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

Periodic boundary condition at Inlet and outlet with Massflow

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

Like Tree3Likes

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   August 1, 2022, 09:04
Default Periodic boundary condition at Inlet and outlet with Massflow
  #1
Member
 
Meysam
Join Date: Dec 2019
Posts: 80
Rep Power: 6
MNMK is on a distinguished road
Hi,

I would like to simulate a corrugated pipe to calculate the pressure drop at different lengths. To reduce the calculation time, I wanted to simulate a section of the duct. I define a periodic interface at inlet and outlet with the Massflow. After 100 iterations, there is a fatal overflow. I would like to know where my mistake was?

regards,
MNMK is offline   Reply With Quote

Old   August 1, 2022, 15:34
Default
  #2
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,827
Rep Power: 27
Gert-Jan will become famous soon enough
This can be anything. With unrealistic boundary conditions, weird numerical settings, or similar, you can get a fatal error. Please look here


https://www.cfd-online.com/Wiki/Ansy...do_about_it.3F
Gert-Jan is offline   Reply With Quote

Old   August 1, 2022, 15:49
Default
  #3
Member
 
Meysam
Join Date: Dec 2019
Posts: 80
Rep Power: 6
MNMK is on a distinguished road
Quote:
Originally Posted by Gert-Jan View Post
This can be anything. With unrealistic boundary conditions, weird numerical settings, or similar, you can get a fatal error. Please look here


https://www.cfd-online.com/Wiki/Ansy...do_about_it.3F
Hi,

thank for your answer. Is my boundary defination correct?
I created an interface with Inlet and Outlet in region list. and also enter the massflow ratio at Inlet interface.
the mesh quality can not be a problem because I got the same error in a simple cylinder.

wishes
MNMK is offline   Reply With Quote

Old   August 1, 2022, 17:33
Default
  #4
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,827
Rep Power: 27
Gert-Jan will become famous soon enough
please post the output file
Gert-Jan is offline   Reply With Quote

Old   August 2, 2022, 04:59
Default
  #5
Member
 
Meysam
Join Date: Dec 2019
Posts: 80
Rep Power: 6
MNMK is on a distinguished road
Quote:
Originally Posted by Gert-Jan View Post
please post the output file
I attached the output file
Attached Files
File Type: txt output.txt (94.4 KB, 10 views)
MNMK is offline   Reply With Quote

Old   August 2, 2022, 05:39
Default
  #6
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,827
Rep Power: 27
Gert-Jan will become famous soon enough
You have only 1 wall? Is it a segment of a straight pipe?
You have 1 gram/s of air as target for the periodic flow, so the software is solving the pressure required to obtain this flow. The Results section says:

| Velocity w | -6.17E+02 | -3.65E+02 |
| Pressure | -1.03E+04 | 1.34E+05 |

This is supersonic flow, whereas you are running isothermal. What are you up to?
I don't know your geometry looks like, but what problem do you want to solve when doing CFD?
How do the results look like in Post? Does it look reaslitic? Isn't the inlet mass flow way too much?
Gert-Jan is offline   Reply With Quote

Old   August 2, 2022, 05:55
Default
  #7
Member
 
Meysam
Join Date: Dec 2019
Posts: 80
Rep Power: 6
MNMK is on a distinguished road
Quote:
Originally Posted by Gert-Jan View Post
You have only 1 wall? Is it a segment of a straight pipe?
You have 1 gram/s of air as target for the periodic flow, so the software is solving the pressure required to obtain this flow. The Results section says:

| Velocity w | -6.17E+02 | -3.65E+02 |
| Pressure | -1.03E+04 | 1.34E+05 |

This is supersonic flow, whereas you are running isothermal. What are you up to?
I don't know your geometry looks like, but what problem do you want to solve when doing CFD?
How do the results look like in Post? Does it look reaslitic? Isn't the inlet mass flow way too much?
Dear Gen,

As I mentioned, my aim is to simulate a corrugated pipe and, because of reducing the calculation time and the number of meshes, I would like to simulate a section. Firstly, I used a simple duct (a cylinder) to be sure my boundary conditions were rational. The high amount of velocity and pressure shows the calculation is not convergence, which is my problem. I tried again to solve it with a smaller time step, which looks better even my Momentum and mass residuals are not perfect.

wishes
MNMK is offline   Reply With Quote

Old   August 2, 2022, 06:46
Default
  #8
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,827
Rep Power: 27
Gert-Jan will become famous soon enough
You need to be sure your boundary conditions are realistic. Then you can judge convergence.
1 g/s of air, is about 1 liter per second. Can you get that through your section?
Not knowing how your geometry looks like........does this 1 l/s apply for the whole cross section (360) or only for a pie of (5).

