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

Generate a c topology mesh of an airfoil

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

Like Tree2Likes
  • 1 Post By cnsidero
  • 1 Post By cnsidero

Reply
 
LinkBack Thread Tools Display Modes
Old   October 17, 2013, 09:37
Smile Generate a c topology mesh of an airfoil
  #1
Fly
New Member
 
Sun Yu
Join Date: Oct 2013
Location: Singapore
Posts: 7
Rep Power: 3
Fly is on a distinguished road
Dear all,

I want to a c type mesh around airfoil NACA 0012. I am a new user of Pointwise and I think my application is something wrong. The followings are my steps:

1. import the airfoil geometry and set the dimensions of top and bottom edges of airfoil

2. create a 2-point curve which is the wake edge, the dimension is also set properly. The interval at the trailing edge is almost the same with that at the beginning of wake edge.


3. Create -->Extrude--> Normal
pick the domain in excessive order (wake edge-->bottom edge--> top edge--->wake edge)
set the initial step size and then run 80 steps

The following are my result. It can be seen that the mesh quality is not bad at the trailing edge. However, at the far field boundary, it is weird. Hope to get some advice from you guys. Thank you very much.
Attached Images
File Type: jpg mesh.jpg (37.9 KB, 172 views)
File Type: jpg mesh2.jpg (41.2 KB, 120 views)
Fly is offline   Reply With Quote

Old   October 17, 2013, 10:06
Default
  #2
Senior Member
 
Chris Sideroff
Join Date: Mar 2009
Location: Ottawa, ON, CAN
Posts: 369
Rep Power: 12
cnsidero is on a distinguished road
Quote:
Originally Posted by Fly View Post
Dear all,

I want to a c type mesh around airfoil NACA 0012. I am a new user of Pointwise and I think my application is something wrong. The followings are my steps:

1. import the airfoil geometry and set the dimensions of top and bottom edges of airfoil

2. create a 2-point curve which is the wake edge, the dimension is also set properly. The interval at the trailing edge is almost the same with that at the beginning of wake edge.


3. Create -->Extrude--> Normal
pick the domain in excessive order (wake edge-->bottom edge--> top edge--->wake edge)
set the initial step size and then run 80 steps

The following are my result. It can be seen that the mesh quality is not bad at the trailing edge. However, at the far field boundary, it is weird. Hope to get some advice from you guys. Thank you very much.
Sun thanks for your post and picture (worth a thousand words;-) To correct the behavior of the extrusion at the end of the wake connector you need to set a boundary condition there. When in the normal extrusion panel (before running the extrusion) go to the Boundary Condition tab, select the end of the wake connector, pick a BC type and click Apply.

If x is your streamwise direction choose either Constant X or Symmetry X. This will make extrusion at the end of the connector only progress in the vertical direction (Y). Note: the difference between Constant and Symmetry is that Symmetry will keep the grid lines at that boundary normal. This is generally only necessary if you are creating a symmetric grid and truly want the grid lines to be normal to the symmetry plane.

-Chris
taxalian likes this.
cnsidero is offline   Reply With Quote

Old   October 18, 2013, 00:00
Default
  #3
Fly
New Member
 
Sun Yu
Join Date: Oct 2013
Location: Singapore
Posts: 7
Rep Power: 3
Fly is on a distinguished road
Hi Chris,

Thank you very much for your reply.

I tried your suggestion, but the problem is not solved. When it runs about 50 steps, it crashed. I think it is because the extrusion interval at the airfoil is much bigger than that at the wake edge (see the picture). But, I choose geometry progression method and set the initial step size and growth rate for both airfoil and wake edge before running the extrusion. I can not figure out why.

Another picture is the geometry I need.

Sun

Quote:
Originally Posted by cnsidero View Post
Sun thanks for your post and picture (worth a thousand words;-) To correct the behavior of the extrusion at the end of the wake connector you need to set a boundary condition there. When in the normal extrusion panel (before running the extrusion) go to the Boundary Condition tab, select the end of the wake connector, pick a BC type and click Apply.

If x is your streamwise direction choose either Constant X or Symmetry X. This will make extrusion at the end of the connector only progress in the vertical direction (Y). Note: the difference between Constant and Symmetry is that Symmetry will keep the grid lines at that boundary normal. This is generally only necessary if you are creating a symmetric grid and truly want the grid lines to be normal to the symmetry plane.

-Chris
Attached Images
File Type: jpg mesh.jpg (71.0 KB, 92 views)
File Type: jpg c mesh.jpg (96.0 KB, 99 views)
Fly is offline   Reply With Quote

Old   October 18, 2013, 05:30
Default
  #4
Senior Member
 
Join Date: Nov 2010
Posts: 128
Rep Power: 6
taxalian is on a distinguished road
Hi Fly,

In addition to what Chris recommended, please try with changing the extrusion method from hyperbolic to algebraic i.e.
Create -->Extrude--> Normal --> Attributes Tab --> Extrusion Method --> Algebraic

I have also attached a simple c type grid with normal extrusion using algebraic method.

