[wildan]

Hello everyone,

Right now I'm working on a steam ejector project. I was asked to create the fluid flow simulation. And currently I'm stucked with the Inflation problem. I know I can't ignore the inflation since it's the fluid flow analysis.

From pic 1-3 (attached on Geometry 1-3.zip), you can see my whole geometry. When I use global mesh only (without inflation), the skewness and orthogonal quality seem good (max 0.79 and min 0.24, respectively) - see pic 4-5 in Skewness & Orthogonal Quality 4-8.zip. But when I insert the inflation, the max skewness: 0.91 and min orthogonal quality: 0.013!! It's decreasing drastically! (see pic 6-7 in Skewness & Orthogonal Quality 4-8.zip).

I've tried to change the inflation options (i.e. smooth transition, total thickness, first layer thickness, changing the layer height, growth rate, etc). Also I've modified the mesh sizing options (global mesh) - i.e. advanced size function, relevance center, smoothing, min-max size, growth rate, etc.

But all of it doesn't improve the mesh quality significantly. FYI, I've tried the sweep, multizone, tetrahedrons, hex dominant, you name it. But still it doesn't solve my problem. I really need your help to solve it.

Thank you very much. I really appreciate your help.

Cheers.

Geometry 1-3.zip

Skewness & Orthogonal Quality 4-8.zip

[vasava]

Can you also upload the workbench files somewhere and post the link? It will be easier to spot the problem rather than making mesh from scratch.

[wildan]

Originally Posted by vasava

Can you also upload the workbench files somewhere and post the link? It will be easier to spot the problem rather than making mesh from scratch.

Thank you for your reply, sir.

I have uploaded the .meshdat files here:

https://www.dropbox.com/s/38e5cwy6ne...h.meshdat?dl=0

From my latest trial (link above), the orthogonal quality is improved a bit (min orthogonal 0.042). I know it's still far from the ideal value.

FYI, I am using ANSYS 16.2. Hopefully you have the same or newer version so that you'll be able to open it.

Thank you very much for your help, sir.

Regards

[vasava]

Not the .meshdat files but the .wbpj file and corresponding folder.

Check the folder where you have saved your workbench setup. There should be yourProject.wbpj file and a folder yourProject_files (Here yourProject= the name with which you saved your workbench files).

[wildan]

Originally Posted by vasava

Not the .meshdat files but the .wbpj file and corresponding folder.

Check the folder where you have saved your workbench setup. There should be yourProject.wbpj file and a folder yourProject_files (Here yourProject= the name with which you saved your workbench files).

Copy that, sir. Here it is:

https://www.dropbox.com/s/ckfji9haln...oject.rar?dl=0

[vasava]

I did not find any special setup in your workbench files except the inflation (that too had only one layer!!). You will need more setup if you want a better mesh.
I tried a quick setup and everything, including inflation, worked quite nicely for me.
I suggest that you try the following:

1. Change sizing function to uniform or fixed (they are same). With uniform sizing you can avoid unnecessary extra fine meshes where they are not needed. In stead you can introduce sizing and make finer mesh where it is needed.
2. The region where the pipes bifurcate has small gaps. You can use appropriate sizing for these walls to get finer mesh so that there are enough elements for calculations.
   Having a smaller sizing will help accommodate the boundary layers from both the walls.
3. You had only one layer for inflation. Make sure you add more layers otherwise there is no point in having inflation.
4. You can also improve mesh quality in Fluent by TUI commands. It doesn't help all the time but mostly it does.

While trying, I also got bad meshes for inflation in that region, giving a smaller face size helped me get a better mesh. And with fluent TUI commands I could get the mesh quality to acceptable value 0.1.

[wildan]

Originally Posted by vasava

I did not find any special setup in your workbench files except the inflation (that too had only one layer!!). You will need more setup if you want a better mesh.
I tried a quick setup and everything, including inflation, worked quite nicely for me.
I suggest that you try the following:

1. Change sizing function to uniform or fixed (they are same). With uniform sizing you can avoid unnecessary extra fine meshes where they are not needed. In stead you can introduce sizing and make finer mesh where it is needed.
2. The region where the pipes bifurcate has small gaps. You can use appropriate sizing for these walls to get finer mesh so that there are enough elements for calculations.
   Having a smaller sizing will help accommodate the boundary layers from both the walls.
3. You had only one layer for inflation. Make sure you add more layers otherwise there is no point in having inflation.
4. You can also improve mesh quality in Fluent by TUI commands. It doesn't help all the time but mostly it does.

