[MNMK]

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,

[Gert-Jan]

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

[MNMK]

Originally Posted by Gert-Jan

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

[Gert-Jan]

please post the output file

[MNMK]

Originally Posted by Gert-Jan

please post the output file

I attached the output file

[Gert-Jan]

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?

[MNMK]

Originally Posted by Gert-Jan

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

[Gert-Jan]

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]

Originally Posted by Gert-Jan

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]

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]

I don`t know why I can not upload the out file.

[Gert-Jan]

And why doesn't it work? What is the problem?

[MNMK]

Originally Posted by Gert-Jan

And why doesn't it work? What is the problem?

It says Invalid file when I upload .

may I send you per Email?

[Gert-Jan]

Originally Posted by MNMK

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]

Originally Posted by MNMK

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?

[ghorrocks]

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.

[MNMK]

Originally Posted by Gert-Jan

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,

[Gert-Jan]

- 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.

[MNMK]

Originally Posted by Gert-Jan

- 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

[Gert-Jan]

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.