How to apply AMR settings

kahjoonyong · July 24, 2017, 07:51

Hello,

I am trying to simulate a simple 2D turbulence flow through a channel with hill in order to get my hand on this software. The idea is to be able to hone my skill using this software before proceeding to a simulation for a reactive flow.

The profile is taken directly from this simulation from NASA, https://turbmodels.larc.nasa.gov/Oth..._periodic.html

Here is a link (http://imgur.com/a/hMS7S) to my case setup and geometry.

I have first simulated this case using only fixed embedding at the top and bottom wall boundary. The simulation was done using both k-Epsilon and k-Omega turbulence model. The results could be seen in the link as well. However the base grid I used for this settings is very fine throughout the profile and it took a long time to simulate. Therefore I would like to try out the AMR setting.

However, AMR would not activate throughout the whole simulation. The number of cells do not increase and no mesh refinement was seen in the post processed results. I have tried to coarsen/refine the base grid, manipulate the grid ratio, deactivate Fixed Embedding, manipulate the embedding scale either or both in Fixed Embedding or/and AMR settings, etc. Nothing seems to work. The only time AMR was shown working is when I increase the 'minimum cells' setting to a very high number. Nevertheless, the simulation crashed when the cell count increased.

I have been trying out different combinations of settings over the course of two weeks. I have been looking everywhere in the internet and in manuals, nothing gives useful resources. I hope someone could take a look in it.

I have attached the .cvg file of the case here as well. Hill.zip
The boundary settings for the wall might vary a little from what I have written in the following lines because I have tested other settings as well. For k-Omega No-Slip boundary conditions are applied.

Short overview of the boundaries:

1. Top and Bottom:
Wall
Velocity: Law of wall
Temperature: Specified value

2. Left Inlet:
Inflow
Velocity in x-Direction 5m/s
Pressure: Zero normal gradient

3. Right outlet
Outflow
Velocity: Zero normal gradient
Pressure: 101325Pa

4. Front and Back
2D

Thank you.

MFGT · July 24, 2017, 08:45

Hi,

from the CONVERGE Manual:

Definition of "amr_vel_sgs_embed": Sub-grid velocity above which a cell will be embedded. 0.1% to 10% of the characteristic velocity in domain

So i would say if your max. Velocity is somewhat between 5 and 6 m/s, your subgridscale of 1m/s is way to high to trigger AMR.
Try reducing this to maybe 0.25, which would be 5% of 5m/s then.

kahjoonyong · July 24, 2017, 08:48

Thank you very much to your reply. I will try it out. I have previously tried 0.1 m/s as well as 0.001m/s, both of them failed. I will try again anyway. I will update you as soon as I have a result.

MFGT · July 24, 2017, 09:12

Which release of CONVERGE do you use?

kahjoonyong · July 24, 2017, 09:13

I am using Converge 2.3

kahjoonyong · July 24, 2017, 10:29

Hello MFGT,

I have ran the simulation with a subgrid scale of 0.25m/s. It did not work. Only Fixed embedding is seen in the final results. I have tried to increase the embedding level to 5 in another simulation. It did not trigger.

Blanco · July 24, 2017, 11:46

Quote:

Originally Posted by kahjoonyong

Thank you very much to your reply. I will try it out. I have previously tried 0.1 m/s as well as 0.001m/s, both of them failed. I will try again anyway. I will update you as soon as I have a result.

The maximum number of cells set in AMR is 100k, which is too low because your base grid should bring to approx. 142k cells. You should increase the maximum number of cells to allow AMR work properly.

kahjoonyong · July 24, 2017, 11:47

Hi MFGT,

I have varied the value of the subgrid velocity to an even smaller value and finally AMR triggered! Thank you very much!

kahjoonyong · July 24, 2017, 11:48

Hi Blanco! That is the reason why it crashed after it triggered! Thank you so much! I just wanted to investigate.

ymao · July 24, 2017, 11:50

Kaihjoonyong,

I have tested this case in Converge.2.3. The AMR actually worked if you changed the sub-grid criterion to very small value, such as 1e-8m/s. At cycle of 501, the cell count increased to 48975 from 14760.

