CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

Seven identical inlets to the volute, how should I define the interface?

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

Like Tree3Likes
  • 1 Post By Opaque
  • 1 Post By Opaque
  • 1 Post By Opaque

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 4, 2021, 21:59
Default Seven identical inlets to the volute, how should I define the interface?
  #1
Member
 
Join Date: Feb 2019
Posts: 37
Rep Power: 7
jmenendez is on a distinguished road
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 (360).

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 360 of the volute inlet) seven times. How should i define it in CFD-PRE?

Thank you very much, I'm a bit blocked.
Attached Images
File Type: jpg 5.jpg (61.9 KB, 73 views)
File Type: png 7.png (117.2 KB, 63 views)
File Type: jpg 9.jpg (55.6 KB, 70 views)
jmenendez is offline   Reply With Quote

Old   February 5, 2021, 01:05
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,749
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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.
ghorrocks is offline   Reply With Quote

Old   February 5, 2021, 06:46
Default
  #3
Member
 
Join Date: Feb 2019
Posts: 37
Rep Power: 7
jmenendez is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
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.

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.
jmenendez is offline   Reply With Quote

Old   February 5, 2021, 09:03
Default
  #4
Senior Member
 
Join Date: Jun 2009
Posts: 1,825
Rep Power: 33
Opaque will become famous soon enough
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?
aero_head likes this.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
Opaque is offline   Reply With Quote

Old   February 5, 2021, 15:46
Default
  #5
Member
 
Join Date: Feb 2019
Posts: 37
Rep Power: 7
jmenendez is on a distinguished road
Quote:
Originally Posted by Opaque View Post
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?

When I do that, CFX only calculates 1 sector in the entire 360 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):
  1. Inlet: 1 passage per mesh, 1 passages to model; 7 passages in 360. Stationary
  2. Impeller: 1 passage per mesh, 1 passages to model; 7 passages in 360. Rotating
  3. Diffuser. 1 passage per mesh, 1 passages to model; 7 passages in 360. Rotating. Stationary
Then, the diffuser to volute interface:
  • Fluid-fluid.
  • Side 1, outet of 1 sector of diffuser (360/7)
  • Side 2, inlet volute (360)
  • General connection, mixing-plane (stage)
Once CFX (solver) has finished, CFX-Post only shows 1 passage connected to the whole volute:





I don't know what to modify, I am desperate with this. Thank you very much for your help.
jmenendez is offline   Reply With Quote

Old   February 5, 2021, 19:11
Default
  #6
Senior Member
 
Join Date: Jun 2009
Posts: 1,825
Rep Power: 33
Opaque will become famous soon enough
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?
aero_head likes this.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
Opaque is offline   Reply With Quote

Old   February 5, 2021, 22:29
Default
  #7
Member
 
Join Date: Feb 2019
Posts: 37
Rep Power: 7
jmenendez is on a distinguished road
Quote:
Originally Posted by Opaque View Post
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?
The situation is the same:



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.
Attached Images
File Type: jpg imba2.jpg (61.4 KB, 51 views)
File Type: png imbalance.png (58.0 KB, 50 views)
File Type: jpg ca.jpg (154.3 KB, 49 views)
jmenendez is offline   Reply With Quote

Old   February 7, 2021, 11:03
Default
  #8
Member
 
Join Date: Feb 2019
Posts: 37
Rep Power: 7
jmenendez is on a distinguished road


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
Attached Images
File Type: png 23.png (26.5 KB, 48 views)
jmenendez is offline   Reply With Quote

Old   February 8, 2021, 10:02
Default
  #9
Senior Member
 
Join Date: Jun 2009
Posts: 1,825
Rep Power: 33
Opaque will become famous soon enough
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.
Opaque is offline   Reply With Quote

Old   February 8, 2021, 22:10
Default
  #10
Member
 
Join Date: Feb 2019
Posts: 37
Rep Power: 7
jmenendez is on a distinguished road
Quote:
Originally Posted by Opaque View Post
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?










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
Attached Images
File Type: png 1.png (105.1 KB, 40 views)
File Type: png 2.png (69.4 KB, 39 views)
File Type: png 3.png (33.5 KB, 40 views)
File Type: png 4.png (22.5 KB, 41 views)
File Type: jpg 6.jpg (41.9 KB, 41 views)
jmenendez is offline   Reply With Quote

Old   February 9, 2021, 09:23
Default
  #11
Senior Member
 
Join Date: Jun 2009
Posts: 1,825
Rep Power: 33
Opaque will become famous soon enough
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.
jmenendez likes this.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
Opaque is offline   Reply With Quote

Old   February 9, 2021, 16:42
Default
  #12
Member
 
Join Date: Feb 2019
Posts: 37
Rep Power: 7
jmenendez is on a distinguished road
Quote:
Originally Posted by Opaque View Post
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.
I tried many different settings to see if it worked by modifying various options (including pitch ratio). Neither with automatic, nor any option worked.

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.
jmenendez is offline   Reply With Quote

Reply

Tags
cfx 16, turbo machinery

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
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


All times are GMT -4. The time now is 23:59.