[zeng1017]

Dear all,
Happy new year. I have tried to do inflation around a cube for two weeks, but still have problem. I would like to generate mesh like the Picture 1. However, what i got from ANSYS meshing is like Picture 2, which is a trapezoid, rather than a square. I have turned off collision avoidance.

I also tried to do it like Picture 3. I cut my domain into several parts in Design modeler, and do inflation for the edges of each part. However around the corner, I got Picture 4. The two interacted inflation couldn't cross each other.

The inflation group of Global mesh controls is shown as picture 5.

Ansys is new to me. If you have any idea, please let me know. Any help appreciated.

[zeng1017]

Picture 6 is my local inflation control. Hope I have made my question clear.

[Antanas]

To get what's on image 1 try to split your geometry and use sweep/multizone with mapped face meshing (see attachment). To get what's on image 3 you should use inflation, but edge sizings (hard) with biasing.

[jjfm20]

Hello, I do recommend you to use local edge sizing, you can set there a bias and control in a better way the meshing. .. This work for multizone method, setting the sizing as "hard".

Regards

Sent from my LG-K430 using CFD Online Forum mobile app

[zeng1017]

Originally Posted by Antanas

To get what's on image 1 try to split your geometry and use sweep/multizone with mapped face meshing (see attachment). To get what's on image 3 you should use inflation, but edge sizings (hard) with biasing.

Thanks a lot for your sketch, Antanas. I will try it out tomorrow. To be honest, I don't know how to use sweep and multizone. I am gonna to learn from the users guide.

[zeng1017]

Originally Posted by jjfm20

Hello, I do recommend you to use local edge sizing, you can set there a bias and control in a better way the meshing. .. This work for multizone method, setting the sizing as "hard".

Regards

Sent from my LG-K430 using CFD Online Forum mobile app

Thanks a lot for your suggestion. It seems multizone is better than cutting the domain into pieces in the Design Modeler. I don't know how to use multizone, but I will learn that tomorrow. Thanks again.

[zeng1017]

Originally Posted by Antanas

To get what's on image 1 try to split your geometry and use sweep/multizone with mapped face meshing (see attachment). To get what's on image 3 you should use inflation, but edge sizings (hard) with biasing.

Originally Posted by jjfm20

Hello, I do recommend you to use local edge sizing, you can set there a bias and control in a better way the meshing. .. This work for multizone method, setting the sizing as "hard".

Regards

Sent from my LG-K430 using CFD Online Forum mobile app

Hi Antanas and jjfm20,
I have finally generated the mesh I want. However, the Fluent calculation diverged when using this mesh (please see picture 7). Then I generated mesh again by only using "inflation" and "face sizing"(please see picture 8). This time it worked well. I found the maximum corner angle is 137.76 ° for picture 7. Is it the reason?

Thanks in advanced.

[siw]

You have a significant element size change between the last inflation layer element and the first quad element. If you are modelling the flow over the cube then this region would be have some flowfield features, unlike in the farfield, so make more inflation layers to have a smoother size transition. Would finer mesh resolution in the wake of the cube improve your solution convergence? You have not given any information about the simulation this mesh is for.

This is all covered in the ANSYS Meshing training material (see the Lecture 5 presentation) which, as an ANSYS customer, you can download from their customer portal.

[zeng1017]

Originally Posted by siw

You have a significant element size change between the last inflation layer element and the first quad element. If you are modelling the flow over the cube then this region would be have some flowfield features, unlike in the farfield, so make more inflation layers to have a smoother size transition. Would finer mesh resolution in the wake of the cube improve your solution convergence? You have not given any information about the simulation this mesh is for.

This is all covered in the ANSYS Meshing training material (see the Lecture 5 presentation) which, as an ANSYS customer, you can download from their customer portal.

Hi Stuart,
Thanks a lot for your reply. I am modeling the flow over cubes(please see picture 9). I am using periodic boundary conditions. The inlet and outlet are cyclic. I know it is not good to have a significant element size change between the last inflation layer element and the first quad element. However, In order to get rid of the element size jump, the inflation may need to be increased to 42 layers. Would that be too many layers?

[siw]

I have done similar simulations myself . You cannot have too many inflation layers, just keep layering them to transition smoothly into the farfield mesh and since those are quad elements then you should not really see where the inflation layer ends. Also their aspect ratio will reduce away from the wall to be more suited to the separated flow around those cubes.

