Volume mesh with layers

AndyZ · March 10, 2013, 18:18

Hello,
I'm new at using ANSA for CFD meshing. I'm getting a good quality surface mesh for a car model and the road and tunnel walls, but then I'm having some difficulties with the volume mesh.

In the ANSA tutorial for external aero, they are using a structured layers mesh only for the road. Since I'm interested in capturing the air speed gradient at the surface of the car, I assume these layers are also supposed to be generated from the car surface. The problem is that afterwards the VOLUME>DEFINE function doesn't recognize the rest of the tunnel volume (without the car and the newly created layers), why is that? There is an autodetected volume, but when I select it nothing gets highlighted.

Also, once I do the layers operation, the side walls are reported as unmeshed, although I can still see the mesh grid on them.. Is it a problem if they remain like this?

vangelis · March 11, 2013, 03:18

Hi Andy,

Which ANSA version are you using?

In the external aero tutorial layers are grown from both car wind tunnel road.

Now coming to your exact problem.

When ANSA grows layers it connect to the side mesh of the windtunnel.
To do that it uses ELEMENTs>RELEASE on the four sides where it connects.
By RELEASE the elements are de-associated from the geometry and ANSA
is free to reconstruct the mesh, create the quad imprint of the layers and connected the layers. As the mesh is RELEASED, these Macros become
unmeshed. In order to avoid accidental remeshing (and hence duplicate mesh)
These Macros become also Frozen. Play around with the visibility flag buttons for FE-mod and Macros and you will see what I mean.

Finally about the problem of Volume detection.

Do you have any layer collapsed areas?
Open the property list and use Show Only to see if ANSA has collapsed
some areas from layers.

To perform the DETECT process follow these steps.

Check in the VOLUMEs>LIST what volumes you have.
You should only have one volume for layers in fact.
You can use Show Only on a volume to inspect it.
Delete any unecessary volume.

Press ALL
Ensure Macros and FE-mod mesh flags are active!
In the SETs button if there is a SET called
Do Not include in Detect
Select it and make it Hide.

Now press DETECT.

Does it work?

Best regards

Vangelis

AndyZ · March 11, 2013, 05:12

Hello,
Thank you for your reply

I am using v.13.2.2

You are right about the layers, I read the tutorial more carefully and now I have the whole volume meshed. One question though : I also had a set with collapsed areas, I put that in hide along with the "do not include....." set, is that ok or should I keep the collapsed set visible?

Thanks again,
Andy

vangelis · March 11, 2013, 05:36

Hi Andy,

The collapsed areas are marked with duplicate FE-mod shell elements
on top of the original surface mesh of the Macros, on the areas of the problems.
Just before DETECT, these shells must be visible,

The SET "Do not include in Detect" contains the original surface mesh of the
macros from which the layers were grown.
As Now you have the TOP_CAP_Fluid_Layers and the Collapsed Areas FE-mod
shells, these original Macros are set to Hide, so that DETECT can work
without finding duplicate shells.

It is a bit complicated but I hope it is clear

cheers

Vangelis

AndyZ · March 11, 2013, 11:46

Hey,

Thanks for your help, it's clearer to me know. I'll try to run my FLUENT analysis tonight with this ANSA mesh, hopefully it's good enough.

Volume info is this:
According to FLUENT Skewness
Average TETRA Quality : 0.259 WORST : 0.9922488
0.00 - 0.10: 350161 15.454 %
0.10 - 0.20: 505417 22.306 %
0.20 - 0.30: 572581 25.270 %
0.30 - 0.40: 446563 19.709 %
0.40 - 0.50: 235915 10.412 %
0.50 - 0.60: 115061 5.078 %
0.60 - 0.70: 34922 1.541 %
0.70 - 0.80: 4223 0.186 %
0.80 - 0.90: 946 0.042 %
Worst than 0.90: 44 0.002 %

This is after FIX QUALITY command. Any chance it can be improved?

