[ICEM] Boundary Layer Y+ Mesh Not Working as Expected

abhi.jam22 · February 4, 2017, 22:24

Hey,

I am using ICEM to generate quadrilateral and hexahedral grids for Airfoils and Wings. The flow Re number is 3 million. The corresponding first cell center height for a grid with y+ <1 is 8.5e-6m. Now earlier I have generated grids without any problem but for the recent work that I am doing I am not getting the grid spacing as I wish. A considerable number of cells from the airfoil wall have a constant thickness even though I have specified the grid growth ratio as 1.2. And the corresponding first cell height is less than required. I have attached pictures which will help explain the problem.
Any help is appreciated. It is causing problems when I solve for the flow.

Thanks

https://drive.google.com/open?id=0B4...TdOMTZjdV8yalU

https://drive.google.com/open?id=0B4...k5STUtILTRYakk

https://drive.google.com/open?id=0B4...TdOMTZjdV8yalU

Wingman · February 5, 2017, 19:11

I'm also simulating airfoils but I'm fairly new. According to what I've read in Fluent Theory guide it is recommended that you apply meshes with Y+ < 1 and expansion factors smaller than 1.1 - but you should keep it above 1.05. Before I read that I always used growth ratio of 1.2.

I can't view your figures. You can attach them to the post. Also upload a screenshot of your edge bunching settings.

abhi.jam22 · February 5, 2017, 19:26

Hey,

I have attached the pics now. Kindly have a look and let me know if you can figure something out.

I have tried various growth ratios and none seem to work. The edge spacing markers seems alright but the grid being formed does not match the markers.

Wingman · February 5, 2017, 19:41

Quote:

Originally Posted by abhi.jam22

Hey,

I have attached the pics now. Kindly have a look and let me know if you can figure something out.

I have tried various growth ratios and none seem to work. The edge spacing markers seems alright but the grid being formed does not match the markers.

Try not to define the Spacing 1.
Spacing 1 = 0

abhi.jam22 · February 5, 2017, 19:51

Tried that as well. Didn't work.

If I reduce the spacing 2 to 8.5e-4, it works fine but then my first cell wouldn't be in y+<1 range.

PLD · February 7, 2017, 07:10

Hi,

I have exactly the same problem as you (Edge nodes distribution not properly used with ICEM v17.1 ).

What version of ICEM are you using? I only encountered this issue with v17.1, I have no problem with v16.2. A blocking that was working with v16.2 does not work the same way with v17.1 and shows the error you get. So my guess is that it could be kind of a bug of v17.1...

So far I have not found how to fix that and this is quite annoying... Now that this is not only me, maybe we should contact ANSYS directly.

Wingman · February 7, 2017, 14:39

Hi,

I'm not sure if it's a similar problem I had once. My triangular mesh didn't generate when I had really small wall spacing. I had it fixed by increasing the number of processors ICEM could use. I think by default it is 1 processor.

Settings -> General -> Number of Processors.

I think if you set value of 0... It will use the maximum number of available processors. You can also fix the number as 2, 4 or as many processors you have. Give it a try!

abhi.jam22 · February 7, 2017, 22:51

I am using v17.1. I will have to try this with some other version as well to check if that is the issue. Any idea how to go about getting this to ansys?

abhi.jam22 · February 7, 2017, 22:55

I changed the processors to 4. Didn't solve the problem.

PLD · February 8, 2017, 07:29

Hi Abhimanyu,

I have just sent an email to ANSYS support. I will let you know when they reply.

PLD · February 8, 2017, 12:40

Hi,

I just got a reply. Actually we just need to modify the Triangulation Tolerance (Settings > Model/Units). Set it to 1e-7 and everything should be fine. You may need to adjust the value but it works in my case.

The default value was probably different in the previous versions...

Regards,

abhi.jam22 · February 9, 2017, 23:48

Yeah...It worked. But I opened the project file in ICEM v14 and there it had no issues with the default tolerance settings. And they were the same as v17 i.e. default of 0.001. Weird behavior.

But atleast we got the solution. Thanks for reaching out to ansys and getting it done.