See Slide 97 of the ANSYS Meshing presentation here https://www.ozeninc.com/wp-content/u...KSHOP_2014.pdf.

[zeng1017]

Originally Posted by siw

I have done similar simulations myself . You cannot have too many inflation layers, just keep layering them to transition smoothly into the farfield mesh and since those are quad elements then you should not really see where the inflation layer ends. Also their aspect ratio will reduce away from the wall to be more suited to the separated flow around those cubes.

See Slide 97 of the ANSYS Meshing presentation here https://www.ozeninc.com/wp-content/u...KSHOP_2014.pdf.

Thanks a lot for your information. It is very useful. I will spend a day trying to understand and then modify my mesh. By the way, which kind of mesh may give better result? I find the following two mesh are commonly used.

[siw]

As always there are pros and cons with both, and different CFDers may give different answers.

I would say the first picture avoids the propagation of the very high aspect ratio cells at the cube walls extending into the flowfield which is not suitable for the turbulent wake regions (hence LES in that area should have cells with unity aspect ratio). However, in the first picture the cells angles deviate from 90deg due to the corners. Which gives the lowest total cell quantity? I would go with the first picture.

But the best way to find out is to run a solution on each mesh and compare the results.

[zeng1017]

Originally Posted by siw

As always there are pros and cons with both, and different CFDers may give different answers.

I would say the first picture avoids the propagation of the very high aspect ratio cells at the cube walls extending into the flowfield which is not suitable for the turbulent wake regions (hence LES in that area should have cells with unity aspect ratio). However, in the first picture the cells angles deviate from 90deg due to the corners. Which gives the lowest total cell quantity? I would go with the first picture.

But the best way to find out is to run a solution on each mesh and compare the results.

You perfectly answered my question. I appreciate your help. I would spend a day to understand the suggestions in the post and then generate a mesh. Have a good evening. Thanks again.

[hemmt]

Originally Posted by zeng1017

You perfectly answered my question. I appreciate your help. I would spend a day to understand the suggestions in the post and then generate a mesh. Have a good evening. Thanks again.

hello zeng.

I m also working on similar type of simulation.
so please guide me generate this type of mesh.

[zeng1017]

Originally Posted by hemmt

hello zeng.

I m also working on similar type of simulation.
so please guide me generate this type of mesh.

Hi Hemant,
I hope I can help. The following pictures are what I got in this few days.
"mapped face meshing" has been removed from V171, so I just used multizone and inflation.
I am still looking a way to generate mesh like picture 1.
If anybody has any idea, please let us know.

[siw]

The only way to get the mesh shown in Picture 1 using ANSYS Meshing is to decompose the geometry into 4-sided (if this is 2D) blocks. Unlike ICEM in which you can make the blocking topology at the mesh level, ANSYS Meshing requires this to be done at the geometry level, so for instance smoothing of the mesh across geometry blocks is not possible.

Use DesignModeler or similar to slice your domain into blocks and then you can use edge sizings (with bias if you like).

I have attached a quick test of what I think you want using DesignModeler and Meshing inside Workbench using v17.2. Unzip and then un-archive in Workbench. I have used a MultiBody Part and notice there is no smoothing.

[zeng1017]

Originally Posted by siw

The only way to get the mesh shown in Picture 1 using ANSYS Meshing is to decompose the geometry into 4-sided (if this is 2D) blocks. Unlike ICEM in which you can make the blocking topology at the mesh level, ANSYS Meshing requires this to be done at the geometry level, so for instance smoothing of the mesh across geometry blocks is not possible.

Use DesignModeler or similar to slice your domain into blocks and then you can use edge sizings (with bias if you like).

I have attached a quick test of what I think you want using DesignModeler and Meshing inside Workbench using v17.2. Unzip and then un-archive in Workbench. I have used a MultiBody Part and notice there is no smoothing.

Hi Stuart，
Nice to hear from you again. I drew a sketch for better understanding your idea. Is it what you mean?

[siw]

Basically, yes. Take a look at the file I uploaded.

[hemmt]

Originally Posted by zeng1017

Hi Hemant,
I hope I can help. The following pictures are what I got in this few days.
"mapped face meshing" has been removed from V171, so I just used multizone and inflation.
I am still looking a way to generate mesh like picture 1.
If anybody has any idea, please let us know.

thanks Zeng,
for your inputs
now let me try it again.

[Antanas]

Originally Posted by zeng1017

"mapped face meshing" has been removed from V171

Wrong. It's still there.