CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > NUMECA

Different order of import mesh in IGG

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 29, 2016, 09:36
Default Different order of import mesh in IGG
  #1
New Member
 
Join Date: Sep 2011
Posts: 7
Rep Power: 7
dijiaqiu is on a distinguished road
Dear All

When i calculate the centrifugal compressor, i found different order of import volute and impller mesh in IGG, the result of efficiency is different. why?

Thank you
dijiaqiu is offline   Reply With Quote

Old   December 29, 2016, 18:22
Default
  #2
Senior Member
 
DarylMusashi's Avatar
 
Holger Dietrich
Join Date: Apr 2011
Location: Germany
Posts: 102
Rep Power: 8
DarylMusashi is on a distinguished road
Dear dijiaqiu,
Sorry, I don't understand the question. May you explain what you mean with "different order"?

Kind regards
Holger
DarylMusashi is offline   Reply With Quote

Old   December 29, 2016, 21:05
Default
  #3
New Member
 
Join Date: Sep 2011
Posts: 7
Rep Power: 7
dijiaqiu is on a distinguished road
Quote:
Originally Posted by DarylMusashi View Post
Dear dijiaqiu,
Sorry, I don't understand the question. May you explain what you mean with "different order"?

Kind regards
Holger
Sorry, I imported volute and impeller mesh in various different orders. For example, first I imported impeller mesh in IGG,then imported volute mesh. Or the reverse sequences. The result of efficiency is different.
dijiaqiu is offline   Reply With Quote

Old   December 29, 2016, 22:02
Default
  #4
Senior Member
 
DarylMusashi's Avatar
 
Holger Dietrich
Join Date: Apr 2011
Location: Germany
Posts: 102
Rep Power: 8
DarylMusashi is on a distinguished road
Dear dijiaqiu,
may I ask how much the efficiency differs in both cases? At a first glance I cannot explain this behavior. I suppose you are going to use FINE/Turbo for your project? Or are you going to proceed with an unstructured mesh (using FINE/Open)?

From my experience it is recommended to merge different meshes in AutoGrid (by creating a 3D effect) instead of using IGG if you want to use FINE/Turbo.
DarylMusashi is offline   Reply With Quote

Old   December 30, 2016, 09:29
Default
  #5
New Member
 
Join Date: Sep 2011
Posts: 7
Rep Power: 7
dijiaqiu is on a distinguished road
Dear DaryMusashi
I merged the meshes in AutoGrid (using FINE/Turbo).The efficiency differs is 5% ~ 10%. the interface between volute and impeller show different total pressure distribution. It's something wrong with the interface, How to check the interface mesh or compute setting is right?
dijiaqiu is offline   Reply With Quote

Old   December 30, 2016, 10:03
Default
  #6
Senior Member
 
DarylMusashi's Avatar
 
Holger Dietrich
Join Date: Apr 2011
Location: Germany
Posts: 102
Rep Power: 8
DarylMusashi is on a distinguished road
Dear dijiaqiu,
for further analysis I would recommend to set the integer expert parameter IWRIT = 1. The expert parameter settings are available under "Computation Steering -> Control Variables" and are only visible when you switch to "expert mode" in the top right corner of the GUI.

IWRIT=1 provides a more detailed report in the .mf file, which is located in your computation directory. You can open it with a text editor and analyse the flow values on both sides of your interfaces now. If everything is correct all flow variables are (nearly) equal on both sides. Maybe it will be helpful to share your insights of the analysis of both cases with us, if you want.

May I ask which type of interface you use for your computation and which relative Mach number your flow has near the interface?
DarylMusashi is offline   Reply With Quote

Old   January 1, 2017, 09:21
Default
  #7
New Member
 
Join Date: Sep 2011
Posts: 7
Rep Power: 7
dijiaqiu is on a distinguished road
Frist thank your help. the type of interface is Conservative Coupling by Pitchwise Row, near the interface relative Mach numeber is about 0.8.

May I ask what's the differences between merging different meshes in AutoGrid(by creating a 3D effect) and merging different meshes in IGG(by importing the project).

kind regards
dijiaqiu is offline   Reply With Quote

Old   January 1, 2017, 17:58
Default
  #8
Senior Member
 
DarylMusashi's Avatar
 
Holger Dietrich
Join Date: Apr 2011
Location: Germany
Posts: 102
Rep Power: 8
DarylMusashi is on a distinguished road
May I ask if you have been able to compare the flow variables on both sides of the interface in your both projects? Theoretically the values should be the same for both projects.

Secondly, have you duplicated your FINE/Turbo project and just linked the other mesh (with different loading order)? This should work without problems, as the resulting mesh is the same in both cases. I would recommend it here, because if you set up the second project manually it might be the case that you used different settings, which result in a different solution.

Have you compared the convergence of the flow variables? In which way do they differ? You can easily do it with the "Monitor" (start it in the top bar of the FINE/Turbo GUI) and load different solution files for comparison.

To answer your question: I prefer to combine projects in AutoGrid5 with 3D effects, as you have the ability to change the meshing parameter of the rows afterwards. Secondly exchanging data is faster, as you only need to exchange the .trb template file for the rows. So only the volute .cgns file (large) is needed for merging.

If you encounter Mach numbers near 1.0 in the region of your interface the "1D non reflecting" interface type might be better (with expert parameter LOCCOR=0). But as you use the same type of interface in both projects this is surely not the reason for the differing efficiency here.
DarylMusashi is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Gambit problems Althea FLUENT 22 January 4, 2017 04:19
Importing Multiple Meshes thomasnwalshiii OpenFOAM Meshing & Mesh Conversion 18 December 19, 2015 19:57
No layers in a small gap bobburnquist OpenFOAM Native Meshers: snappyHexMesh and Others 6 August 26, 2015 09:38
2nd order boundary conditions for 2nd order discretization? quarkz Main CFD Forum 30 December 26, 2011 08:12
mesh missing after import in fluent morteza08 FLUENT 0 July 23, 2010 02:22


All times are GMT -4. The time now is 18:25.