet (etc.Q kg/s) outlet -> average static pressure (0 pa) how can i define these boundaries? thank! wayne |
|
April 11, 2008, 10:29 |
by the ways
what is the SLIP
|
#28 |
Senior Member
|
by the ways
what is the SLIP boundary in your case ?in my case the hub and shroud are all rotating boundary like blade(i patch them in MRFZones file).and in CFX the hub and shroud are always in that way. any way if possible please let your collegue Niklas send me one of his cases.thanks! wayne |
|
April 14, 2008, 01:11 |
Hi
could you tell me how t
|
#29 |
Senior Member
|
Hi
could you tell me how to use the massFlowrateBoundary condition? in polymesh/boundary of 0/u? |
|
April 14, 2008, 03:09 |
Hi
I add to 0/U:
INLE
|
#30 |
Senior Member
|
Hi
I add to 0/U: INLET { type massFlowRateInletVelocity; massFlowRate 3.06; // Mass flow rate [kg/s] } the error is --> FOAM FATAL IO ERROR : keyword value is undefined in dictionary "/home/waynezw0618/OpenFOAM/waynezw0618-1 .4.1/run/impeller/./GS1/0/U::INLET" file: /home/waynezw0618/OpenFOAM/waynezw0618-1.4.1/run/impeller/./GS1/0/U::INLET from line 33 to line 36. From function dictionary::lookupEntry(const word& keyword) const in file db/dictionary/dictionary.C at line 146. how can i dfine the massflowratevelocity boundary? |
|
April 14, 2008, 03:57 |
Add 'value' statement to your
|
#31 |
Member
|
Add 'value' statement to your BC in U.
INLET { type massFlowRateInletVelocity; massFlowRate 3.06; // Mass flow rate [kg/s] value uniform 3.06; } |
|
April 14, 2008, 08:48 |
Hi Eric
what is value uniform
|
#32 |
Senior Member
|
Hi Eric
what is value uniform 3.06refer to? massflow rate or velocity? thanks wayne |
|
April 14, 2008, 08:54 |
I'm not sure about the impleme
|
#33 |
Member
|
I'm not sure about the implementation, but generally it implies the default starting value of the BC, in this case massflow rate. If you get an error post it here and I'll check it.
//Eric |
|
April 14, 2008, 23:21 |
Hi
it still do not works
if
|
#34 |
Senior Member
|
Hi
it still do not works if run without value uniform 3.06; error message is : --> FOAM FATAL IO ERROR : keyword value is undefined in dictionary "/home/waynezw0618/OpenFOAM/waynezw0618-1.4.1/run/tutorials/icoFoam/inlettry/0/U ::in" file: /home/waynezw0618/OpenFOAM/waynezw0618-1.4.1/run/tutorials/icoFoam/inlettry/0/U: :in from line 34 to line 35. From function dictionary::lookupEntry(const word& keyword) const in file db/dictionary/dictionary.C at line 146. FOAM exiting and if with red{value uniform 3.06; } the error is: --> FOAM FATAL IO ERROR : Expected a '(' while reading VectorSpace<form,>, found on line 36 the doubleScalar 3.06 file: /home/waynezw0618/OpenFOAM/waynezw0618-1.4.1/run/tutorials/icoFoam/inlettry/0/U: :value at line 36. From function Istream::readBegin(const char*) in file db/IOstreams/IOstreams/Istream.C at line 94. FOAM exiting i turn to Doxygen,and example of the BC specification:: inlet { type massFlowRateInletVelocity; massFlowRate 0.2; // Mass flow rate [kg/s] } how to ? |
|
April 15, 2008, 00:18 |
ok, then you need to write
|
#35 |
Member
|
ok, then you need to write
value uniform (0 0 0); /eric |
|
April 15, 2008, 00:34 |
Hi Eric
it can run with val
|
#36 |
Senior Member
|
Hi Eric
it can run with value uniform (0 0 0); but it looks like the boundary velocity is defined by (0 0 0),not as a massflowRateInletVelocity. and when i turn to Doxygen,there is no such construct of massFlowRateInletVelocity. can you tell me the details ? thanks wayne |
|
April 15, 2008, 02:35 |
Wayne,
As Eric said, you al
|
#37 | |
Senior Member
Mark Olesen
Join Date: Mar 2009
Location: https://olesenm.github.io/
Posts: 1,685
Rep Power: 40 |
Wayne,
As Eric said, you also need to add a 'value' entry to the dictionary. I.e., 'value' for generic initialization (you can consider it a placeholder) and the 'massFlowRate' is used for actually setting the boundary condition as a fixed massflow rate. At the following iterations you'll see that the 'value' field is indeed filled with the calculated velocity field on the boundary patch. As for your point Quote:
massFlowRateInletVelocityFvPatchVectorField ( const fvPatch&, const DimensionedField ...&, const dictionary& ); If in doubt, you should always take the source code as being authoritative. This is the really beauty of OpenFOAM - the algorithms are open for viewing and you can adjust them for your purposes. |
||
April 15, 2008, 23:38 |
Hi Mark
thanks for your reply
|
#38 |
Senior Member
|
Hi Mark
thanks for your reply,for i am not quite familiar with C++.so please excuse my question. in the construction \quote { massFlowRateInletVelocityFvPatchVectorField ( const fvPatch&, const DimensionedField ...&, const dictionary& ): fixValueFvPatchField<vector>(p,iF,dict) .... } and this construction will be initialized by fixValueFvPatchField<vector>(p,iF,dict),and then i turn fixValueFvPatchField to find relative construction.and it is initialized by: fvPatchField<type>(p,iF,Field<type>("value",dict,p .size())) and what is the "value" here? how does the "dict" works? by the way another quesion in the member function of massFlowRateInletVelocity there is operator==(n*avgU/rhop) what is the use of == ? is it overloaded the '==' operator for the volVectorField type as the "="? thanks wayne |
|
April 16, 2008, 02:36 |
Wayne,
The dictionary class
|
#39 |
Senior Member
Mark Olesen
Join Date: Mar 2009
Location: https://olesenm.github.io/
Posts: 1,685
Rep Power: 40 |
Wayne,
The dictionary class *is* explained in doxygen docs. It is also possible to follow the inheritance of the fixedmass patch via the doxygen docs to find out which class has implemented the 'operator==' (not to be confused with the 'operator='). Perhaps someone else on the forum would be kind enough to do the digging for you and explain it. Otherwise you'll have to do it yourself. A modicum of C++ knowledge might be useful. |
|
April 16, 2008, 22:30 |
Hi Mark
thanks!
wayne
|
#40 |
Senior Member
|
Hi Mark
thanks! wayne |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Equations in the MRFsimpleFOAM | waynezw0618 | OpenFOAM Running, Solving & CFD | 5 | May 7, 2015 04:43 |
Convergence with MRFSimpleFoam | grugg | OpenFOAM Running, Solving & CFD | 7 | March 28, 2014 04:56 |
MRFSimpleFoam | xdanielx | OpenFOAM Running, Solving & CFD | 0 | December 17, 2008 01:28 |
Strange Velocity | JoeSa | CFX | 1 | September 28, 2006 09:13 |
Strange oscillating velocity | zonexo | Main CFD Forum | 2 | April 6, 2006 11:38 |