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

[ICEM] Moving from 2D to 3D mesh

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

Like Tree4Likes
  • 1 Post By bluebase
  • 2 Post By bluebase
  • 1 Post By bluebase

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   April 26, 2021, 09:49
Exclamation Moving from 2D to 3D mesh
  #1
New Member
 
Matthew Potts
Join Date: Apr 2021
Posts: 4
Rep Power: 2
mattpotts is on a distinguished road
Hello, I'm encountering a problem while trying to extrude my existing 2D mesh of a wing profile into 3D.

My 2D mesh is a rectangle with the edges listed as parts labelled as inlet, outlet, upperbound and lowerbound. I used this mesh in 2D simulations with these parts as my boundary conditions, calculating from the inlet.

I'm looking to simulate a uniform-span wing and note any 3D effects seen, so for the 3D mesh, I simply want the mesh to be repeated and remain constant across the span-length of the wing, and change the boundary conditions from being one edge each of the rectangular 2D mesh to being one face each of the cuboid 3D mesh.

My problem arises when I try and use the extrude mesh tool to copy my exiting 2D mesh into different planes. Although the mesh itself is the shape I desire, when I hide all parts except for the inlet, I can see that the inlet is still just one edge of the original mesh rather than being an entire face, and the same is true for the other three boundaries. Sure enough, when I open up the mesh in Fluent I'm not given the option of setting these four parts as boundary conditions.

Any help would be greatly appreciated, as I've been stuck on this problem for quite some time and nobody I've spoken to about it until now has had any idea how to fix this problem. Apologies if my explanation isn't particularly clear, this is my first time posting on one of these forums so I haven't much experience in trying to describe my problems in this manner.
mattpotts is offline   Reply With Quote

Old   April 26, 2021, 14:54
Default
  #2
Senior Member
 
Join Date: Nov 2020
Location: Canada
Posts: 332
Rep Power: 4
aero_head is on a distinguished road
Hello Matthew,

It would help to post photos along with your explanation in order to get a better idea of what the issue is.

It sounds like it is an issue with some of the faces/blocking potentially. So it would help, again, to see an image of the mesh along with an image of the blocking/relevant faces.
aero_head is offline   Reply With Quote

Old   April 27, 2021, 07:04
Question
  #3
New Member
 
Matthew Potts
Join Date: Apr 2021
Posts: 4
Rep Power: 2
mattpotts is on a distinguished road
The mesh is for a corrugated dragonfly wing profile

2d mesh.png
this is the original 2d mesh
list of parts.png
this is a list of the parts of the extruded mesh on icem
isometric.png
this is the isometric view of the extruded mesh

extrusion.png
this is the side view of the extruded mesh (don't worry about the low number of divisions; I'll refine the mesh once I've figured out the problem) - I want the "outlet" part to be this entire face so I can set it as a boundary condition on Fluent

hopefully these images help illustrate the problem, thank you for helping!
mattpotts is offline   Reply With Quote

Old   April 27, 2021, 16:37
Default
  #4
Senior Member
 
Sebastian Engel
Join Date: Jun 2011
Location: Germany
Posts: 557
Rep Power: 18
bluebase will become famous soon enough
Could you also please add a picture, or two, of the geometry entities - at least the bounding box.


I'd guess, that you still have only a 2D geometry. But as far as i know, boundary elements are only created when the are associated to geometry entites. Not having surfaces in your third coordinate would mean there is nothing to associate - leaving you with edges/blocks in internal mode.
Although internal blocks can be filled with elements, they are not covered by boundary elements which would construct a boundary part for the solver.
aero_head likes this.
bluebase is offline   Reply With Quote

Old   April 27, 2021, 21:24
Default
  #5
Senior Member
 
Join Date: Nov 2020
Location: Canada
Posts: 332
Rep Power: 4
aero_head is on a distinguished road
Quote:
Originally Posted by bluebase View Post
Could you also please add a picture, or two, of the geometry entities - at least the bounding box.


I'd guess, that you still have only a 2D geometry. But as far as i know, boundary elements are only created when the are associated to geometry entites. Not having surfaces in your third coordinate would mean there is nothing to associate - leaving you with edges/blocks in internal mode.
Although internal blocks can be filled with elements, they are not covered by boundary elements which would construct a boundary part for the solver.
Yes, sorry, this is what I wanted to observe as well, as it was my hunch that it was still being seen as
a 2D geometry as well. Thanks for wording it better - in the future I'll try to better explain what I'm looking for like you have done.
aero_head is offline   Reply With Quote

Old   April 28, 2021, 10:06
Question
  #6
New Member
 
Matthew Potts
Join Date: Apr 2021
Posts: 4
Rep Power: 2
mattpotts is on a distinguished road
Quote:
Originally Posted by bluebase View Post
Could you also please add a picture, or two, of the geometry entities - at least the bounding box.