And one more thing, I don't know of your experiece with FLUENT, but.. I have imported my mesh into FLUENT (new "Mesh" element in the project, import my mesh there, then drag it over the Mesh in the FLUENT case). In the FLUENT setup, I see that my surfaces "road" and "car" are not found in the Boundary Conditions, I can't specify which boundary to use for drag/lift/moment calculation... What am I missing?

Thanks,
Andy

vangelis · March 12, 2013, 02:04

Hi Andy,

If you do not see all the zones in Fluent it may be that not the whole
model was visible when you output from ANSA.

Go back to ANSA.
Press ALL
Ensure that FE-mod, Macros and Volumes flag are all active.

(I assume that you start ANSA in CFD setup so all quality criteria
are predefined for CFD)
Press VOLUMEs>IMPROVE>FIX QUAL Visible

Check the Volume Stats again, they should be better now.

Finally use Fluent output with everything visible.

Hope this helps

Best regards

Vangelis

AndyZ · March 13, 2013, 00:06

Hello,

It works, thanks!

vangelis · March 13, 2013, 02:18

You are welcome!

cfdivan · August 15, 2013, 08:37

Hi all,

I am facing the same problem and I already tried yours sugestion but when I do DETECT i only have fluid_layers. It looks like there is no volume of fluid. Do you have any clue how can I fix this?

Thanks!

vangelis · August 19, 2013, 03:34

Hi cfdivan,

What message do you get in the text window when you press DETECT?
Have you followed the steps described above:

"The collapsed areas are marked with duplicate FE-mod shell elements
on top of the original surface mesh of the Macros, on the areas of the problems.
Just before DETECT, these shells must be visible,

The SET "Do not include in Detect" contains the original surface mesh of the
macros from which the layers were grown.
As Now you have the TOP_CAP_Fluid_Layers and the Collapsed Areas FE-mod
shells, these original Macros are set to Hide, so that DETECT can work
without finding duplicate shells"

Can you upload an image of the model?

cfdivan · August 27, 2013, 15:50

Hi Vangelis,

I already tried all the steps but i am still struggling with it. The "BL" mesh is created but by doing autodetec no additional mesh is detected (only "BL" mesh is present). Do you have any clue of what I am doing wrong?

Thank you very much for your help.

vangelis · August 28, 2013, 01:54

Hi cfdivan,

Can you tell me what ANSA reports in the text window at the bottom left
when you press DETECT?
Might it report some duplicate elements?

Also, prior to DETECT can you set in MESH menu
SHADOW OFF
WIRE OFF
BOUNDS ON

so that ANSA displays in red the free edges and in cyan the triple ones?

Can you check if there is a opening in the volume or something like that?

Vangelis

cfdivan · September 14, 2013, 10:07

Hi Vangelis,

I am so sorry to give you a feedbcak too late. Meanwhile I was away from this project.
I already checked the geometry and there is a very small hole in the geometry. Very likely is what messing all up. I already fixed the problem and I'll give a try again.

Thk u very much for your very usefull help.
Regards,

vangelis · September 15, 2013, 16:27

you are welcome cfdivan

i am sure it will work now!

March 10, 2013, 18:18	Volume mesh with layers	#1
AndyZ New Member Join Date: Dec 2011 Posts: 4 Rep Power: 14	Hello, I'm new at using ANSA for CFD meshing. I'm getting a good quality surface mesh for a car model and the road and tunnel walls, but then I'm having some difficulties with the volume mesh. In the ANSA tutorial for external aero, they are using a structured layers mesh only for the road. Since I'm interested in capturing the air speed gradient at the surface of the car, I assume these layers are also supposed to be generated from the car surface. The problem is that afterwards the VOLUME>DEFINE function doesn't recognize the rest of the tunnel volume (without the car and the newly created layers), why is that? There is an autodetected volume, but when I select it nothing gets highlighted. Also, once I do the layers operation, the side walls are reported as unmeshed, although I can still see the mesh grid on them.. Is it a problem if they remain like this?

