[jins9158]

I simulated a double suction fan analysis and reviewed the results.

I wanted to know the discharge rate from a double suction fan, and then I found a problem.

I applied 80CMH flow at the outlet as an analysis condition, and applied a total pressure of 0pa as an inlet condition.

According to the law of conservation of mass, the flow rate at the inlet and outlet is the same at 80 cmh, but the flow rate discharged from the fan interface is 90 cmh, which is a strange result.

Before that, I reviewed the following situations and judged that convergence was achieved, but it is a bit confusing..

When interpreting, I identified the following situations:

1. residual 10^-3 level
2. Inlet and outlet pressure monitoring
3. Imbalance less than 1%

I seem to have applied the timescale(10^-5 level) to an appropriate level, can I get some advice on what the problem is?

I attached output file and some image

[jins9158]

Originally Posted by WilliamWilliams90

Begin with the time step obtained from the total residence time across all domains. However, this is only a beginning point; if it is readily converging, raise it; if it is difficult to converge, lower it. Let's give this a try and let's see how that goes.

Thank you for replying my question

I already tried it. I controlled auto time scale between 1 ~ 0.001.

I think that the data error seems to have occurred between the interface faces.

[ghorrocks]

Auto time scale does not calculate fluid residence time. It is usually a lot smaller than that. So you will probably find the fluid residence time will lead to a much larger time step size.

I have checked your output file and your imbalances are fine. So the global conservation is OK - your mismatch between the inlet and outlet flow rates is likely to be caused by you calculating it inaccurately.

I note that the simulation has poorly converged residuals and it seems to have been doing this for a long time. This FAQ discusses what to do about it: https://www.cfd-online.com/Wiki/Ansy...gence_criteria

[Gert-Jan]

1) make sure you evaluate on Total Pressure, not on Pressure

2) The flow is probably not nicely aligned with the interface. This might lead to wrong results. Solely look to inlet and outlet, or at components normal to your interface, if possible.

[Opaque]

I cannot figure out what interface you are referring to since you are not referencing names in your output file.

However, when comparing mass flow across an interface be extremely careful with you are doing so on a frame change interface (rotor-stator / stator-rotor) with a reduced model. You must account for the pitch change across the interface. Since you are using periodic, I can easily assume the pitch ratio may not be 1.

Mass Flow Side 1 = Mass Flow Side * (or / ) Pitch ratio

depending on how you define your pitch ratio.

[jins9158]

Originally Posted by ghorrocks

Auto time scale does not calculate fluid residence time. It is usually a lot smaller than that. So you will probably find the fluid residence time will lead to a much larger time step size.

I have checked your output file and your imbalances are fine. So the global conservation is OK - your mismatch between the inlet and outlet flow rates is likely to be caused by you calculating it inaccurately.

I note that the simulation has poorly converged residuals and it seems to have been doing this for a long time. This FAQ discusses what to do about it: https://www.cfd-online.com/Wiki/Ansy...gence_criteria

Thank you for relying my question.

your advice is good for me much

you said that "your mismatch between the inlet and outlet flow rates is likely to be caused by you calculating it inaccurately."

I think you misunderstand

inlet and outlet mass is same, but interface mass is not same (reference 1 image)

Mass flow of all location is same excep for interface about stationary domain and rotationary domain.

So I don't quite uderstand. Although mass flow of inlet & outlet is same, interface is not same.

Could I need to simulate unsteady condition?

My computer resource is not good and I don't have time, so I want to simulate steady condition including periodic condition.

[jins9158]

Originally Posted by Gert-Jan

1) make sure you evaluate on Total Pressure, not on Pressure

2) The flow is probably not nicely aligned with the interface. This might lead to wrong results. Solely look to inlet and outlet, or at components normal to your interface, if possible.

Thank you for relying my quesiton

Do you mean that the mesh is not good between face of interface about connection face?

When I made mesh, I made same size about interface.

[jins9158]

Originally Posted by Opaque

I cannot figure out what interface you are referring to since you are not referencing names in your output file.

However, when comparing mass flow across an interface be extremely careful with you are doing so on a frame change interface (rotor-stator / stator-rotor) with a reduced model. You must account for the pitch change across the interface. Since you are using periodic, I can easily assume the pitch ratio may not be 1.

Mass Flow Side 1 = Mass Flow Side * (or / ) Pitch ratio

depending on how you define your pitch ratio.

Thank you for replying my question

The number of impeller's wing is 46. so I set up '7.82609 degree' about pitch angle(360/46 = 7.82609). So, I think that picth change is not bad.

[Opaque]

Originally Posted by jins9158

Thank you for replying my question

The number of impeller's wing is 46. so I set up '7.82609 degree' about pitch angle(360/46 = 7.82609). So, I think that pitch change is not bad.

If you have pitch change, you have to scale the mass flow when crossing the interfaces.

The discretization only guarantees that

Mass Flow on 360[deg] of Side 1 = Mass Flow on 360[deg] of Side 2

MassFlow_Side1_sector = MassFlow_360 / No sector Side 1
MassFlow_Side2_sector = MassFlow_360 / No sector Side 2

MassFlow_Side2_sector          No of sectors Side1
---------------------- =  ----------------------------
MassFlow_Side1_sector          No of sectors Side2

If the number of sectors is the same, the mass flow on both sides would be identical.

[ghorrocks]

Opaque has explained why your flow rate at the interface is not matching the inlet or outlet flow.

Could I need to simulate unsteady condition?

Possibly. Work through the issues listed on the FAQ I linked to to see if you can run it steady state before trying a transient simulation. But if those things do not work you will need to run it transient.

[jins9158]

Originally Posted by Opaque

If you have pitch change, you have to scale the mass flow when crossing the interfaces.

The discretization only guarantees that

Mass Flow on 360[deg] of Side 1 = Mass Flow on 360[deg] of Side 2

MassFlow_Side1_sector = MassFlow_360 / No sector Side 1
MassFlow_Side2_sector = MassFlow_360 / No sector Side 2

MassFlow_Side2_sector          No of sectors Side1
---------------------- =  ----------------------------
MassFlow_Side1_sector          No of sectors Side2

If the number of sectors is the same, the mass flow on both sides would be identical.

Thank you for relpying my question~

I am sorry to bother you, but I don't understand your advice well.

I think we misunderstand each other. So I attached some images.

I am very pleasure to get me advice to you

I am very thank you and I hope to get advice again.

image3.jpg
image of Rotating domain

image4.jpg
image of interface (R1,R2 to S)

image5.jpg
image of interface (R2 to S)

image5.jpg
image of interface (R1 to R2, Periodic)

[jins9158]

Originally Posted by ghorrocks

Opaque has explained why your flow rate at the interface is not matching the inlet or outlet flow.



Possibly. Work through the issues listed on the FAQ I linked to to see if you can run it steady state before trying a transient simulation. But if those things do not work you will need to run it transient.

Thank you for your concern.

I am scheduled to review your advice.

Again, thank you so much.