[ICEM] Export mesh statistics for use in Richardson Extrapolation for grid sensitivity study

JuPa · April 16, 2013, 07:33

Hi,

Following the post from another user in this thread (http://www.cfd-online.com/Forums/cfx...-analysis.html) I want to do a grid sensitivity study using the Richardson extrapolation method.

The first step is to define a representative cell, mesh or grid size,

. For three-dimensional simulations

$h=\left[ \frac{1}{N}\sum^{N}_{i=1}{ \Delta V_{i}} \right]^{ \frac{1}{3}}$

where $\Delta V_{i}$ is the volume of the $i^{th}$ cell,

is the total number of cells used for the computations.

My problem is I don't know how to extract the values of $\Delta V_{i}$ from ICEM as ideally I'd like to do the Richardson Extrapolation method in Excel, where I can compare different meshes. In ICEM how do I export mesh statistics such as volume of each cell? Can it be exported as a handy .csv file?

I refer you to the paper I am using: http://journaltool.asme.org/Template...umAccuracy.pdf

Thank you

RodriguezFatz · April 16, 2013, 07:48

Since you just need the ratio of h(fine)/h(coarse) calculation of an actual value of "h" is not necessary.
How do you want to do the refinement in ICEM?

JuPa · April 16, 2013, 08:01

Quote:

Originally Posted by RodriguezFatz

Since you just need the ratio of h(fine)/h(coarse) calculation of an actual value of "h" is not necessary.
How do you want to do the refinement in ICEM?

My variable of interest is wall heat transfer coefficient at the various boundaries. I am using the SST turbulence model. For accurate heat transfer predictions I need a Y+ < 1. So far the maximum Y+ I have on any of my boundaries is 1.6.

I will do the refinement in ICEM by applying more nodes in the thermal boundary layer.

RodriguezFatz · April 16, 2013, 08:03

Do you use blocking / hexa meshing or unstructured?

JuPa · April 16, 2013, 08:11

Quote:

Originally Posted by RodriguezFatz

Do you use blocking / hexa meshing or unstructured?

I use blocking (hexa mesh). Before I export the mesh in .cfx5 format I right click on "Pre-Mesh" and click on "Convert to Unstructured Mesh".

RodriguezFatz · April 16, 2013, 08:13

Great. Then you have all the numbers...
Do you refine the whole grid by using the mesh->refine utility, or do you change the number of nodes of some relevant edges?

Is this 2d? Can you post some picture?

JuPa · April 16, 2013, 08:24

Quote:

Originally Posted by RodriguezFatz

Great. Then you have all the numbers...
Do you refine the whole grid by using the mesh->refine utility, or do you change the number of nodes of some relevant edges?

Is this 2d? Can you post some picture?

It is 2D axisymmetric. I change the number of nodes of relevant edges. The geometry is shown below:

Do you want a picture of the mesh?

RodriguezFatz · April 16, 2013, 08:31

How large is your coarsest mesh?
In 2d (and such a simple geometry) it is often affordable to just refine the whole mesh, which means you will end up with a 4 times larger mesh (2 x in "x" and 2 x in "y" direction). Would that be ok for you?

JuPa · April 16, 2013, 08:48

Quote:

Originally Posted by RodriguezFatz

How large is your coarsest mesh?
In 2d (and such a simple geometry) it is often affordable to just refine the whole mesh, which means you will end up with a 4 times larger mesh (2 x in "x" and 2 x in "y" direction). Would that be ok for you?

The coarsest mesh has 6500 elements and 3072 nodes. I do have the computational resources to double, triple and quadruple the number of elements and nodes.

However what I am interested in is the Richardson extrapolation method I mentioned in my original post.

RodriguezFatz · April 16, 2013, 09:05

It's always the same method:
In your case, save your coarse mesh. Then refine the (unstructured) mesh, by clicking on "Edit Mesh -> Adjust Mesh Density". Here you can use "Refine All Mesh", method "pure refinement", steps "1". ->apply.
You will get a mesh, that is 2 times finer in each dimension.
Save that mesh. Do the same refinement again and you will end up with a even finer mesh.

Now run your simulation on all three meshes. Use the coarse results as interpolation for initializing the other runs.
For each simulation you need one single "important" value, such as you heat transfer coefficient or whatever. Using the nomenclature of your pdf, these values are the phi 3, 2 an 1. Since you doubled the number of points in each dimension the value of r21 and r32 is "2".
Here we go!

JuPa · April 16, 2013, 09:45

Thank you! That actually does help.

RodriguezFatz · April 16, 2013, 10:34

If you did that, you could post the values here for others to see how it works...

lentschi · January 18, 2014, 19:57

Hello,

I have one additional question regarding the Richardson Interpolation: What is about r21 and r32 if only the total number of cells is doubled (by splitting one direction)?

Example:

Coarse: 3 Million cells
Reference: 6 Million cells
Fine: 12 Million cells

I then r21=r32=1.25??

Thanks in advance.

//Markus

Suman Sapkota · July 5, 2018, 09:35

Hello,
I found this post relevant. I got a result of 1.7th order accuracy when i did the grid independent study with Richardson's method. I simulated a pump with refinement about 1.5 and high resolution scheme was used which is 1st to 2nd order accurate. It would be nice to know if it is possible to get 2nd order accurate solution from the grid refinement, especially when the flow may not align with the grid lines, i.e highly turbulent + three-dimensional. Also, if someone has seen similar behavior of the order of accuracy, please tell me.