Maybe it is better to first try a pressure drop and see what mass flow you get. Start with a dp of 1 Pa.
MNMK likes this.
Gert-Jan is offline   Reply With Quote

Old   August 2, 2022, 06:51
Default
  #9
Member
 
Meysam
Join Date: Dec 2019
Posts: 80
Rep Power: 6
MNMK is on a distinguished road
Quote:
Originally Posted by Gert-Jan View Post
You need to be sure your boundary conditions are realistic. Then you can judge convergence.
1 g/s of air, is about 1 liter per second. Can you get that through your section?
Not knowing how your geometry looks like........does this 1 l/s apply for the whole cross section (360) or only for a pie of (5).

Maybe it is better to first try a pressure drop and see what mass flow you get. Start with a dp of 1 Pa.
It flows through whole cross section(360). I will try it.
MNMK is offline   Reply With Quote

Old   August 26, 2022, 08:10
Default
  #10
Member
 
Meysam
Join Date: Dec 2019
Posts: 80
Rep Power: 6
MNMK is on a distinguished road
Hello again,

I have found a solution to simulate a simple duct with the periodic boundary condition. Firstly, I simulated the duct with the inlet (mass flow) and outlet (relative pressure zero) boundary condition with Auto timescale. Then from the out file of the convergence calculation, I chose the best Timescale and used it for my periodic calculation, which worked so well.
Now my problem is this method for the corrugated pipe does not work. Now my problem is this method for the corrugated pipe does not work. Are there any ideas or suggestions? I have attached a photo of my geometry and the out file.

Capture1.PNG
MNMK is offline   Reply With Quote

Old   August 26, 2022, 08:12
Default
  #11
Member
 
Meysam
Join Date: Dec 2019
Posts: 80
Rep Power: 6
MNMK is on a distinguished road
I don`t know why I can not upload the out file.
MNMK is offline   Reply With Quote

Old   August 26, 2022, 10:21
Default
  #12
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,827
Rep Power: 27
Gert-Jan will become famous soon enough
And why doesn't it work? What is the problem?
Gert-Jan is offline   Reply With Quote

Old   August 26, 2022, 11:06
Default
  #13
Member
 
Meysam
Join Date: Dec 2019
Posts: 80
Rep Power: 6
MNMK is on a distinguished road
Quote:
Originally Posted by Gert-Jan View Post
And why doesn't it work? What is the problem?
It says Invalid file when I upload .

may I send you per Email?
MNMK is offline   Reply With Quote

Old   August 26, 2022, 11:13
Default
  #14
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,827
Rep Power: 27
Gert-Jan will become famous soon enough
Quote:
Originally Posted by MNMK View Post
Hello again,

I have found a solution to simulate a simple duct with the periodic boundary condition. Firstly, I simulated the duct with the inlet (mass flow) and outlet (relative pressure zero) boundary condition with Auto timescale. Then from the out file of the convergence calculation, I chose the best Timescale and used it for my periodic calculation, which worked so well.
Now my problem is this method for the corrugated pipe does not work. Now my problem is this method for the corrugated pipe does not work. Are there any ideas or suggestions? I have attached a photo of my geometry and the out file.

Attachment 91342
And why doesn't it work? What is the problem?
Gert-Jan is offline   Reply With Quote

Old   August 26, 2022, 11:15
Default
  #15
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,827
Rep Power: 27
Gert-Jan will become famous soon enough
Quote:
Originally Posted by MNMK View Post
It says Invalid file when I upload .

may I send you per Email?

That is weird. I presume you tried the "attachments" in Advanced mode?
MNMK likes this.
Gert-Jan is offline   Reply With Quote

Old   August 27, 2022, 00:33
Default
  #16
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,703
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
I think there is a size limit on attachments on the forum, and it is quite small, maybe 100kB.