Quote:
Originally Posted by Fly View Post
Hi Chris,

Thank you very much for your reply.

I tried your suggestion, but the problem is not solved. When it runs about 50 steps, it crashed. I think it is because the extrusion interval at the airfoil is much bigger than that at the wake edge (see the picture). But, I choose geometry progression method and set the initial step size and growth rate for both airfoil and wake edge before running the extrusion. I can not figure out why.

Another picture is the geometry I need.

Sun
Attached Images
File Type: jpg c-topology mesh.jpg (56.1 KB, 85 views)
taxalian is offline   Reply With Quote

Old   October 18, 2013, 09:18
Default
  #5
Fly
New Member
 
Sun Yu
Join Date: Oct 2013
Location: Singapore
Posts: 7
Rep Power: 3
Fly is on a distinguished road
Hi, Taxalian,

Thank you so much for your suggestion. The mesh is so great in your picture.

I tried your way, but the extrusion will stop after some steps, my result is attached.

I am wondering if I had set up something wrong. Could you guide me the way you create the mesh?

Thanks again.

Quote:
Originally Posted by taxalian View Post
Hi Fly,

In addition to what Chris recommended, please try with changing the extrusion method from hyperbolic to algebraic i.e.
Create -->Extrude--> Normal --> Attributes Tab --> Extrusion Method --> Algebraic

I have also attached a simple c type grid with normal extrusion using algebraic method.
Attached Images
File Type: jpg c mesh.jpg (80.2 KB, 70 views)
Fly is offline   Reply With Quote

Old   October 18, 2013, 11:00
Default
  #6
Senior Member
 
Chris Sideroff
Join Date: Mar 2009
Location: Ottawa, ON, CAN
Posts: 369
Rep Power: 12
cnsidero is on a distinguished road
Quote:
Originally Posted by Fly View Post
Hi Chris,

Thank you very much for your reply.

I tried your suggestion, but the problem is not solved. When it runs about 50 steps, it crashed. I think it is because the extrusion interval at the airfoil is much bigger than that at the wake edge (see the picture). But, I choose geometry progression method and set the initial step size and growth rate for both airfoil and wake edge before running the extrusion. I can not figure out why.

Another picture is the geometry I need.

Sun
Use the hyperbolic method for this mesh. To correct the behavior you're seeing you need to the modify the volume smoothing parameter in the Attributes tab under Smooth Parameters. Specifically, you should lower to a small value for the first portion of the extrusion and then increase later in the extrusion.

For example, if you wanted to extrude for 80 total steps I would set the volume smoothing to 0.05 for the first 20, increase it to 0.1 for the next 20, increase it to 0.3 for the next 20 and set it to the default 0.5 for the last 20.

That's just an example so you're likely going to have to adjust your values to get the desired result but it gives you a basic template to follow.

Let me know how it goes, Chris
cnsidero is offline   Reply With Quote

Old   October 18, 2013, 12:06
Default
  #7
Senior Member
 
Join Date: Nov 2010
Posts: 128
Rep Power: 6
taxalian is on a distinguished road
If you want to use hyperbolic method, then simply follow Chris's instructions.
But in order to get also reasonably good c-mesh with algebraic extrusion you also need to increase the number of step and direction iterations in the attributes tab. Also start initially with smaller growth rate of about 1.1 to 1.05 and after some few iterations increase the growth rate. By doing this you will get a good nice mesh, of course in your case you need to fine tune the parameters to get the desired mesh.
taxalian is offline   Reply With Quote

Old   October 19, 2013, 06:39
Default
  #8
Fly
New Member
 
Sun Yu
Join Date: Oct 2013
Location: Singapore
Posts: 7
Rep Power: 3
Fly is on a distinguished road
Hi Chrish,

I tried your idea and it does work to improve the mesh. The attachment is my best result.

I have no idea about the meaning of volume smoothing parameter even after I read the explanation in the user manual book. Thus, I have to try to guess the value in this case. It is depressing that I cannot repeat my result after numerous attempts.

My general idea is to increase the "volume" value in every 5 steps, the minimum value is 0.1 and maximum 1.0.

I want to increase the distance between the leading edge of airfoil and the free stream boundary.

Quote:
Originally Posted by cnsidero View Post
Use the hyperbolic method for this mesh. To correct the behavior you're seeing you need to the modify the volume smoothing parameter in the Attributes tab under Smooth Parameters. Specifically, you should lower to a small value for the first portion of the extrusion and then increase later in the extrusion.