March 11, 2013, 11:46		#5
AndyZ New Member Join Date: Dec 2011 Posts: 4 Rep Power: 14	Hey, Thanks for your help, it's clearer to me know. I'll try to run my FLUENT analysis tonight with this ANSA mesh, hopefully it's good enough. Volume info is this: According to FLUENT Skewness Average TETRA Quality : 0.259 WORST : 0.9922488 0.00 - 0.10: 350161 15.454 % 0.10 - 0.20: 505417 22.306 % 0.20 - 0.30: 572581 25.270 % 0.30 - 0.40: 446563 19.709 % 0.40 - 0.50: 235915 10.412 % 0.50 - 0.60: 115061 5.078 % 0.60 - 0.70: 34922 1.541 % 0.70 - 0.80: 4223 0.186 % 0.80 - 0.90: 946 0.042 % Worst than 0.90: 44 0.002 % This is after FIX QUALITY command. Any chance it can be improved? And one more thing, I don't know of your experiece with FLUENT, but.. I have imported my mesh into FLUENT (new "Mesh" element in the project, import my mesh there, then drag it over the Mesh in the FLUENT case). In the FLUENT setup, I see that my surfaces "road" and "car" are not found in the Boundary Conditions, I can't specify which boundary to use for drag/lift/moment calculation... What am I missing? Thanks, Andy Last edited by AndyZ; March 11, 2013 at 14:07.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
[Other] mesh airfoil NACA0012	anand_30	OpenFOAM Meshing & Mesh Conversion	13	March 7, 2022 17:22
Gambit problems	Althea	FLUENT	22	January 4, 2017 03:19
[snappyHexMesh] No layers in a small gap	bobburnquist	OpenFOAM Meshing & Mesh Conversion	6	August 26, 2015 09:38
Moving mesh	Niklas Wikstrom (Wikstrom)	OpenFOAM Running, Solving & CFD	122	June 15, 2014 06:20
[ICEM] Generating Mesh for STL Car in Windtunnel Simulation	tommymoose	ANSYS Meshing & Geometry	48	April 15, 2013 04:24

March 11, 2013, 03:18		#2
vangelis Senior Member Vangelis Skaperdas Join Date: Mar 2009 Location: Thessaloniki, Greece Posts: 287 Rep Power: 21	Hi Andy, Which ANSA version are you using? In the external aero tutorial layers are grown from both car wind tunnel road. Now coming to your exact problem. When ANSA grows layers it connect to the side mesh of the windtunnel. To do that it uses ELEMENTs>RELEASE on the four sides where it connects. By RELEASE the elements are de-associated from the geometry and ANSA is free to reconstruct the mesh, create the quad imprint of the layers and connected the layers. As the mesh is RELEASED, these Macros become unmeshed. In order to avoid accidental remeshing (and hence duplicate mesh) These Macros become also Frozen. Play around with the visibility flag buttons for FE-mod and Macros and you will see what I mean. Finally about the problem of Volume detection. Do you have any layer collapsed areas? Open the property list and use Show Only to see if ANSA has collapsed some areas from layers. To perform the DETECT process follow these steps. Check in the VOLUMEs>LIST what volumes you have. You should only have one volume for layers in fact. You can use Show Only on a volume to inspect it. Delete any unecessary volume. Press ALL Ensure Macros and FE-mod mesh flags are active! In the SETs button if there is a SET called Do Not include in Detect Select it and make it Hide. Now press DETECT. Does it work? Best regards Vangelis

March 11, 2013, 05:12		#3
AndyZ New Member Join Date: Dec 2011 Posts: 4 Rep Power: 14	Hello, Thank you for your reply I am using v.13.2.2 You are right about the layers, I read the tutorial more carefully and now I have the whole volume meshed. One question though : I also had a set with collapsed areas, I put that in hide along with the "do not include....." set, is that ok or should I keep the collapsed set visible? Thanks again, Andy

