|
[Sponsors] |
Seven identical inlets to the volute, how should I define the interface? |
![]() |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
![]() |
![]() |
#1 |
Member
Join Date: Feb 2019
Posts: 37
Rep Power: 7 ![]() |
Hi all
I am studying a turbocharger on CFX: 7 sectors. I have done the whole turbocharger machine (7 sectors): inlet, impeller, diffuser and volute, it has about 26 million elements. At the workstation the computation time is expensive (around 15 hours) and I am thinking of reducing the problem by sacrificing some of the model, so I want to compute 1 sector, instead of 7, and then copy the outlet periodically around the input of the volute (360º). So I reduce the mesh to about 5 million elements (a big simplification): My problem is that I don't know how to define this condition in CFD-pre. The volute-diffuser interface is mixing-plane type. In short, the turbocharger with all sectors modeled is: ![]() very computationally expensive for modifications, and now I'm trying to calculate ONLY 1 sector (not all seven, like before) and connect them (all seven copies) to the inlet of the volute. But I do not know how to do it. And this happens to me: ![]() ![]() And I don't know how to replicate this passage (outlet repeated periodically around 360º of the volute inlet) seven times. How should i define it in CFD-PRE? Thank you very much, I'm a bit blocked. |
|
![]() |
![]() |
![]() |
![]() |
#2 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,816
Rep Power: 144 ![]() ![]() ![]() ![]() |
Have you looked at the CFX tutorials? They cover how to model segments of the rotor like this.
The CFX tutorials are available on the ANSYS Customer webpage or the ANSYS Academic page.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
![]() |
![]() |
![]() |
![]() |
#3 | |
Member
Join Date: Feb 2019
Posts: 37
Rep Power: 7 ![]() |
Quote:
I have seen all the tutorials. There is no tutorial about my question, that's why I ask it in this forum. If you know a tutorial about what I ask please tell me which one. |
||
![]() |
![]() |
![]() |
![]() |
#4 |
Senior Member
Join Date: Jun 2009
Posts: 1,850
Rep Power: 33 ![]() |
Not exactly sure about your question, but here is my take on explaining it
There should be a surface mesh on the volute side that represents the full circle for one side of the interface, and the other side is the surface mesh on the 1 sector side. Select the mixing plane model and you should be set. The software will replicate the surface mesh on the sector side for the missing part of the circumference and it will use the flow conditions from the "main sector" and impose those as the input flow into the volute. If you start your stream lines from the volute side of the interface they should start from all around the interface, do they not?
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
![]() |
![]() |
![]() |
![]() |
#5 | |
Member
Join Date: Feb 2019
Posts: 37
Rep Power: 7 ![]() |
Quote:
When I do that, CFX only calculates 1 sector in the entire 360º volute inlet (but within the volute there is only fluid from one sector, not from the others): ![]() In green is the volute interfase, then the sector connected to it. In this situation CFX calculates the flow of one sector in the volute, not the mix of all seven. I have: inlet+rotor+diffuser (with turbo-mode):
![]() I don't know what to modify, I am desperate with this. Thank you very much for your help. |
||
![]() |
![]() |
![]() |
![]() |
#6 |
Senior Member
Join Date: Jun 2009
Posts: 1,850
Rep Power: 33 ![]() |
Your plot is starting the streamlines from the inlet.
I suggested starting from the volute of the interface, not the inlet. How does it look starting from that way?
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
![]() |
![]() |
![]() |
![]() |
#7 | |
Member
Join Date: Feb 2019
Posts: 37
Rep Power: 7 ![]() |
Quote:
![]() The imbalance: ![]() The boundary conditions are: Inlet: total pressure and temperature. Outlet (volute): massflow. It is curious the imbalance in the volute. If I replicate within CFD-Post all sectors: ![]() So it doesn't seem like a CFD-Post or graphics problem. CFX has only calculated one sector discharging to the volute, not all seven. Thank you very much. Also, when I measure pressure etc, they are not correct values. |
||
![]() |
![]() |
![]() |
![]() |
#8 |
Member
Join Date: Feb 2019
Posts: 37
Rep Power: 7 ![]() |
![]() Could this be the problem? My analysis is in steady state. Also, the volute for compressors is not automated by ANSYS, it has to be made from scratch outside of ANSYS and then coupled with the diffuser. How can this be? CFX does not allow to calculate only one sector and then introduce seven of them in the volute? Maybe I'm trying something that can't be done in CFX |
|
![]() |
![]() |
![]() |
![]() |
#9 |
Senior Member
Join Date: Jun 2009
Posts: 1,850
Rep Power: 33 ![]() |
Not certain, but I think something if off in your setup.
Could you please post the "domain interface" section definition for your case? It would be interesting to see your frame change and pitch change model settings. Also, if you look into the output file, there should be a diagnostic section for such domain interface as well, could you please post that section? If the software is using only 1 sector against the 360 degree interface side, the non-overlap section should be 6/7 * 100, correct?