For example, if you wanted to extrude for 80 total steps I would set the volume smoothing to 0.05 for the first 20, increase it to 0.1 for the next 20, increase it to 0.3 for the next 20 and set it to the default 0.5 for the last 20.

That's just an example so you're likely going to have to adjust your values to get the desired result but it gives you a basic template to follow.

Let me know how it goes, Chris
Attached Images
File Type: jpg c mesh.jpg (35.3 KB, 63 views)
Fly is offline   Reply With Quote

Old   October 19, 2013, 11:23
Default
  #9
Senior Member
 
Chris Sideroff
Join Date: Mar 2009
Location: Ottawa, ON, CAN
Posts: 369
Rep Power: 12
cnsidero is on a distinguished road
Quote:
Originally Posted by Fly View Post
Hi Chris,

I tried your idea and it does work to improve the mesh. The attachment is my best result.

I have no idea about the meaning of volume smoothing parameter even after I read the explanation in the user manual book. Thus, I have to try to guess the value in this case. It is depressing that I cannot repeat my result after numerous attempts.

My general idea is to increase the "volume" value in every 5 steps, the minimum value is 0.1 and maximum 1.0.

I want to increase the distance between the leading edge of airfoil and the free stream boundary.
My general understanding is the volume smoothing parameter controls how quickly the transverse spacing become equal. You'll notice if you extrude a O-mesh that eventually the extrusion become a circle with uniform spacing around the circumference. By lowering the smoothing parameter, you let the extrusion maintain the original transverse spacing distribution further (hence why the extrusion keeps the airfoil shape when it's a small value).

So the idea is to keep the volume smoothing low early in the extrusion and thus maintaining the airfoil shape and then as it gets further away, allow the volume smoothing to increase so the shape gets more uniform - in the case of a C-topology more like a sideways U.

Honestly, the mesh you generate looks really good. I not sure how much better you need it to be. If it's a matter of how far away from the leading edge you want the boundary of mesh to be it typically should be 40-50 chord lengths upstream for minimizing the effect of boundary conditions on the something as sensitive as drag. Measure how far away your current boundary is from the leading edge and adjust it if necessary. There is a re-extrude command in Pointwise where you can modify an existing extrusion so you don't have to start the extrusion from scratch everytime.
Fly likes this.
cnsidero is offline   Reply With Quote

Old   October 19, 2013, 23:27
Default
  #10
Fly
New Member
 
Sun Yu
Join Date: Oct 2013
Location: Singapore
Posts: 7
Rep Power: 3
Fly is on a distinguished road
Thanks, Taxalian.

Yes, my growth rate is about 1.1. There is about 240 points on the airfoil and the first step size is 4.0e-4 (the chord length is 1).

I followed your instruction but I can not get the mesh as well as yours. Could you specify the parameters you fine-tuned?

Thank you.

Quote:
Originally Posted by taxalian View Post
If you want to use hyperbolic method, then simply follow Chris's instructions.
But in order to get also reasonably good c-mesh with algebraic extrusion you also need to increase the number of step and direction iterations in the attributes tab. Also start initially with smaller growth rate of about 1.1 to 1.05 and after some few iterations increase the growth rate. By doing this you will get a good nice mesh, of course in your case you need to fine tune the parameters to get the desired mesh.
Fly is offline   Reply With Quote

Old   October 19, 2013, 23:50
Default
  #11
Fly
New Member
 
Sun Yu
Join Date: Oct 2013
Location: Singapore
Posts: 7
Rep Power: 3
Fly is on a distinguished road
Thank you for your reply. It is straightforward and simple to understand.

I am sorry that I did not make it clear about the last sentence in the last message. I mean that I want the length from the leading edge and free stream boundary (noted as L1) to be the same as that from wake edge and upper boundary (noted as L2, both 20, just as the same as mesh I quote in my second message). In this way, I hope to minimize the effect of boundary layer just as you said.

In my practice, the L2 is about 20 but L1 only about 14. If I want to increase L1, L2 will increase dramatically. Thus, the mesh looks much like a semi-circle.


There is other parameters in smoothing parameters, like "Explicit", "Implicit".
Is it necessary to tune them for a better mesh?
Quote:
Originally Posted by cnsidero View Post
My general understanding is the volume smoothing parameter controls how quickly the transverse spacing become equal. You'll notice if you extrude a O-mesh that eventually the extrusion become a circle with uniform spacing around the circumference. By lowering the smoothing parameter, you let the extrusion maintain the original transverse spacing distribution further (hence why the extrusion keeps the airfoil shape when it's a small value).

So the idea is to keep the volume smoothing low early in the extrusion and thus maintaining the airfoil shape and then as it gets further away, allow the volume smoothing to increase so the shape gets more uniform - in the case of a C-topology more like a sideways U.

