CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > REEF3D

N61 Emergency stop--velocity exceeding critical value in less 0.01 meter mesh size.

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   July 4, 2021, 20:50
Default N61 Emergency stop--velocity exceeding critical value in less 0.01 meter mesh size.
  #1
New Member
 
NSW
Join Date: May 2020
Posts: 20
Rep Power: 4
pipi is on a distinguished road
Hi Reef3d Team,

When I test my CFD model mesh size of less than 0.01 meter, the model almost encounter Emergency stop -- N61 velocity exceeding critical value.

I saw in the user guide the default value of N61 is 500.

How do I deal with this issue? I don't think the 0.005 or 0.007 is a very small mesh size.

The attachment is my summary of the calculation time in different CFL numbers and meshes sizes.

Thanks in advance.

Kind regards
Dongfang
Attached Images
File Type: png issue.png (5.5 KB, 9 views)
File Type: png summary1.png (51.0 KB, 14 views)
File Type: png summary2.png (10.5 KB, 6 views)
pipi is offline   Reply With Quote

Old   July 5, 2021, 09:23
Default
  #2
Senior Member
 
Hans Bihs
Join Date: Jun 2009
Location: Trondheim, Norway
Posts: 146
Rep Power: 14
valgrinda is on a distinguished road
Hi Dongfang,
Which case are you running? That info is needed in order to understand what is going on. Maybe you can share your setup files?
Hans
__________________
Hans Bihs
Team REEF3D
www.reef3d.com
valgrinda is offline   Reply With Quote

Old   July 5, 2021, 09:35
Default
  #3
New Member
 
NSW
Join Date: May 2020
Posts: 20
Rep Power: 4
pipi is on a distinguished road
Hi Hans,

Thanks for your reply.

My case is almost like the 2D Dam Break with tailwater.

The control.txt and ctrl.txt as showing below
-----------------------------------
control.txt
C 11 21
C 12 3
C 13 3
C 14 2
C 15 21
C 16 21

B 1 0.001
B 10 0.0 12.0 0.0 0.05 0.0 1.0
O 10 11.98 12.0 0.0 0.05 0.0 0.1


M 10 24
------------------------------------------------
ctrl.txt
D 10 4
D 20 2
D 30 1
F 30 3
F 40 3
F 50 4
F 70 0.0 0.5 0.0 0.05 0.0 0.5
F 70 0.5 11.98 0.0 0.05 0.0 0.1
N 10 14
N 11 11
N 40 1
N 41 10
N 47 0.1
M 10 24
P 10 1
P 30 0.01
W 22 -9.81
P 61 4.0 0.0 0.05
P 51 4.0 0.0
--------------------------------------------

Kind regards
Dongfang
pipi is offline   Reply With Quote

Old   July 5, 2021, 09:59
Default
  #4
Senior Member
 
Hans Bihs
Join Date: Jun 2009
Location: Trondheim, Norway
Posts: 146
Rep Power: 14
valgrinda is on a distinguished road
Please try with N 40 2 or 3. Let me know whether that works.
Hans
__________________
Hans Bihs
Team REEF3D
www.reef3d.com
valgrinda is offline   Reply With Quote

Old   July 6, 2021, 21:14
Default
  #5
New Member
 
NSW
Join Date: May 2020
Posts: 20
Rep Power: 4
pipi is on a distinguished road
Hi Hans,

I have been finished test models under CFL number = 0.1,0.2,0.3,0.5,0.8,1 and mesh size =0.007,0.005,0.003 situations.

I tested N40 2 and 3, it seems that the results of choosing N40 2 will be better, but the overall performance is still not satisfactory.

The attachment is the summary of the results

Do you have other suggestions?

Kind regards
Dongfang
Attached Images
File Type: png N40 2.png (38.5 KB, 14 views)
pipi is offline   Reply With Quote

Old   July 9, 2021, 15:20
Default
  #6
Senior Member
 
Hans Bihs
Join Date: Jun 2009
Location: Trondheim, Norway
Posts: 146
Rep Power: 14
valgrinda is on a distinguished road
Hi Dongfang,

I have had a look at the case. A couple of remarks:
- see the attached control files, that setup runs well for me
- more efficient to go fully 2D, that means only 1 cell in y-direction
- since it is 2D, there is no need to go to 0.001m cells, this is way too fine for this case. With 0.01m dx, there is still a lot of detail, including the breaking waves.
- I used 3rd-order RK, it just (always) works
- what about the outflow? it looks like it should be free stream, so I used B 77 2
- also regarding the outflow: I haven't changed your geometry, but it is better to extend the domain a bit and avoid sudden geometry changes just before the outflow. Why have the step there if you don't want to model it?
Attached Files
File Type: txt ctrl.txt (219 Bytes, 9 views)
File Type: txt control.txt (139 Bytes, 9 views)
__________________
Hans Bihs
Team REEF3D
www.reef3d.com
valgrinda is offline   Reply With Quote

Old   July 12, 2021, 01:14
Default
  #7
New Member
 
NSW
Join Date: May 2020
Posts: 20
Rep Power: 4
pipi is on a distinguished road
Dear Hans,

Thanks for your suggestion! It's very useful! REEF3D could successfully simulate a very small mesh size (0.01m).

