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

[ANSYS Meshing] inflating sweep method

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

Like Tree12Likes
  • 1 Post By blazejpop
  • 10 Post By cubejan
  • 1 Post By NaveenCFD

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   January 5, 2014, 16:54
Default inflating sweep method
  #1
Member
 
Błażej Popławski
Join Date: Jul 2013
Posts: 34
Rep Power: 11
blazejpop is on a distinguished road
Hello guys.

I'm trying to mesh fluid domain around duct of the propeller with sweep method. It works good, but when I try to add inflation it's automatically deactivated because of "Invalid method". I don't know what I'm doing wrong. Can anyone help me with this issue?

I'm adding a picture of inflation and sweep method details.
Attached Images
File Type: jpg inflation.jpg (50.3 KB, 358 views)
File Type: jpg sweep.jpg (52.3 KB, 321 views)
blazejpop is offline   Reply With Quote

Old   January 6, 2014, 07:38
Default
  #2
Member
 
Błażej Popławski
Join Date: Jul 2013
Posts: 34
Rep Power: 11
blazejpop is on a distinguished road
OK. So the answer is: inflation is automatically deactivated when the mapped face meshing is enabled.

Can anyone tell me why?
ana_mg likes this.

Last edited by blazejpop; January 6, 2014 at 17:36.
blazejpop is offline   Reply With Quote

Old   June 18, 2014, 09:48
Default
  #3
New Member
 
Julien Grün
Join Date: Jun 2014
Posts: 1
Rep Power: 0
juliengrun is on a distinguished road
Same problem as you, mapped Faces lock inflation.
I read the Ansys Mesher User Guide, lot of informations about inflation include parameters, auto-inflation... But nothing about the relation between
Mapped Face and Inflation.

Someone can explain us the problem or an Idea to solve the problem.

I try to make my Own Mesh of A Naca Airfoil.
Here is a Naca0012 with a correct Mesh (Mapped face and Inflation I presume)
Attached Images
File Type: jpg Nodes.jpg (82.5 KB, 187 views)
juliengrun is offline   Reply With Quote

Old   June 19, 2014, 08:28
Default
  #4
Member
 
Błażej Popławski
Join Date: Jul 2013
Posts: 34
Rep Power: 11
blazejpop is on a distinguished road
You can try some "pseudo-inflation" in such cases as yours by adding biasing and division options, but in complex geometries it will be a big problem.
I still don't know the answer for the question posed in this topic.
blazejpop is offline   Reply With Quote

Old   November 7, 2014, 09:55
Default
  #5
New Member
 
Jan Schulz
Join Date: Nov 2014
Posts: 2
Rep Power: 0
cubejan is on a distinguished road
To inflate a sweep method, you need to name a manual source face in the sweep options.
After this right mouse button on the sweep method in the tree outline-->inflate this method.

As far as I understand:
sweep inflation works in 2d, ansys meshes the source face with inflation layers and sweeps this face through the body. (possible boundaries are only edges, not faces like in the normal inflation method)

the normal inflation method works in 3d, you can select all the faces, which need inflation
cubejan is offline   Reply With Quote

Old   June 30, 2016, 06:19
Default
  #6
Member
 
Omid Shekari
Join Date: Jun 2016
Posts: 43
Rep Power: 8
Omish is on a distinguished road
Hi
If you add inflation by RC on mesh and inserting inflation, yes it'll be deactivated automatically with either sweep mode or multizone mode. But the solution to add inflation is to do this: LC on mesh, and search for inflation tab in details view (below "outline view") and use it as you did the previous way. But there's still a weird problem. I've tried this in only one single gometry (a U-shape pipe) and it didn't make any change. I'd made the Min sizing in to a small amount, and there was already an automatic structured fine mesh with sweep method, but without inflation for edges. Then I added inflation but after generating nothing changed. It might work for you. If you tried it please let me know about the result.
And a good suggestion for you. Use "point wise" for this mesh. It's very user friendly and easy to use after watching a tutorial on youtube "getting started with pointwise" and the meshing process becomes very short with fantastic result.
Omish is offline   Reply With Quote

Old   July 27, 2017, 10:23
Default Sweeping Boundary Layer
  #7
New Member
 
Marc
Join Date: Jun 2012
Location: Glasgow
Posts: 8
Rep Power: 12
laingmj is on a distinguished road
All you have to do is turn on manual source and target in the weeping options. Once you have done that select the face as the geometry and the edge as the boundary.

Job done
__________________
Marc
laingmj is offline   Reply With Quote

Old   March 11, 2019, 05:25
Thumbs up Solved
  #8
New Member
 
Naveen
Join Date: Mar 2019
Posts: 1
Rep Power: 0
NaveenCFD is on a distinguished road
Hi
I faced similar problem and after some trials I found the solution. In my case I have a large cylinder (pressure plenum), from which small cylindrical outlet pipes (6 nos) are projecting outward. I wish to have swept mesh with inflation in all the six pipes and unstructured mesh with inflation in the plenum. Towards this the plenum is suppressed first and all the six cylindrical pipes stay unconnected with each other. Then by Right click on the "mesh" select method and select sweep, select the pipe for body and the source face as the free end of pipe. then RC on the sweep (below mesh in tree) select inflation, select the free face and for boundary select the edge surrounding the face. Do the same for all pipes one by one. Then un-suppress the plenum and give the inflation for it and update the mesh. Hope it works for others
betterglobe likes this.
NaveenCFD is offline   Reply With Quote

Reply

Tags
inflation, sweep

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
On the alpha Eqn of VOF method when using Immersed boundary method in OpenFOAM keepfit OpenFOAM 4 January 31, 2014 15:32
[ANSYS Meshing] 2D Sweep Method austin.m ANSYS Meshing & Geometry 0 July 19, 2012 11:22
[ANSYS Meshing] Method: Sweep with Quads peterputer ANSYS Meshing & Geometry 0 July 18, 2012 14:22
[Gmsh] discretizer - gmshToFoam Andyjoe OpenFOAM Meshing & Mesh Conversion 13 March 14, 2012 05:35
Code for most powerfull FDV Method D.S.Nasan Main CFD Forum 6 September 4, 2008 03:08


All times are GMT -4. The time now is 19:50.