Honestly, the mesh you generate looks really good. I not sure how much better you need it to be. If it's a matter of how far away from the leading edge you want the boundary of mesh to be it typically should be 40-50 chord lengths upstream for minimizing the effect of boundary conditions on the something as sensitive as drag. Measure how far away your current boundary is from the leading edge and adjust it if necessary. There is a re-extrude command in Pointwise where you can modify an existing extrusion so you don't have to start the extrusion from scratch everytime.
Fly is offline   Reply With Quote

Old   October 20, 2013, 13:37
Default
  #12
Senior Member
 
Join Date: Nov 2010
Posts: 128
Rep Power: 6
taxalian is on a distinguished road
Quote:
Originally Posted by Fly View Post
Thanks, Taxalian.

Yes, my growth rate is about 1.1. There is about 240 points on the airfoil and the first step size is 4.0e-4 (the chord length is 1).

I followed your instruction but I can not get the mesh as well as yours. Could you specify the parameters you fine-tuned?

Thank you.
Hi Fly,

I think you need to initially start as follows:

under the relaxation parameters within the attributes tab you can do the following:

change direction option: 0.95 instead of default value of 0.5
change step size: 0.95 instead of default value of 0.7
direction and step size iterations: start with something like 150

the grid i showed previously consists of 200 grid points on the airfoil and 100 point on the wake connector. Make sure to have a uniform clustering in the trailing edge of the airfoil and start of the wake connector.
taxalian is offline   Reply With Quote

Old   December 3, 2013, 18:12
Default
  #13
New Member
 
Yosheph Yang
Join Date: Nov 2012
Location: Ankara, Turkey
Posts: 24
Rep Power: 4
andromeda91 is on a distinguished road
Quote:
Originally Posted by Fly View Post
Dear all,

I want to a c type mesh around airfoil NACA 0012. I am a new user of Pointwise and I think my application is something wrong. The followings are my steps:

1. import the airfoil geometry and set the dimensions of top and bottom edges of airfoil

2. create a 2-point curve which is the wake edge, the dimension is also set properly. The interval at the trailing edge is almost the same with that at the beginning of wake edge.


3. Create -->Extrude--> Normal
pick the domain in excessive order (wake edge-->bottom edge--> top edge--->wake edge)
set the initial step size and then run 80 steps

The following are my result. It can be seen that the mesh quality is not bad at the trailing edge. However, at the far field boundary, it is weird. Hope to get some advice from you guys. Thank you very much.
Hi Sun,

I am trying to do what you have done. How can I choose the edges like you do? I could only choose wake edge --> bottom edge --> top edge. I could not choose the wake edge once more.
andromeda91 is offline   Reply With Quote

Old   April 6, 2014, 07:19
Default
  #14
Member
 
Payam D.
Join Date: Aug 2011
Posts: 80
Blog Entries: 3
Rep Power: 5
pdp.aero is on a distinguished road
Here is what you should do when you are planning to create C-Type grid:
1- Create a connector from your trailing edge to the aft portion of your desired domain.
2- Distribute all the connectors with appropriate number of nodes.
3- Select all the connectors.
4- Create> extrude>normal
5- Assemble special> delete all the edges
6- Select outer space, upper surface, lower surface, and again outer space connectors respectively.
7- Save edge and done
8- Set splay boundary condition for the outer space connector with appropriate splay factor, as an example 0.01.
9- Set attribute condition. for example you may set ds= 0.0001, GR= 1.18, Max ds=0.75, Explicit=0.1, Implicit=15, KB=3.25(super critical airfoils), Volume=0.25, steps= 60. Do not forget to correct the extrusion orientation in case you need to change it.
10- RUN
pdp.aero is offline   Reply With Quote

Old   April 19, 2014, 00:16
Default
  #15
Fly
New Member
 
Sun Yu
Join Date: Oct 2013
Location: Singapore
Posts: 7
Rep Power: 3
Fly is on a distinguished road
Quote:
Originally Posted by andromeda91 View Post
Hi Sun,

I am trying to do what you have done. How can I choose the edges like you do? I could only choose wake edge --> bottom edge --> top edge. I could not choose the wake edge once more.
Hi andromeda,

Sorry for the late reply. Have you solved the problem now?
Fly 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
Problem with airfoil shape optimization robyTKD SU2 Shape Design 6 June 13, 2013 19:13
2D Mesh Generation Tutorial for GMSH aeroslacker Open Source Meshers: Gmsh, Netgen, CGNS, ... 12 January 19, 2012 04:52
Icemcfd 11: Loss of mesh from surface mesh option? Joe CFX 2 March 26, 2007 18:10
Problem when trying to generate a new mesh gaottino OpenFOAM Meshing & Mesh Conversion 0 June 30, 2006 07:51
How to control Minximum mesh space? hung FLUENT 7 April 18, 2005 09:38


All times are GMT -4. The time now is 15:14.