CFD Online Discussion Forums

CFD Online Discussion Forums (
-   OpenFOAM Running, Solving & CFD (
-   -   patchInjection (

yingkun July 4, 2011 05:15

I use the coalChemistryFoam solver, the own simplifiedSiwek case is closed ,I change it to have one inlet and one outlet,and then I need to inject coal through the inlet ,so I use patchInjection instead of manualInjection which specifies the coal parcel positions,but when running,it always out of temperature range around Time = 0.15s
I think there may be something I missed in the patchInjection model,can anybody help me?

matejfor July 5, 2011 05:14

I do only isothermal particle flows at the moment, but from my previous experience with other codes these things may happen when:

* you introduce too much particles to one place, hence the source is too large - linearisation of the source may help or different particle distribution at inlet

* the volume fraction of particles near inlet gets too high - hence the source plays dirty with you as in previous case

* the time step is large - big source from reaction or evaporation know the story already

* the mesh quality -especially the concavity of the mesh is bad or skew brings numerical problem to the solution. Now it depends if you're using 1.6 or 1.7 OF where this could be bigger problem or you use 2.0 where the tracking has been rewritten.

try to write down some info on your particles to find out where and what happens.

good luck

yingkun July 6, 2011 05:05

1 Attachment(s)
Thank you for your reply!
you give me some good inspirations, I am going to check everyone of your suggestions,and I still have some thing confused:
1.the "volumeFlowRate" in patchInjection model means what? does it equal to "the volume fraction of particles near inlet" you said ?
2. the "parcelsPerSecond" is 1e5 in my case,is it alright?
3.I use OF1.7.1,does it matter something?
the accessories is my coalcloudproperties file
Attachment 8303

thank you!

matejfor July 6, 2011 15:43

Hi Ying,

ad 1 - the volumeFlowRate gives the m3/s of particles injected. When you look at the source <foam>/src/lagrangian/intermediate/submodels/Kinematic/injectionModel/PatchInjection/PatchInjection.C you will find the way the totalVolumeInjected is computed by integrating the volumeFlowRate over the patchInjectors and time.

ParcelsPerSecond is 1e5 ...well it depends :)...on what? on how many parcels you need to represent the dispersed phase. The more parcels you are integrating the more memory will be needed. The numbers I need for MY simulations are from 5000 to 50 000 parcels. But you should actually test your simulation for the sensitivity in your dispersed phase representation in a similar way you do your Grid independence study (now I believe you are a good boy and you are not skipping this, ey?).

I guess you may use 1.7.1 happily. I'm now testing the 2.0 as I had some stability issue in parallel computations with particles. You should only be aware that especially Lagrangian part of the code is rewritten significantly in version 2. which may or may affect your settings or coding, I'm not sure at the moment.

good luck

yingkun July 10, 2011 03:02

there an other question,what is the difference of inlet velocity between 0 file and coalcloudproperties /patchIjection file(while I using "inlet" patch as the injector)?

matejfor July 11, 2011 03:17

This is the easy one I know :).
in 0/lagrangian/<cloudName>/U you have velocities of the particles already present in the domain according to the 0/lagrangian/<cloudName>/position file.
The velocities in 0/U are the velocities of the continuous phase (air) and in the <case>/constant/<cloudName>Properites you have velocities of the injected particles which might or might not be the same as the air velocity.


All times are GMT -4. The time now is 18:53.