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

[TurboGrid] Diffuser passage for radial compressor in ansys turbogrid

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 1, 2018, 03:05
Default Diffuser passage for radial compressor in ansys turbogrid
  #1
New Member
 
Vasudevan K
Join Date: Oct 2015
Posts: 13
Rep Power: 7
CFDvasu11 is on a distinguished road
Hi

I have curve files for the blade, hub and shroud. When I extend my curve file upstream of rotor blade, an inlet is automatically created in Turbogrid V18.1, but I am not getting the same result when I do it downstream of the blade in order to get the diffuser.
Also, I'm getting a message "No valid outlet mesh found, outlet is turned off" when I load my curve files.

Also if someone can tell me a way to create diffuser when I'm using curve files in data import wizard in Bladegen, It will be of great help as I'm struggling with both the methods.

Suggestions are welcome.
CFDvasu11 is offline   Reply With Quote

Old   March 1, 2018, 03:31
Default
  #2
Senior Member
 
M
Join Date: Dec 2017
Posts: 375
Rep Power: 7
AtoHM is on a distinguished road
Can you add an image of what TGrid does and what you expect it to do?
AtoHM is offline   Reply With Quote

Old   March 1, 2018, 04:42
Default
  #3
New Member
 
Vasudevan K
Join Date: Oct 2015
Posts: 13
Rep Power: 7
CFDvasu11 is on a distinguished road
Thanks for the reply. I have attached two photos with highlighted regions of interest.

The image named Turbogrid shows the geometry created by Turbodgrid when I used the curve files (area marked with free form should be diffuser). But it has mentioned it along rotor passage. You can see an inlet portion created sepeartely. I extended the curves upstream of the blades and the inlet domain was created automatically. When I tried the same no separate domain was created when i tried extending the curves downstream of rotor.

When i tried trimming the outlet, the extended portion of curve was not used as diffuser either (although I don't if it would) as shown in the image Turbogrid2.png

So I would to know as how generally a diffuser is modeled when I model my rotor in Turbogrid.
Attached Images
File Type: png TurboGrid.png (50.5 KB, 44 views)
File Type: png TurboGrid2.png (42.5 KB, 39 views)
CFDvasu11 is offline   Reply With Quote

Old   March 1, 2018, 05:02
Default
  #4
Senior Member
 
M
Join Date: Dec 2017
Posts: 375
Rep Power: 7
AtoHM is on a distinguished road
I am not a 100% sure, since I have only used it for axial turbomachinery yet, but I saw something similar there.

Basically, there are two ways to model the outlet one of which might give such a result. In the Mesh Data options -> Mesh Size and at the bottom, there are check boxes for Inlet and Outlet Domain. If you have "Outlet Domain" off, you are still able to model it, by manually setting outlet position (I think that is what you did?) at the Outlet Options. This I think can lead to this.
If you instead check the box to include it ("Outlet Domain" on), the region could be as you expect. Then, your option to "trim outlet" refers to the area, where TGrid "ends" the blade mesh and begins an outlet mesh with a set expansion ratio, which can be edited under Mesh Data -> Outlet.
I found this kind of confusing at the beginning as well, but once figured out, it is a good feature.
AtoHM is offline   Reply With Quote

Old   March 1, 2018, 07:23
Default
  #5
New Member
 
Vasudevan K
Join Date: Oct 2015
Posts: 13
Rep Power: 7
CFDvasu11 is on a distinguished road
Thanks AtoHM, I've tried what you suggested. But when I check the outlet domain box and click apply, it throws an error which says "the is no valid outlet domain to mesh. The outlet will be turned off".
I don't know why. I've also searched the internet for this error but no luck for me.
CFDvasu11 is offline   Reply With Quote

Old   March 1, 2018, 08:58
Default
  #6
Senior Member
 
M
Join Date: Dec 2017
Posts: 375
Rep Power: 7
AtoHM is on a distinguished road
First of all: yes this is exactly the problem I had and good news: this is going to help you get rid of it

The problem: you are giving TGrid shroud and hub contours. By using all of this data in the Outlet options (I guess you have "fully extend" active?), TGrid uses it. But, it does not know if your model actually includes an outlet or for example a veeeery long blade. So, you have to tell it which part of the contours you give belong to the blade and outlet regions respectively.

I added an image of my axial geometry, also recreating your error. There "fully extend" is used in Outlet options. TGrid tries to mesh blade and outlet in one run and gives this strange twisted geometry. Additionally telling it to include the outlet, it doesnt know how to handle that, since outlet is already meshed!

Now, to avoid this: go to Geometry->Outlet options. There, specify a trimming. Since you have a radial type, try a radius thats above the blade trailing edge but well below the maximum radius you gave in your contours. Let TGrid refresh the geometry. Now, since Outlet is still inactive in Mesh Data, go there and try to activate it. Should work. At the position where you trimmed the outlet, there should be a recognizeable split between blade and outlet mesh.

Excuse my Paint skills. I hope it still helps to resolve your issue.
Attached Images
File Type: png TGrid_outlet.PNG (84.8 KB, 34 views)
File Type: png TGrid_outlet_trim.PNG (85.3 KB, 37 views)
File Type: png withOutlet.PNG (78.1 KB, 37 views)
File Type: png withoutOutlet.PNG (59.7 KB, 37 views)
AtoHM is offline   Reply With Quote

Reply

Tags
bladegen, radial compressor, turbogrid

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
How to simulate a diffuser in ansys fluent Hello_Fluent FLUENT 8 February 26, 2019 20:47
Pro/E to ANSYS Parameterization Guide Trues ANSYS 4 April 18, 2018 05:52
Ansys CFX Turbogrid, Problem with blade leading edge sitting on hub at inlet Irondome CFX 9 August 18, 2016 18:56
[TurboGrid] GE rotor B geometry for Ansys turbogrid sonny ANSYS Meshing & Geometry 6 August 29, 2014 20:01
Exporting results from CFX to ANSYS ?? sohail ahmed CFX 1 December 20, 2007 01:10


All times are GMT -4. The time now is 14:37.