March 11, 2013, 05:36		#4
vangelis Senior Member Vangelis Skaperdas Join Date: Mar 2009 Location: Thessaloniki, Greece Posts: 287 Rep Power: 21	Hi Andy, The collapsed areas are marked with duplicate FE-mod shell elements on top of the original surface mesh of the Macros, on the areas of the problems. Just before DETECT, these shells must be visible, The SET "Do not include in Detect" contains the original surface mesh of the macros from which the layers were grown. As Now you have the TOP_CAP_Fluid_Layers and the Collapsed Areas FE-mod shells, these original Macros are set to Hide, so that DETECT can work without finding duplicate shells. It is a bit complicated but I hope it is clear cheers Vangelis

March 12, 2013, 02:04		#6
vangelis Senior Member Vangelis Skaperdas Join Date: Mar 2009 Location: Thessaloniki, Greece Posts: 287 Rep Power: 21	Hi Andy, If you do not see all the zones in Fluent it may be that not the whole model was visible when you output from ANSA. Go back to ANSA. Press ALL Ensure that FE-mod, Macros and Volumes flag are all active. (I assume that you start ANSA in CFD setup so all quality criteria are predefined for CFD) Press VOLUMEs>IMPROVE>FIX QUAL Visible Check the Volume Stats again, they should be better now. Finally use Fluent output with everything visible. Hope this helps Best regards Vangelis

March 13, 2013, 00:06		#7
AndyZ New Member Join Date: Dec 2011 Posts: 4 Rep Power: 14	Hello, It works, thanks!

March 13, 2013, 02:18		#8
vangelis Senior Member Vangelis Skaperdas Join Date: Mar 2009 Location: Thessaloniki, Greece Posts: 287 Rep Power: 21	You are welcome!

August 15, 2013, 08:37		#9
cfdivan Member Join Date: Jun 2011 Posts: 51 Rep Power: 14	Hi all, I am facing the same problem and I already tried yours sugestion but when I do DETECT i only have fluid_layers. It looks like there is no volume of fluid. Do you have any clue how can I fix this? Thanks!

August 19, 2013, 03:34		#10
vangelis Senior Member Vangelis Skaperdas Join Date: Mar 2009 Location: Thessaloniki, Greece Posts: 287 Rep Power: 21	Hi cfdivan, What message do you get in the text window when you press DETECT? Have you followed the steps described above: "The collapsed areas are marked with duplicate FE-mod shell elements on top of the original surface mesh of the Macros, on the areas of the problems. Just before DETECT, these shells must be visible, The SET "Do not include in Detect" contains the original surface mesh of the macros from which the layers were grown. As Now you have the TOP_CAP_Fluid_Layers and the Collapsed Areas FE-mod shells, these original Macros are set to Hide, so that DETECT can work without finding duplicate shells" Can you upload an image of the model?

August 27, 2013, 15:50		#11
cfdivan Member Join Date: Jun 2011 Posts: 51 Rep Power: 14	Hi Vangelis, I already tried all the steps but i am still struggling with it. The "BL" mesh is created but by doing autodetec no additional mesh is detected (only "BL" mesh is present). Do you have any clue of what I am doing wrong? Thank you very much for your help.

August 28, 2013, 01:54		#12
vangelis Senior Member Vangelis Skaperdas Join Date: Mar 2009 Location: Thessaloniki, Greece Posts: 287 Rep Power: 21	Hi cfdivan, Can you tell me what ANSA reports in the text window at the bottom left when you press DETECT? Might it report some duplicate elements? Also, prior to DETECT can you set in MESH menu SHADOW OFF WIRE OFF BOUNDS ON so that ANSA displays in red the free edges and in cyan the triple ones? Can you check if there is a opening in the volume or something like that? Vangelis

September 14, 2013, 10:07		#13
cfdivan Member Join Date: Jun 2011 Posts: 51 Rep Power: 14	Hi Vangelis, I am so sorry to give you a feedbcak too late. Meanwhile I was away from this project. I already checked the geometry and there is a very small hole in the geometry. Very likely is what messing all up. I already fixed the problem and I'll give a try again. Thk u very much for your very usefull help. Regards,

September 15, 2013, 16:27		#14
vangelis Senior Member Vangelis Skaperdas Join Date: Mar 2009 Location: Thessaloniki, Greece Posts: 287 Rep Power: 21	you are welcome cfdivan i am sure it will work now!