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

Question about extrude command in pointwise16.04

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

Like Tree1Likes
  • 1 Post By cnsidero

Reply
 
LinkBack Thread Tools Display Modes
Old   March 11, 2013, 00:34
Post Question about extrude command in pointwise16.04
  #1
New Member
 
Join Date: Mar 2013
Posts: 9
Rep Power: 4
GJ_hit is on a distinguished road
Hi all
Thank you for your attention.
I am trying to simulate a 3D airplane in an unstructured mesh.
Now I want to create 10mm Boundary Layer by extruding(extrue -nomral command ) the unstructured domain into prism block for viscous simulation, but the extrusion stopped for negative skew jacobian at 1mm.

My model and the direction of the extrusion showed in picture 1
1.What should I do?
2.Which parameter I should pay attention.
3.If I don’t use the extrude-normal command, is there any good way to create prism block by Pointwise?

I need your help ,thank you.

Ps:
1.I tried to turn off the smoothing and change the different initial delta s but it doesn’t work.
2.I know if the spacing in the region A little bigger it will extrude better, but in this case I shouldn’t do this.
Attached Images
File Type: jpg picture1.jpg (60.6 KB, 36 views)
File Type: jpg picutre2.jpg (91.7 KB, 30 views)
GJ_hit is offline   Reply With Quote

Old   March 11, 2013, 20:24
Default
  #2
Senior Member
 
Chris Sideroff
Join Date: Mar 2009
Location: Ottawa, ON, CAN
Posts: 371
Rep Power: 12
cnsidero is on a distinguished road
Extruding layers from concave (internal) corners is always the most difficult because the layers from the opposing surfaces collide and cause the front to get mangled up.

Anyway, I put together a mesh that looks similar to yours to help diagnose the problem and offer a solution. You might want to try enabling the "Triangle Aspect" parameter. On my mesh (that looks like yours) I was only able to extrude 10 layers with Triangle Aspect off. Turning it on and I was able to get more than 25 layers. This parameter limits the smoothing of the triangles on the front as excessive smoothing can cause the triangles to pile up in the corner and thus inhibit layer growth. With this parameter on, the resulting triangles on the front will look more non-uniform (i.e. stretched) but you should get more layers.

You can also try increasing the Direction and Step Size Iterations under Relaxation. By doubling each of these (without Triangle Aspect) I was able to go from 10 to 17 layers. Modify these parameters in addition to the Triangle Aspect parameter should get you significantly more layers.

Let me know if that works, Chris

Quote:
Originally Posted by GJ_hit View Post
Hi all
Thank you for your attention.
I am trying to simulate a 3D airplane in an unstructured mesh.
Now I want to create 10mm Boundary Layer by extruding(extrue -nomral command ) the unstructured domain into prism block for viscous simulation, but the extrusion stopped for negative skew jacobian at 1mm.

My model and the direction of the extrusion showed in picture 1
1.What should I do?
2.Which parameter I should pay attention.
3.If I don’t use the extrude-normal command, is there any good way to create prism block by Pointwise?

I need your help ,thank you.

Ps:
1.I tried to turn off the smoothing and change the different initial delta s but it doesn’t work.
2.I know if the spacing in the region A little bigger it will extrude better, but in this case I shouldn’t do this.
mm.abdollahzadeh likes this.

Last edited by cnsidero; March 11, 2013 at 21:28.
cnsidero is offline   Reply With Quote

Old   March 12, 2013, 12:05
Default
  #3
New Member
 
Join Date: Mar 2013
Posts: 9
Rep Power: 4
GJ_hit is on a distinguished road
Thanks Chris Sideroff
I followed your advice and it workded well.

The triangle Aspect is very important in this case, I can get more layers by choosing it; Increasing the Direction Iteations is very useful but the quality of block is bad, cmobine these methods is a good way.

But it is also far away from the quantity i wanted , i think the size of the triangle near the corner limited the layers.
Commonly we must refine the grid near the corner for flowfield here changed drastically
1.Are there any other way to generate prism block in Pointwise?
2.Can I assemble the prism block manually just like in Gambit?

Thank you for your help

PS:Increasing the step size Iteration reduced the number of layers.
GJ_hit is offline   Reply With Quote

Old   March 13, 2013, 18:50
Default
  #4
Senior Member
 
Chris Sideroff
Join Date: Mar 2009
Location: Ottawa, ON, CAN
Posts: 371
Rep Power: 12
cnsidero is on a distinguished road
Quote:
Originally Posted by GJ_hit View Post
Thanks Chris Sideroff
But it is also far away from the quantity i wanted , i think the size of the triangle near the corner limited the layers.
Depends on what your definition of "quality" is. What solver are you using?

Quote:
1.Are there any other way to generate prism block in Pointwise?
You can try one of two other approaches. You could try creating a structured mesh (at least for the boundary layer). Structured blocks have the advantage that they can be created from either an extrusion or manually assembled. You would likely get the best quality mesh using a structured mesh but it will likely take a little longer to create.

The other approach is the anistropic tet mesher, aka T-Rex. Because T-Rex has the ability to combine the boundary layer tets into prisms, it will generally do a much better job with less effort at creating unstructured boundary layer meshes with prisms. You will need to use Pointwise V17 to be able to use to T-Rex. There's more info about it here: http://www.pointwise.com/T-Rex/

Quote:
2.Can I assemble the prism block manually just like in Gambit?
Unfortunately, it's not possible to manually assemble a prism block in Pointwise.

Quote:
Thank you for your help
No problem.

Last edited by cnsidero; March 13, 2013 at 21:57.
cnsidero is offline   Reply With Quote

Old   March 15, 2013, 00:48
Default
  #5
New Member
 
Join Date: Mar 2013
Posts: 9
Rep Power: 4
GJ_hit is on a distinguished road
Thank you very much
I have already created the BL with the structure block and prism block
Much obliged to you for your help
GJ_hit 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
small question about the functionalities of topological changes in OpenFoam ngj OpenFOAM Running, Solving & CFD 2 February 28, 2013 11:02
Question Re Engineering Data Source imnull ANSYS 0 March 5, 2012 14:51
Extrude 2d tetra mesh jose antonio ANSYS Meshing & Geometry 1 June 28, 2011 13:18
internal field question - PitzDaily Case atareen64 OpenFOAM Running, Solving & CFD 2 January 26, 2011 16:26
CHANNEL FLOW: a question and a request Carlos Main CFD Forum 4 August 23, 2002 05:55


All times are GMT -4. The time now is 10:05.