CFD Online Logo CFD Online URL
Home > Forums > Software User Forums > ANSYS > CFX

How to extrude 2D Mesh in ICEM CFD?

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

Like Tree1Likes
  • 1 Post By myron

LinkBack Thread Tools Search this Thread Display Modes
Old   December 24, 2006, 07:05
Default How to extrude 2D Mesh in ICEM CFD?
Posts: n/a
I am trying to extrude a 2D Mesh from a simple square geometry

this is what i am doing

1. Create the 2D geometry ((a square ) in X-Y plane

2. create a 3D Bounding Box. Give equal no: of nodes for each edge and see the premesh.

3. then I create a "curve", normal to one of the "points" of the square (distance equal to the cell size in the Z-direction)

4. Unless I convert the current mesh to unstructured by right-clicking on premesh, I dont see the Extrude Mesh option in the Mesh tab highlighted. (Is this the case?)

5. I use Extrude Mesh by curve option to create the 3D Mesh

6. When I click export to CFX, I see a warning in ICEM box, "the family BODY has mixed of 2D and 3D elements and this is not allowed in CFX -5"

What does the above error mean?

Is the procedure that I am following right? I am not using the "Extrude by element normal" method as it is giving large thickness in the Z-direction. One more thing, when to define parts in such a problem so that I can select location for a Boundary Condition later in CFX?

I hope somebody responds to my queries
  Reply With Quote

Old   December 24, 2006, 14:19
Default Re: How to extrude 2D Mesh in ICEM CFD?
Posts: n/a
You are doing 2D or 3D Simulation. If 2D than extruding one element thick in z or normal direction will definitely work. Procedure-> 1.Make 2D Geometry of Problem.Define Boundaries by parts. 2.Make a 2d Planar Block 3.Associate Edges to curve than associate vertices. 4.Specify no of nodes. 5.Premesh than convert the mesh into unstrutured(only the format) 7.Close Project.Than open only the mesh . 8.Extrude by normal method one element (2D) or more elementsif (3D can also define ur parts name in the extrude tool menu. 9.Save and import to CFX. I hope this will help and work.


  Reply With Quote

Old   December 26, 2006, 03:34
Default Re: How to extrude 2D Mesh in ICEM CFD?
Posts: n/a
Hi manu

Thanks a lot

But still everything doesnt seem to work as i want it to be

I am doing 3D simulation (Does CFX handle 2D simulations, I

dont think so.... My geometry doesnt require a 3D analysis,

so I want to make a 2D Mesh and extrude it to 3D

Please address the following things:

1. In the Extrude Mesh window that appears after clicking

on the icon, I select all the elements by typing "a". Even

If use the "Extrude by element normal" method with 1 layer

I see that the length/thickness/extrusion distance in the

third direction "z" is very large!!! Is there any means by

which this can be manipulated? Or is this absolutely

normal? Is there a way in which I can specify

the "extrusion distance" myself so that I can avoid this

system-default extrusion distance which in this case

appears to be very large...

2. In the Extrude Mesh window, there is provision for

defining part names. But it simply asks for name to be

given for the sides. In this case there are four sides but

not all of them will be assigned a similar boundary. I

could not make your "Define Bounadries by parts after

creating a 2D Geometry" strategy work

3. After exporting the mesh to CFX, I still see this

warning that " the body (name of the body that I created

before blocking) has mixed of 2D and 3D elements which is

not allowed in CFX -5" Can this warning be ignored

or does it have any impact?
  Reply With Quote

Old   December 26, 2006, 08:41
Default Re: How to extrude 2D Mesh in ICEM CFD?
Posts: n/a
Once you have loaded the 2D mesh - just a surface mesh - look at the parts list. My guess is that the surface mesh is in the part where you originally defined your 'body' to be (for the blocking). You'll probably want to move this surface mesh into a part for the representative surface.

I believe CFX requires one-element-thick mesh for a 2D analysis.

Mesh > Extrude Mesh. The volume part name is for the newly-created 3D elements. The Side Part is for the 'sides' of the extrusion. The Top Part is for the opposite end of the extrusion (the 'end' of the extrusion). You specify the Number of Layers and the Spacing Type. The Spacing Type default is set to 'Fixed' and a Spacing of 1. If you want a smaller extrusion layer, change the 'Spacing' value to your desired thickness. If you specify more than one layer, each layer has the 'Spacing' value.

Once you have the extruded mesh you can use the Parts branch to separate the surface mesh into appropriate groups. (Create parts, add to parts, etc.)
PrincessAngina likes this.
  Reply With Quote

Old   December 26, 2006, 23:11
Default Re: How to extrude 2D Mesh in ICEM CFD?
Posts: n/a
Hi Myron, Thanks a ton for the detailed mail!

I actually wanted to decrease the spacing of my extruded

mesh.But I wrongly called it thickness, hence the confusion

Now I have given a value of 0.01 for spacing and found the

mesh to my satisfaction.

Even I am able to assign mesh to desired parts

I just have one more question.

Is the solution influenced by the spacing value?Ideally

what should be the spacing value?

I tried out a simple problem both in 3D and and by this way

of extruding a 2D Mesh. I find that the solutions in both

the above cases are sufficiently close to each other

But I want to know if something can be done to bridge the

difference. Or is it that way only because we are making an

approximation in the case of extruded mesh?
  Reply With Quote

Old   December 27, 2006, 07:22
Default Re: How to extrude 2D Mesh in ICEM CFD?
Posts: n/a
I think in 2D Simulation Extrude distance has no effect bcoz there are no nodes in between the two at ends. But in 3D ( i.e more no of nodes in z directioin)it will greatly influence the result and that will ofcourse depend on the physics of the problem.If you want to do a transient case than definitely you should consider the proper extrude distance. Hope this is what u want to now???

  Reply With Quote

Old   December 27, 2006, 08:39
Default Re: How to extrude 2D Mesh in ICEM CFD?
Posts: n/a
Hi Manu,

I am really not able to understand what u mean by 2D and 3D?

Are you talking in relevance to CFX? Isnt what u are

getting by extruding also a 3D Mesh?
  Reply With Quote

Old   December 27, 2006, 11:58
Default Re: How to extrude 2D Mesh in ICEM CFD?
Posts: n/a
yes its all revence to CFX.Since you can not do a 2D Simulation directly in CFX so we somehow have to make the code fool by giving an element thick mesh.Yes its a 3D Mesh but not 3D Simulation.Thats wht i meant in previous post.
  Reply With Quote


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
ICEM CFD 5.0 - 2D to 3D Mesh Extrude James Date CFX 7 October 22, 2013 03:46
Loading previously saved mesh in ICEM CFD user0314 ANSYS Meshing & Geometry 1 September 20, 2011 12:46
[ICEM] Problem with volume mesh in ICEM CFD kolapoasafa ANSYS Meshing & Geometry 2 September 16, 2011 03:54
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 11:55
How to corse mesh in icem cfd? Priety CFX 2 October 2, 2006 03:57

All times are GMT -4. The time now is 13:14.