April 16, 2013, 07:33	Export mesh statistics for use in Richardson Extrapolation for grid sensitivity study	#1
JuPa Senior Member Mr CFD Join Date: Jun 2012 Location: Britain Posts: 361 Rep Power: 15	Hi, Following the post from another user in this thread (http://www.cfd-online.com/Forums/cfx...-analysis.html) I want to do a grid sensitivity study using the Richardson extrapolation method. The first step is to define a representative cell, mesh or grid size, . For three-dimensional simulations $h=\left[ \frac{1}{N}\sum^{N}_{i=1}{ \Delta V_{i}} \right]^{ \frac{1}{3}}$ where $\Delta V_{i}$ is the volume of the $i^{th}$ cell, is the total number of cells used for the computations. My problem is I don't know how to extract the values of $\Delta V_{i}$ from ICEM as ideally I'd like to do the Richardson Extrapolation method in Excel, where I can compare different meshes. In ICEM how do I export mesh statistics such as volume of each cell? Can it be exported as a handy .csv file? I refer you to the paper I am using: http://journaltool.asme.org/Template...umAccuracy.pdf Thank you

April 16, 2013, 07:48		#2
RodriguezFatz Senior Member Philipp Join Date: Jun 2011 Location: Germany Posts: 1,297 Rep Power: 27	Since you just need the ratio of h(fine)/h(coarse) calculation of an actual value of "h" is not necessary. How do you want to do the refinement in ICEM? __________________ The skeleton ran out of shampoo in the shower.

April 16, 2013, 08:03		#4
RodriguezFatz Senior Member Philipp Join Date: Jun 2011 Location: Germany Posts: 1,297 Rep Power: 27	Do you use blocking / hexa meshing or unstructured? __________________ The skeleton ran out of shampoo in the shower.

April 16, 2013, 08:13		#6
RodriguezFatz Senior Member Philipp Join Date: Jun 2011 Location: Germany Posts: 1,297 Rep Power: 27	Great. Then you have all the numbers... Do you refine the whole grid by using the mesh->refine utility, or do you change the number of nodes of some relevant edges? Is this 2d? Can you post some picture? __________________ The skeleton ran out of shampoo in the shower.

April 16, 2013, 08:31		#8
RodriguezFatz Senior Member Philipp Join Date: Jun 2011 Location: Germany Posts: 1,297 Rep Power: 27	How large is your coarsest mesh? In 2d (and such a simple geometry) it is often affordable to just refine the whole mesh, which means you will end up with a 4 times larger mesh (2 x in "x" and 2 x in "y" direction). Would that be ok for you? __________________ The skeleton ran out of shampoo in the shower.

April 16, 2013, 09:05		#10
RodriguezFatz Senior Member Philipp Join Date: Jun 2011 Location: Germany Posts: 1,297 Rep Power: 27	It's always the same method: In your case, save your coarse mesh. Then refine the (unstructured) mesh, by clicking on "Edit Mesh -> Adjust Mesh Density". Here you can use "Refine All Mesh", method "pure refinement", steps "1". ->apply. You will get a mesh, that is 2 times finer in each dimension. Save that mesh. Do the same refinement again and you will end up with a even finer mesh. Now run your simulation on all three meshes. Use the coarse results as interpolation for initializing the other runs. For each simulation you need one single "important" value, such as you heat transfer coefficient or whatever. Using the nomenclature of your pdf, these values are the phi 3, 2 an 1. Since you doubled the number of points in each dimension the value of r21 and r32 is "2". Here we go! JuPa likes this. __________________ The skeleton ran out of shampoo in the shower.

April 16, 2013, 09:45		#11
JuPa Senior Member Mr CFD Join Date: Jun 2012 Location: Britain Posts: 361 Rep Power: 15	Thank you! That actually does help.

April 16, 2013, 10:34		#12
RodriguezFatz Senior Member Philipp Join Date: Jun 2011 Location: Germany Posts: 1,297 Rep Power: 27	If you did that, you could post the values here for others to see how it works... __________________ The skeleton ran out of shampoo in the shower.

January 18, 2014, 19:57		#13
lentschi Member sirLentschi Join Date: Nov 2010 Posts: 87 Rep Power: 16	Hello, I have one additional question regarding the Richardson Interpolation: What is about r21 and r32 if only the total number of cells is doubled (by splitting one direction)? Example: Coarse: 3 Million cells Reference: 6 Million cells Fine: 12 Million cells I then r21=r32=1.25?? Thanks in advance. //Markus

July 5, 2018, 09:35	cfx particle tracking	#14
Suman Sapkota Member Suman Sapkota Join Date: Feb 2018 Posts: 32 Rep Power: 8	Hello, I found this post relevant. I got a result of 1.7th order accuracy when i did the grid independent study with Richardson's method. I simulated a pump with refinement about 1.5 and high resolution scheme was used which is 1st to 2nd order accurate. It would be nice to know if it is possible to get 2nd order accurate solution from the grid refinement, especially when the flow may not align with the grid lines, i.e highly turbulent + three-dimensional. Also, if someone has seen similar behavior of the order of accuracy, please tell me.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Gambit problems	Althea	FLUENT	22	January 4, 2017 04:19
2D mesh export of an original 3D model	Yogendra Shastri	Main CFD Forum	0	February 22, 2008 14:14
fluent add additional zones for the mesh file	SSL	FLUENT	2	January 26, 2008 12:55
Icemcfd 11: Loss of mesh from surface mesh option?	Joe	CFX	2	March 26, 2007 19:10
How to control Minximum mesh space?	hung	FLUENT	7	April 18, 2005 10:38