Also, I do not think a ".out" file is a valid file type for the forum either. Rename it as a ".txt" file and try again.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   August 29, 2022, 02:37
Default
  #17
Member
 
Meysam
Join Date: Dec 2019
Posts: 80
Rep Power: 6
MNMK is on a distinguished road
Quote:
Originally Posted by Gert-Jan View Post
That is weird. I presume you tried the "attachments" in Advanced mode?
Dear Gert-Jan,

I had to delete some Iterations because of file size limit. However, I think necessary information is included.

wishes,
Attached Files
File Type: txt text.txt (190.1 KB, 3 views)
MNMK is offline   Reply With Quote

Old   August 29, 2022, 03:56
Default
  #18
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,827
Rep Power: 27
Gert-Jan will become famous soon enough
- You have a FINMES error. This means Final Message. Not very helpful
- You use k epsilon. Better use SST
- Why do you use a physical timestepping. Better use auto timescale and let CFX determine the size based on occurring phenomena.
- Your case is not converging at all. Did you create a backup just before the crash? If not, please do. This might help in finding the cause.
- The modelling approach you use, with translational peridicity works pretty will, if the tubes are straight. Then the velocity in and out have a change to make sense, provided there is no huge recirculation and backflow in the outlet, because that will appear at the inlet as well, which the solver does not like. For the same reason, it is common practice in CFD in general to move outlets downstream such that objects of interest do not influence outlets and vice versa. In your geometry, you have a similar problem. I think there will be many recirculations just in front of your outlet that will affect the flow in the inlet. Therefore I am not convinced your approach will work for this geometry.
- Did you try to perform a simulation on a segment instead of full 360? This might help.
- Did you try to make the interface on the smallest diameter instead of the largest diameter. I would expect that to work better since the recirculations close to the outlet will be reduced.
Gert-Jan is offline   Reply With Quote

Old   August 29, 2022, 04:08
Default
  #19
Member
 
Meysam
Join Date: Dec 2019
Posts: 80
Rep Power: 6
MNMK is on a distinguished road
Quote:
Originally Posted by Gert-Jan View Post
- You have a FINMES error. This means Final Message. Not very helpful
- You use k epsilon. Better use SST
- Why do you use a physical timestepping. Better use auto timescale and let CFX determine the size based on occurring phenomena.
- Your case is not converging at all. Did you create a backup just before the crash? If not, please do. This might help in finding the cause.
- The modelling approach you use, with translational peridicity works pretty will, if the tubes are straight. Then the velocity in and out have a change to make sense, provided there is no huge recirculation and backflow in the outlet, because that will appear at the inlet as well, which the solver does not like. For the same reason, it is common practice in CFD in general to move outlets downstream such that objects of interest do not influence outlets and vice versa. In your geometry, you have a similar problem. I think there will be many recirculations just in front of your outlet that will affect the flow in the inlet. Therefore I am not convinced your approach will work for this geometry.
- Did you try to perform a simulation on a segment instead of full 360? This might help.
- Did you try to make the interface on the smallest diameter instead of the largest diameter. I would expect that to work better since the recirculations close to the outlet will be reduced.

Hi,

Give me a little time. I will prepare better out file with the mentioned points. However, I appreciate your quick reply.

have a nice day
MNMK is offline   Reply With Quote

Old   August 29, 2022, 05:29
Default
  #20
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,827
Rep Power: 27
Gert-Jan will become famous soon enough
The output file is completely clear. No need to create a better one.
The FINMES error is not helpful but CFX is to blame. This error is there already for 20 years and has never been helpful. There is not much you can do about it.
Gert-Jan 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
Boundary condition types for pressure inlet and outlet Sam Phillips OpenFOAM Running, Solving & CFD 5 February 21, 2021 12:45
Wind turbine simulation Saturn CFX 58 July 3, 2020 01:13
Can I achieve better convergence? sheaker CFX 12 September 19, 2019 15:36
Turbomachinery Mass imbalance sheaker CFX 12 September 5, 2019 08:09
Wrong flow in ratating domain problem Sanyo CFX 17 August 15, 2015 06:20


All times are GMT -4. The time now is 03:13.