While trying, I also got bad meshes for inflation in that region, giving a smaller face size helped me get a better mesh. And with fluent TUI commands I could get the mesh quality to acceptable value 0.1.

Thank you very much for your advice, sir.

However, after doing multiple setups, I got worse orthogonal quality (best result I've got is 0.18, and it's not improving with fluent TUI commands). I've attached 'em below.

Could you by any chance attach your setup including min-max sizing and inflation setup? I would really appreciate your help.

Again, thank you very much.

[wildan]

UPDATE: Finally I got the same value as yours in FLUENT. I hope this is gonna work. Thank you very much, Mr. Vasava!

[vasava]

I am logged in to ubuntu right now and dont have access to Ansys. But I am glad that your mesh settings are working out.

[dottorbiker]

hi everyone!
I've exactly the same problem: the mesh quality drastically decrease when I insert the inflation layers.
Any suggestion? My solver is CXF. I've used as size function proximity and curvature.
below the photos of the geometry and of the quality. I'm working on a quarter of the full geometry thanks to the symmetry.
here the proj file (v 17): https://1drv.ms/f/s!AlY0liGuZwHig8gzMBTNug38m3oE2w

Thanks
Michele

[vasava]

Michele, I have no experience with CFX (and no access as well) and I do not know if CFX has TUI commands to improve mesh qualities just like fluent. You can try suggestions I gave to Wildan and see if they workout for you.

I will have a look at your case with fluent when I have time.

[dottorbiker]

Originally Posted by vasava

Michele, I have no experience with CFX (and no access as well) and I do not know if CFX has TUI commands to improve mesh qualities just like fluent. You can try suggestions I gave to Wildan and see if they workout for you.

I will have a look at your case with fluent when I have time.

thanks Vasava for you reply and your time.
sure,I've tried to follow the suggestions that you have gave to Wildan but I haven't obtained good results.
I have no idea how to use (if they are in CFX) the TUI commands.
Michele

[vasava]

Michele, I am unable to download your case files. I tried thrice and it stopped downloading midway. Either your case files are way too big or it my office internet. Anyways, Can you upload it somewhere else? Also compress the files.

[dottorbiker]

Originally Posted by vasava

Michele, I am unable to download your case files. I tried thrice and it stopped downloading midway. Either your case files are way too big or it my office internet. Anyways, Can you upload it somewhere else? Also compress the files.

Sorry for the waste of time!
Now I have put in the same folder also the meshdat file called "mesh", compressed and not.
Thanks
Michele

[vasava]

Firstly, I checked the mesh quality for your mesh with fluent and it passed all the checks. Of course the mesh quality was low (0.013) but with TUI commands I could get it to 0.103674. So your mesh (after TUI manipulations) should be good enough for calculations.

Next, I tried a quick setup with my own recommendations and again I could get a mesh (after TUI manipulations) which was alright for calculations.

Here is what I did:

1. Switched to uniform sizing method from proximity&Curvature. This gave better control over mesh sizing.
2. Introduced sizing on cover, frame and fan walls. With sizing coupled with uniform sizing method, I decide where mesh is fine and not Ansys. When I introduced sizing, there were no more bad elements close to fan walls. The mesh quality in that region was about 0.13. I guess this is what you were looking for.
3. Reduced number of inflation layers to 10. I think 10 is enough. Even 8 would do.

Again, I dont have CFX so I dont know if there are ways to improve mesh quality in CFX. I dont even know how to check mesh quality in CFX. So, lets wait for someone who is expert on CFX to give you a better opinion on this one.

[dottorbiker]

Originally Posted by vasava

Firstly, I checked the mesh quality for your mesh with fluent and it passed all the checks. Of course the mesh quality was low (0.013) but with TUI commands I could get it to 0.103674. So your mesh (after TUI manipulations) should be good enough for calculations.

Next, I tried a quick setup with my own recommendations and again I could get a mesh (after TUI manipulations) which was alright for calculations.