Just for your record,
Regarding on how I choose this sub-velocity criterion of 1e-8m/s, in fact, Converge could output this value through non-transport passive of VEL_SGS.

1) Materials>Species>Non-transport Passive, Add, type VEL_SGS
2) Output/Post Processing > Post variable selection > Cells > Species/Passive, Check box 'Passive', select VEL_SGS through drop-down menu

Given this VEL_SGS, we could test AMR trigger easily.

kahjoonyong · July 24, 2017, 12:00

Quote:

Originally Posted by ymao

Kaihjoonyong,

I have tested this case in Converge.2.3. The AMR actually worked if you changed the sub-grid criterion to very small value, such as 1e-8m/s. At cycle of 501, the cell count increased to 48975 from 14760.

Just for your record,
Regarding on how I choose this sub-velocity criterion of 1e-8m/s, in fact, Converge could output this value through non-transport passive of VEL_SGS.

1) Materials>Species>Non-transport Passive, Add, type VEL_SGS
2) Output/Post Processing > Post variable selection > Cells > Species/Passive, Check box 'Passive', select VEL_SGS through drop-down menu

Given this VEL_SGS, we could test AMR trigger easily.

Hello Yijin Mao,

Thank you vary much for your advice! This is going to be very helpful. I will take note of that.

Also shout out to MFGT and Blanco for the quick solution. You basically just saved my day.

Kah Joon Yong

MFGT · July 28, 2017, 04:18

Good to know it finally worked.
Since i use the code for engine simulation only, the amr settings from the examples pretty much fit my simulations.

Also, i cant afford to get more and more cells. The maximum is around 2mio for my cases. So a subgrid scale of 1m/s for velocity and 2.5K for temperature work fine in engine cases.

July 24, 2017, 07:51	How to apply AMR settings	#1
kahjoonyong New Member Kah Joon Yong Join Date: Jul 2017 Location: Munich, Germany Posts: 23 Rep Power: 8	Hello, I am trying to simulate a simple 2D turbulence flow through a channel with hill in order to get my hand on this software. The idea is to be able to hone my skill using this software before proceeding to a simulation for a reactive flow. The profile is taken directly from this simulation from NASA, https://turbmodels.larc.nasa.gov/Oth..._periodic.html Here is a link (http://imgur.com/a/hMS7S) to my case setup and geometry. I have first simulated this case using only fixed embedding at the top and bottom wall boundary. The simulation was done using both k-Epsilon and k-Omega turbulence model. The results could be seen in the link as well. However the base grid I used for this settings is very fine throughout the profile and it took a long time to simulate. Therefore I would like to try out the AMR setting. However, AMR would not activate throughout the whole simulation. The number of cells do not increase and no mesh refinement was seen in the post processed results. I have tried to coarsen/refine the base grid, manipulate the grid ratio, deactivate Fixed Embedding, manipulate the embedding scale either or both in Fixed Embedding or/and AMR settings, etc. Nothing seems to work. The only time AMR was shown working is when I increase the 'minimum cells' setting to a very high number. Nevertheless, the simulation crashed when the cell count increased. I have been trying out different combinations of settings over the course of two weeks. I have been looking everywhere in the internet and in manuals, nothing gives useful resources. I hope someone could take a look in it. I have attached the .cvg file of the case here as well. Hill.zip The boundary settings for the wall might vary a little from what I have written in the following lines because I have tested other settings as well. For k-Omega No-Slip boundary conditions are applied. Short overview of the boundaries: 1. Top and Bottom: Wall Velocity: Law of wall Temperature: Specified value 2. Left Inlet: Inflow Velocity in x-Direction 5m/s Pressure: Zero normal gradient 3. Right outlet Outflow Velocity: Zero normal gradient Pressure: 101325Pa 4. Front and Back 2D Thank you.

