# Multiple inlet mass flow rate

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

 September 5, 2019, 09:16 Multiple inlet mass flow rate #1 Member   Join Date: Mar 2019 Posts: 81 Rep Power: 6 Dear Foamers, I am trying to simulate a geometry with multiple inlets (i.e. 5) and one outlet. I have created the mesh in Salome and grouped all the inlets under one name of Inlet. Then I assigned the mass flow rate boundary condition to Inlet by dividing the total flow to 5 (i.e. the number of inlets). I thought that it would be assigned to each individual inlet and when considered together they would add to the total amount. However, when checking the patch mass flow rate at inlets and outlet, it seems that 1/5 of the mass flow is going through . It seems counter intuitive for me to use the total mass flow rate (but seems like I have to do it). In that case, how would OpenFoam divide the flow rate? Would it be equally divided among all the inlets? Does anyone have experience in this regard? PS: the geometry is complicated and the mesh is huge so it takes a lot of time to test all the possibilities Makkus likes this.

 September 6, 2019, 04:06 #2 Senior Member   Tom Fahner Join Date: Mar 2009 Location: Breda, Netherlands Posts: 623 Rep Power: 31 Hi, All faces will get the average velocity that gives in total the supplied flow rate. So if all your inlets are the same size, every inlet will have the same flow rate, but if there is a difference in area for those inlets, there will be a difference in the flow rate per inlet. Regards, Tom

 September 6, 2019, 07:20 #3 Senior Member   Carlo_P Join Date: May 2019 Location: Italy Posts: 176 Rep Power: 7 I'm quite sure that OpenFoam thinks that all the patches are one patch called Inlet. So you have to apply the total mass flow, indipendet of the number of surfaces. I'm pretty sure. If you want, you can try a very simple pipes with two inlet and check the outlet massflow. I have to do in some months, so if you report the solution, I will aprreciated a lot.

September 6, 2019, 10:29
#4
Member

Join Date: Mar 2019
Posts: 81
Rep Power: 6
Quote:
 Originally Posted by tomf Hi, All faces will get the average velocity that gives in total the supplied flow rate. So if all your inlets are the same size, every inlet will have the same flow rate, but if there is a difference in area for those inlets, there will be a difference in the flow rate per inlet. Regards, Tom
Hi Tom,

Thank you very much for shedding light on this issue. Indeed, it is as you mentioned but I really do not get the motivation behind this to behave in this manner when dealing with mass flow rate. For my case, one of the inlets is smaller than the rest and now I have to remesh the geometry . I think the best case would be to have an option of some sort for the user to specify if they want an equal flow rate or different flow rates (depending on the cross-sectional area)

September 6, 2019, 10:33
#5
Member

Join Date: Mar 2019
Posts: 81
Rep Power: 6
Quote:
 Originally Posted by Carlo_P I'm quite sure that OpenFoam thinks that all the patches are one patch called Inlet. So you have to apply the total mass flow, indipendet of the number of surfaces. I'm pretty sure. If you want, you can try a very simple pipes with two inlet and check the outlet massflow. I have to do in some months, so if you report the solution, I will aprreciated a lot.

Yes, but if the patches have different size, OF will attribute different mass flow rates (which is not what I wanted). The outlet mass flow is equal to the assigned mass flow rate to Inlet in 0 directory (i.e. the total mass flow).

September 6, 2019, 10:42
#6
Senior Member

Tom Fahner
Join Date: Mar 2009
Location: Breda, Netherlands
Posts: 623
Rep Power: 31
Quote:
 Originally Posted by mm66 I think the best case would be to have an option of some sort for the user to specify if they want an equal flow rate or different flow rates (depending on the cross-sectional area)
Hi,

Unfortunately that goes against the philosophy of the whole code, which is based on unstructured polyhedral cells. This means that a face, belonging to a cell is not necessarily related to other faces in it's neighbourhood. So there is no way for the code to know if a particular face is geometrically close or not to another face of the same patch. So your idea has far more consequences than this remeshing. However you may get away with this by using the createPatch utility, which you can use to manipulate a mesh. Than you keep the mesh, but just rename the small inlet to inlet_small (or whatever you prefer). You should look up the functionality though.

Another option might be the use of the extrapolateProfile true setting, but your success may vary. I have had cases fail or show highly unphysical results when I used it.

Cheers,
Tom

 September 6, 2019, 11:04 #7 Senior Member   Carlo_P Join Date: May 2019 Location: Italy Posts: 176 Rep Power: 7 Why you can't use a fixed velocity? It would be the same for all the surfaces that compose the Inlet patch

September 6, 2019, 11:29
#8
Member

Join Date: Mar 2019
Posts: 81
Rep Power: 6
Quote:
 Originally Posted by Carlo_P Why you can't use a fixed velocity? It would be the same for all the surfaces that compose the Inlet patch

I wished it was like that. But the problem is that in this incompressible flow, the mass flow rate is the same among all inlets but not the velocity (due to the geometrical difference)...

 September 10, 2019, 10:09 #9 Senior Member   Yann Join Date: Apr 2012 Location: France Posts: 805 Rep Power: 24 Why not using several independent inlet patches instead of a single one?

September 10, 2019, 13:25
#10
Member

Join Date: Mar 2019
Posts: 81
Rep Power: 6
Quote:
 Originally Posted by Yann Why not using several independent inlet patches instead of a single one?
Yes, that was what I had to do at the end of the day...

 Tags mass flow rate bc, openfoam 1806, patch average, salome