I think making sure just one cell in the y-direction is very important.

In some cases, the reservoir height is not too great (0.14m), I could even get the result under the mesh size smaller than 0.01m (I test 0.007m, 0.005m, 0.003m.), All works well!

However, when I use 0.36m reservoir height, the model still encounters N61 emergency stop question when I set mesh size smaller than 0.01m. I try N40 3, N40 6, all of these cannot work. I think it may very unstable for the model to simulate a very high reservoir collapses process. So if I really want to make the mesh size is smaller than 0.01m, which part you recommend for me to concentrate on to modify this model?


Kind regards
Dongfang
pipi is offline   Reply With Quote

Old   July 12, 2021, 10:15
Default
  #8
Senior Member
 
Hans Bihs
Join Date: Jun 2009
Location: Trondheim, Norway
Posts: 146
Rep Power: 14
valgrinda is on a distinguished road
Hi Dongfang,

at which stage do you get the crash for the reservoir height of 0.36m? At the beginning when you see the breaking waves or when the wave hits the outflow?
__________________
Hans Bihs
Team REEF3D
www.reef3d.com
valgrinda is offline   Reply With Quote

Old   July 12, 2021, 10:46
Default
  #9
New Member
 
NSW
Join Date: May 2020
Posts: 20
Rep Power: 4
pipi is on a distinguished road
Dear Hans,

It depends on the mesh size. I set the simulated time as 10s, when the mesh size is 0.007m or 0.005m, the model will stop at around 8s, but when the mesh size is 0.003, the model will stop around 1s.

Another thing, Hans, the maximum speed obtained by the model is half lower than the results obtained in the lab. The velocity difference is significant.

I try to set the viscosity of water to 0 but the velocity change is small, just increase a little bit. I guess this may be because in the early stage of the reservoir collapse, in order to stabilize the model, the internal algorithm cut some energy, Resulting in the flow velocity being smaller than the lab value. In order to increase the flow velocity, which part of the settings do you think I should pay attention to, or which settings can have a great impact on the flow velocity?

Kind regards
Dongfang
pipi is offline   Reply With Quote

Old   July 13, 2021, 05:49
Default
  #10
Senior Member
 
Hans Bihs
Join Date: Jun 2009
Location: Trondheim, Norway
Posts: 146
Rep Power: 14
valgrinda is on a distinguished road
Hi Dongfang,

could you send me the setup of the experiments? It sounds, like there is a mismatch.
__________________
Hans Bihs
Team REEF3D
www.reef3d.com
valgrinda is offline   Reply With Quote

Old   July 16, 2021, 06:58
Default
  #11
New Member
 
NSW
Join Date: May 2020
Posts: 20
Rep Power: 4
pipi is on a distinguished road
Hi Hans,

I think I have been solved this issue, thanks for your help, the model works well!

Thanks again for your patient explanation!

Kind regards
Dongfang
pipi is offline   Reply With Quote

Old   July 16, 2021, 07:06
Default
  #12
Senior Member
 
Hans Bihs
Join Date: Jun 2009
Location: Trondheim, Norway
Posts: 146
Rep Power: 14
valgrinda is on a distinguished road
Great to hear!
__________________
Hans Bihs
Team REEF3D
www.reef3d.com
valgrinda is offline   Reply With Quote

Old   July 20, 2021, 08:46
Default
  #13
New Member
 
NSW
Join Date: May 2020
Posts: 20
Rep Power: 4
pipi is on a distinguished road
Dear Hans,

Sorry to bother you again.

I simulate a Dam break process contain tailwater (as showing in the figure). I tested this model under the same mesh size (0.005m), but different CFL value (0.1,0.2,0.3,0.5,0.8,1), the tailwater height has a dramatic decrease at the beginning of simulation when the CFL value is great(as showing in the figure), because there is an object at the outlet which height equal to tailwater height, so I think significant tailwater height reduction should not happen in theory. . .

Do you have some opinion about it?

Thanks a lot!

Kind regards
Dongfang
Attached Images
File Type: png Model.png (3.7 KB, 6 views)
File Type: png Different CFL number result.png (110.2 KB, 6 views)
Attached Files
File Type: txt control.txt (136 Bytes, 0 views)
File Type: txt ctrl.txt (311 Bytes, 2 views)
pipi is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
sliding mesh problem in CFX Saima CFX 46 September 11, 2021 08:38
foam-extend-4.1 release hjasak OpenFOAM Announcements from Other Sources 19 July 16, 2021 06:02
Worse accuracy in LES models than in RANS models dferrando OpenFOAM Running, Solving & CFD 0 August 30, 2017 05:56
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 12:55
How to control Minximum mesh space? hung FLUENT 7 April 18, 2005 10:38


All times are GMT -4. The time now is 21:39.