I'd guess, that you still have only a 2D geometry. But as far as i know, boundary elements are only created when the are associated to geometry entites. Not having surfaces in your third coordinate would mean there is nothing to associate - leaving you with edges/blocks in internal mode.
Although internal blocks can be filled with elements, they are not covered by boundary elements which would construct a boundary part for the solver.
Ahhh I think you're correct about the geometry still only being 2D. I'm unsure how to show a picture of the bounding box but from toggling points in the geometry and vertices in the blocking I can see that only the points on the original face of the mesh are highlighted. How would I go about rectifying this problem?
mattpotts is offline   Reply With Quote

Old   April 28, 2021, 13:27
Default
  #7
Senior Member
 
Sebastian Engel
Join Date: Jun 2011
Location: Germany
Posts: 557
Rep Power: 18
bluebase will become famous soon enough
Quote:
Originally Posted by aero_head View Post
Yes, sorry, this is what I wanted to observe as well, as it was my hunch that it was still being seen as
a 2D geometry as well. Thanks for wording it better - in the future I'll try to better explain what I'm looking for like you have done.
It absolutely was not my intention to make you feel being corrected or to correct your answer (for which there also is no reason).





Quote:
Originally Posted by mattpotts View Post
Ahhh I think you're correct about the geometry still only being 2D. I'm unsure how to show a picture of the bounding box but from toggling points in the geometry and vertices in the blocking I can see that only the points on the original face of the mesh are highlighted. How would I go about rectifying this problem?

There are extrusion features for geometry entities as well. have a look into the create surface menus. Then copy the original surface representing the fluid domain to the "top" of the prisms to close it up.


Depending on how your somewhat wildly looking foil has been created and how fine your boundary elements become you might need to run build topology. Though save that step untill you actually run into problems with the newly created geos.
aero_head and mattpotts like this.
bluebase is offline   Reply With Quote

Old   April 28, 2021, 14:45
Default
  #8
Senior Member
 
Join Date: Nov 2020
Location: Canada
Posts: 332
Rep Power: 4
aero_head is on a distinguished road
[QUOTE=bluebase;802734]It absolutely was not my intention to make you feel being corrected or to correct your answer (for which there also is no reason).


Oh, sorry, it wasn't my intention to imply this, for the record I didn't feel at all like you were correcting me. I just liked your wording much better was all.

In my head your question was exactly what I wanted to ask, but the thought didn't reach my fingers. Meant more to thank you for this! Once again where my thoughts did not come out correctly.
aero_head is offline   Reply With Quote

Old   April 29, 2021, 10:06
Unhappy
  #9
New Member
 
Matthew Potts
Join Date: Apr 2021
Posts: 4
Rep Power: 2
mattpotts is on a distinguished road
Quote:
Originally Posted by bluebase View Post
It absolutely was not my intention to make you feel being corrected or to correct your answer (for which there also is no reason).








There are extrusion features for geometry entities as well. have a look into the create surface menus. Then copy the original surface representing the fluid domain to the "top" of the prisms to close it up.


Depending on how your somewhat wildly looking foil has been created and how fine your boundary elements become you might need to run build topology. Though save that step untill you actually run into problems with the newly created geos.
Sorry once again, but I've spent the past three hours trying to sort out the issue and have made little-to-no progress. Could you please explain what you mean by "copy the original surface representing the fluid domain to the "top" of the prisms to close it up"?

I've created rectangular surfaces over each edge of the domain and added them to their respective boundary parts, but this appears to have no effect on the mesh itself, as I can still only select all four edges simultaneously as a single boundary condition, when in actuality I want the inlet and lowerbound to be velocity-inlets and the outlet and upperbound to be outflows.

Having looked at a few tutorials it appears the extrude mesh function exists for cases wherein you simulate from the original solid to the extruded end, but I want to simulate from left to right, as I did in 2D. Is this therefore impossible?
mattpotts is offline   Reply With Quote

Old   April 30, 2021, 08:55
Default
  #10
Senior Member
 
Sebastian Engel
Join Date: Jun 2011
Location: Germany
Posts: 557
Rep Power: 18
bluebase will become famous soon enough
Sweep Curve is the actual feature name i forgot to mention. An snapshot from the manual:

Screenshot_20210430_144102.png


This feature extrudes only curves. So, if you would extrude a rectangle, sweeping would only create 4 surfaces from the original 4 curves. But to close the domain you need a surface inside the original rectangle, and close the 6th surface to close the cube.

If you did not have a a surface before to fill your 2D domain, then you now do need them to associate faces to these surface which enables the boundary element creation.


Look into the Transform Geometry menu for Translation. This feature will make it straight forward to copy a surface to an other location - you can use the same vector as you have used with sweep curve.






When extruding the 2D blocking to 3D, i suggest you to use the translate option. You should also use planar 2D blocking instead of surface blocking for the original blocking.






Quote:
Is this therefore impossible?
Yes, it absolutely is.
aero_head likes this.
bluebase is offline   Reply With Quote

Reply

Tags
3d meshing, boundary condition, extrude mesh, icem

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
[snappyHexMesh] SnappyHexMesh for internal Flow vishwa OpenFOAM Meshing & Mesh Conversion 24 June 27, 2016 08:54
Trying to set up Moving Mesh Problem dreamchaser CFX 5 December 15, 2014 00:07
snappyhexmesh remove blockmesh geometry philipp1 OpenFOAM Running, Solving & CFD 2 December 12, 2014 10:58
[Gmsh] 2D Mesh Generation Tutorial for GMSH aeroslacker OpenFOAM Meshing & Mesh Conversion 12 January 19, 2012 03:52
[snappyHexMesh] external flow with snappyHexMesh chelvistero OpenFOAM Meshing & Mesh Conversion 11 January 15, 2010 19:43


All times are GMT -4. The time now is 14:29.