July 24, 2017, 11:50		#10
ymao New Member Yijin Mao Join Date: Jun 2017 Location: Convergent Science, Madison WI Posts: 20 Rep Power: 8	Kaihjoonyong, I have tested this case in Converge.2.3. The AMR actually worked if you changed the sub-grid criterion to very small value, such as 1e-8m/s. At cycle of 501, the cell count increased to 48975 from 14760. Just for your record, Regarding on how I choose this sub-velocity criterion of 1e-8m/s, in fact, Converge could output this value through non-transport passive of VEL_SGS. 1) Materials>Species>Non-transport Passive, Add, type VEL_SGS 2) Output/Post Processing > Post variable selection > Cells > Species/Passive, Check box 'Passive', select VEL_SGS through drop-down menu Given this VEL_SGS, we could test AMR trigger easily. __________________ __________________ *Yijin Mao, Ph.D.* Support/Application Engineer CONVERGECFD

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Two computer cluster - problems with settings	dradenkovic	OpenFOAM Running, Solving & CFD	9	November 13, 2017 04:16
Lift and Drag coeff change with V 16 and 13 PISO for same mesh file and same settings	arunraj	FLUENT	0	June 2, 2016 22:43
[OpenFOAM.org] Compile OF 2.3 on Mac OS X .... the patch	gschaider	OpenFOAM Installation	225	August 25, 2015 19:43
Fluid-Solid Interface Settings for a Rotating Water Container	r.mojtaba	CFX	4	October 14, 2013 19:01
thermoBaffleProperties object settings	calim_cfd	OpenFOAM	0	October 4, 2011 10:17

July 24, 2017, 08:45		#2
MFGT Senior Member Tobias Join Date: May 2016 Location: Germany Posts: 267 Rep Power: 11	Hi, from the CONVERGE Manual: Definition of "amr_vel_sgs_embed": Sub-grid velocity above which a cell will be embedded. 0.1% to 10% of the characteristic velocity in domain So i would say if your max. Velocity is somewhat between 5 and 6 m/s, your subgridscale of 1m/s is way to high to trigger AMR. Try reducing this to maybe 0.25, which would be 5% of 5m/s then.

July 24, 2017, 08:48		#3
kahjoonyong New Member Kah Joon Yong Join Date: Jul 2017 Location: Munich, Germany Posts: 23 Rep Power: 8	Thank you very much to your reply. I will try it out. I have previously tried 0.1 m/s as well as 0.001m/s, both of them failed. I will try again anyway. I will update you as soon as I have a result.

July 24, 2017, 09:12		#4
MFGT Senior Member Tobias Join Date: May 2016 Location: Germany Posts: 267 Rep Power: 11	Which release of CONVERGE do you use?

July 24, 2017, 09:13		#5
kahjoonyong New Member Kah Joon Yong Join Date: Jul 2017 Location: Munich, Germany Posts: 23 Rep Power: 8	I am using Converge 2.3

July 24, 2017, 10:29		#6
kahjoonyong New Member Kah Joon Yong Join Date: Jul 2017 Location: Munich, Germany Posts: 23 Rep Power: 8	Hello MFGT, I have ran the simulation with a subgrid scale of 0.25m/s. It did not work. Only Fixed embedding is seen in the final results. I have tried to increase the embedding level to 5 in another simulation. It did not trigger.

July 24, 2017, 11:47		#8
kahjoonyong New Member Kah Joon Yong Join Date: Jul 2017 Location: Munich, Germany Posts: 23 Rep Power: 8	Hi MFGT, I have varied the value of the subgrid velocity to an even smaller value and finally AMR triggered! Thank you very much!

July 24, 2017, 11:48		#9
kahjoonyong New Member Kah Joon Yong Join Date: Jul 2017 Location: Munich, Germany Posts: 23 Rep Power: 8	Hi Blanco! That is the reason why it crashed after it triggered! Thank you so much! I just wanted to investigate.

July 28, 2017, 04:18		#12
MFGT Senior Member Tobias Join Date: May 2016 Location: Germany Posts: 267 Rep Power: 11	Good to know it finally worked. Since i use the code for engine simulation only, the amr settings from the examples pretty much fit my simulations. Also, i cant afford to get more and more cells. The maximum is around 2mio for my cases. So a subgrid scale of 1m/s for velocity and 2.5K for temperature work fine in engine cases.