February 4, 2017, 22:24	Boundary Layer Y+ Mesh Not Working as Expected	#1
abhi.jam22 New Member Abhimanyu Join Date: Jul 2014 Posts: 19 Rep Power: 12	Hey, I am using ICEM to generate quadrilateral and hexahedral grids for Airfoils and Wings. The flow Re number is 3 million. The corresponding first cell center height for a grid with y+ <1 is 8.5e-6m. Now earlier I have generated grids without any problem but for the recent work that I am doing I am not getting the grid spacing as I wish. A considerable number of cells from the airfoil wall have a constant thickness even though I have specified the grid growth ratio as 1.2. And the corresponding first cell height is less than required. I have attached pictures which will help explain the problem. Any help is appreciated. It is causing problems when I solve for the flow. Thanks https://drive.google.com/open?id=0B4...TdOMTZjdV8yalU https://drive.google.com/open?id=0B4...k5STUtILTRYakk https://drive.google.com/open?id=0B4...TdOMTZjdV8yalU

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
[snappyHexMesh] sHM layer process keeps getting killed	MBttR	OpenFOAM Meshing & Mesh Conversion	4	August 15, 2016 04:21
[snappyHexMesh] SnappyHexMesh no layers and no decent mesh for complex geometry	pizzaspinate	OpenFOAM Meshing & Mesh Conversion	1	February 25, 2015 08:05
[snappyHexMesh] Layers:problem with curvature	giulio.topazio	OpenFOAM Meshing & Mesh Conversion	10	August 22, 2012 10:03
POSDAT problem	piotka	STAR-CD	4	June 12, 2009 09:43
errors	Fahad	Main CFD Forum	0	March 23, 2004 14:20

February 5, 2017, 19:11		#2
Wingman Member William Join Date: Aug 2016 Posts: 56 Rep Power: 10	I'm also simulating airfoils but I'm fairly new. According to what I've read in Fluent Theory guide it is recommended that you apply meshes with Y+ < 1 and expansion factors smaller than 1.1 - but you should keep it above 1.05. Before I read that I always used growth ratio of 1.2. I can't view your figures. You can attach them to the post. Also upload a screenshot of your edge bunching settings.

February 5, 2017, 19:51		#5
abhi.jam22 New Member Abhimanyu Join Date: Jul 2014 Posts: 19 Rep Power: 12	Tried that as well. Didn't work. If I reduce the spacing 2 to 8.5e-4, it works fine but then my first cell wouldn't be in y+<1 range.

February 7, 2017, 07:10		#6
PLD New Member Pierre-Luc Join Date: Oct 2011 Location: UK Posts: 16 Rep Power: 15	Hi, I have exactly the same problem as you (Edge nodes distribution not properly used with ICEM v17.1 ). What version of ICEM are you using? I only encountered this issue with v17.1, I have no problem with v16.2. A blocking that was working with v16.2 does not work the same way with v17.1 and shows the error you get. So my guess is that it could be kind of a bug of v17.1... So far I have not found how to fix that and this is quite annoying... Now that this is not only me, maybe we should contact ANSYS directly.

February 7, 2017, 14:39		#7
Wingman Member William Join Date: Aug 2016 Posts: 56 Rep Power: 10	Hi, I'm not sure if it's a similar problem I had once. My triangular mesh didn't generate when I had really small wall spacing. I had it fixed by increasing the number of processors ICEM could use. I think by default it is 1 processor. Settings -> General -> Number of Processors. I think if you set value of 0... It will use the maximum number of available processors. You can also fix the number as 2, 4 or as many processors you have. Give it a try!

February 7, 2017, 22:51		#8
abhi.jam22 New Member Abhimanyu Join Date: Jul 2014 Posts: 19 Rep Power: 12	I am using v17.1. I will have to try this with some other version as well to check if that is the issue. Any idea how to go about getting this to ansys?

February 7, 2017, 22:55		#9
abhi.jam22 New Member Abhimanyu Join Date: Jul 2014 Posts: 19 Rep Power: 12	I changed the processors to 4. Didn't solve the problem.

February 8, 2017, 07:29		#10
PLD New Member Pierre-Luc Join Date: Oct 2011 Location: UK Posts: 16 Rep Power: 15	Hi Abhimanyu, I have just sent an email to ANSYS support. I will let you know when they reply.

February 8, 2017, 12:40		#11
PLD New Member Pierre-Luc Join Date: Oct 2011 Location: UK Posts: 16 Rep Power: 15	Hi, I just got a reply. Actually we just need to modify the Triangulation Tolerance (Settings > Model/Units). Set it to 1e-7 and everything should be fine. You may need to adjust the value but it works in my case. The default value was probably different in the previous versions... Regards,

February 9, 2017, 23:48		#12
abhi.jam22 New Member Abhimanyu Join Date: Jul 2014 Posts: 19 Rep Power: 12	Yeah...It worked. But I opened the project file in ICEM v14 and there it had no issues with the default tolerance settings. And they were the same as v17 i.e. default of 0.001. Weird behavior. But atleast we got the solution. Thanks for reaching out to ansys and getting it done.