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
![]() |
![]() |
![]() |
![]() |
#10 | |
Member
Join Date: Feb 2019
Posts: 37
Rep Power: 7 ![]() |
Quote:
![]() ![]() ![]() ![]() ![]() Domain Interface Name : DIFFUSER to DIFFUSER Periodic 1 Discretization type = 1:1 Domain Interface Name : DIFFUSER to IMPELLER Discretization type = GGI Intersection type = Direct Non-overlap area fraction on side 1 = 0.00E+00 Non-overlap area fraction on side 2 = 0.00E+00 Pitch ratio ( user specified ) = 1.000 Pitch angle for side 1 [degrees] = 51.429 Pitch angle for side 2 [degrees] = 51.429 Domain Interface Name : DIFFUSER to VOLUTE Discretization type = GGI Intersection type = Direct Non-overlap area fraction on side 1 = 0.00E+00 Non-overlap area fraction on side 2 = 8.34E-01 Pitch ratio ( user specified ) = 1.000 Pitch angle for side 1 [degrees] = 51.429 Pitch angle for side 2 [degrees] = 360.000 Domain Interface Name : IMPELLER to IMPELLER Internal Discretization type = GGI Intersection type = Direct Non-overlap area fraction on side 1 = 4.37E-04 Non-overlap area fraction on side 2 = 5.50E-04 Domain Interface Name : IMPELLER to IMPELLER Internal 2 Discretization type = GGI Intersection type = Direct Non-overlap area fraction on side 1 = 4.96E-04 Non-overlap area fraction on side 2 = 5.25E-04 Domain Interface Name : IMPELLER to IMPELLER Periodic 1 Discretization type = 1:1 Domain Interface Name : IMPELLER to INLET Discretization type = GGI Intersection type = Direct Non-overlap area fraction on side 1 = 0.00E+00 Non-overlap area fraction on side 2 = 0.00E+00 Pitch ratio ( user specified ) = 1.000 Pitch angle for side 1 [degrees] = 51.429 Pitch angle for side 2 [degrees] = 51.429 Domain Interface Name : INLET to INLET Periodic 1 Discretization type = 1:1 I just tried pitch 51.429 side 1 and 51.429 side 2 (instead 360) and CFX solver gives me error: ERROR #555000005 has occurred in subroutine THETA_CONT_FIN. | | Message: | | | | A transition between +/-180 degrees could not be found on side 2 | | of domain interface: | | | | DIFFUSER to VOLUTE | | | | The algorithm which calculates this value attempts to search for | | the first element face at this transition. Sometimes this will | | fail if the pitch angle is incorrect. The pitch angle for this | | side of the interface is: 51.429 degrees. If this does not | | seem correct then please carefully examine your interface for any | | of the following: | | | | 1) side 2 has more than 360 degrees of revolution | | 2) side 2 intersects zero radius | | 3) side 2 has element faces normal AND parallel to the axis | | 4) side 2 has element faces at the low radial or axial position | | which are very thin in the axial or radial direction, or the | | edges which make up the inner radius/axial position do not form | | an arc of revolution so that the flow solver can accurately | | determine the pitch angle. | | | | If any of situations 1-3 apply you can try changing Transformation | | Type to "None" instead of "Automatic". If the 4th situation is | | the problem then you must explicitly specify the pitch angles | | of side 1 and 2 of the interface. You may have to change both | | settings to get the flow solver running. | +--------------------------------------------------------------------+ +--------------------------------------------------------------------+ | An error has occurred in cfx5solve: | | | | The ANSYS CFX partitioner exited with return code 1. | +-------------------------------------------------------------------- After reading that indication I think the problem is the cad or geometry of the volute inlet |
||
![]() |
![]() |
![]() |
![]() |
#11 |
Senior Member
Join Date: Jun 2009
Posts: 1,850
Rep Power: 33 ![]() |
May I ask why you have setup the Pitch Change model to Value = 1?
Your setup is definitely not a 1:1 pitch ratio by any means. I would use the Automatic option, and see what happens.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
![]() |
![]() |
![]() |
![]() |
#12 | |
Member
Join Date: Feb 2019
Posts: 37
Rep Power: 7 ![]() |
Quote:
I think the problem is the CAD or geometry of the volute inlet. I think it does not detect it as a surface of revolution. The volute was made out of ANSYS and exported to Spaceclaim The tongue area is very difficult to mesh, it gives many problems. |
||
![]() |
![]() |
![]() |
Tags |
cfx 16, turbo machinery |
|
|
![]() |
||||
Thread | Thread Starter | Forum | Replies | Last Post |
Table bounds warnings at: END OF TIME STEP | CFXer | CFX | 4 | July 16, 2020 23:44 |
Wrong flow in ratating domain problem | Sanyo | CFX | 17 | August 15, 2015 06:20 |
Installing OF 1.6 on Mac OS X | gschaider | OpenFOAM Installation | 129 | June 19, 2010 09:23 |
Convective Heat Transfer - Heat Exchanger | Mark | CFX | 6 | November 15, 2004 15:55 |
Replace periodic by inlet-outlet pair | lego | CFX | 3 | November 5, 2002 20:09 |