Here is what I did:

1. Switched to uniform sizing method from proximity&Curvature. This gave better control over mesh sizing.
2. Introduced sizing on cover, frame and fan walls. With sizing coupled with uniform sizing method, I decide where mesh is fine and not Ansys. When I introduced sizing, there were no more bad elements close to fan walls. The mesh quality in that region was about 0.13. I guess this is what you were looking for.
3. Reduced number of inflation layers to 10. I think 10 is enough. Even 8 would do.

Again, I dont have CFX so I dont know if there are ways to improve mesh quality in CFX. I dont even know how to check mesh quality in CFX. So, lets wait for someone who is expert on CFX to give you a better opinion on this one.

dear vasava, really thank you for your time and your experience.
Unfortunately I'have never used Fluent and TUI to mesh, but, because you have obtained what I want, I'm trying to understand how to use it.
If it is possible, could you send me some screenshot of the parameters that you have set in fluent to understand more fast where the commands are?
Thank you
Michele

[vasava]

Fluent TUI commands are pretty simple to use. You may first want to read what exactly they do.

For example if you want to improve mesh quality you can follow these steps:

1. Type mesh and press enter. You can press enter again to see options available under mesh .
2. Type repair-improve and press enter. You can press enter again to see available options.
3. You can enable options like allow-repair-at-boundaries, include-local-polyhedra-conversion-in-repair, repair-face-handedness, repair-face-node-order and repair-wall-distance.
   Write the option, press enter, write answer 'Yes' or 'No' and press enter.
   This will activate the option.
   
4. Once you have selected all the desired options you can start repairing mesh by entering repair or improve mesh quality by entering
   improve-quality.
   
   Executing Repairing command once or twice is enough. But the command for improving quality needs to be run several times.
   
   Check mesh quality and repeat these commands until the mesh quality reaches to satisfactory level.

Now these commands may or may not work for all the mesh. I mean these commands are handy but it is not like they can fix any and every bad mesh. I believe they are good if the mesh has only minor issues (e.g. very low % of elements are bad elements).

Also after executing the commands if you dont see any improvement in the mesh then you will have to go back to ansys meshing, change mesh and try something else.

[dottorbiker]

Originally Posted by vasava

Fluent TUI commands are pretty simple to use. You may first want to read what exactly they do.

For example if you want to improve mesh quality you can follow these steps:

1. Type mesh and press enter. You can press enter again to see options available under mesh .
2. Type repair-improve and press enter. You can press enter again to see available options.
3. You can enable options like allow-repair-at-boundaries, include-local-polyhedra-conversion-in-repair, repair-face-handedness, repair-face-node-order and repair-wall-distance.
   Write the option, press enter, write answer 'Yes' or 'No' and press enter.
   This will activate the option.
   
4. Once you have selected all the desired options you can start repairing mesh by entering repair or improve mesh quality by entering
   improve-quality.
   
   Executing Repairing command once or twice is enough. But the command for improving quality needs to be run several times.
   
   Check mesh quality and repeat these commands until the mesh quality reaches to satisfactory level.

Now these commands may or may not work for all the mesh. I mean these commands are handy but it is not like they can fix any and every bad mesh. I believe they are good if the mesh has only minor issues (e.g. very low % of elements are bad elements).

Also after executing the commands if you dont see any improvement in the mesh then you will have to go back to ansys meshing, change mesh and try something else.

thank you, I'll follow your instructions carefully!

[Alamu]

The mesh quality can be improved by
1. Partitioning the domain using simple shapes as square, triangles and use face meshing by matching equal no.of. divisions.
2. Give small sizing for edge sizing, face sizing and body sizing. The skewness and aspect ratio comes down. Max skewness 0.91 is not bad.

[ddungntu]

Originally Posted by Alamu

The mesh quality can be improved by
1. Partitioning the domain using simple shapes as square, triangles and use face meshing by matching equal no.of. divisions.
2. Give small sizing for edge sizing, face sizing and body sizing. The skewness and aspect ratio comes down. Max skewness 0.91 is not bad.

Dear Sir,

Is it possible to split domain at free surface?

I am trying to simulate the water entry problems using Ansys CFX (2-way FSI). As I know the mesh quality of free surface is important to capture properly water interface during impact. So I have tried to divide the fluid domain to two blocks to mesh independently, but it does not work (i.e. CFX could not find the interface).

Could you please help me to make a good mesh at the expected region (free surface), without split fluid domain?

Thank you in advance!