[DKY2Y]

Originally Posted by Christophe

Also, 24 total seconds, may take a very very long time to solve. Especially when using a proper time step for transient turbo machinery. These settings are probably appropriate for something rotating at 100 rpm.

I have written the following details for my transient simulation:
Total Time=10s
Time steps=0.001 s
Initial time=0 s

Output control
Backup:
Time step=100

Transient Results:
Time step interval=10

Does the Solution for the transient simulation look right so far as seen from the attached pictures?

[ghorrocks]

Please do not PM me with duplicates of posts you have made on the forum. If it is on the forum I will see it.

Is this a steady state or transient simulation?

This does not look converged adequately.

[DKY2Y]

Originally Posted by ghorrocks

Please do not PM me with duplicates of posts you have made on the forum. If it is on the forum I will see it.

Is this a steady state or transient simulation?

This does not look converged adequately.

Yeah it is a transient simulation however the simulation has not converged yet. It has been running for the past 24 hours.

The youtube video which I was watching used a transient simulation of an impeller and volute excluding cavitation. However I used the same values of time steps as the video did.

[ghorrocks]

Before you do any simulation you need to do some basic validation and verification first. The most important bit of this is to determine what mesh, time step and convergence criteria is required for your simulation.

The time step size is simplified by using adaptive time steps, homing in of 3-5 coeff loops per iteration. Then the solver will find its own time step size.

But you should do a sensitivity analysis on mesh size and convergence criteria first, so you know what settings you need for the accuracy you require.

[DKY2Y]

Originally Posted by ghorrocks

Before you do any simulation you need to do some basic validation and verification first. The most important bit of this is to determine what mesh, time step and convergence criteria is required for your simulation.

The time step size is simplified by using adaptive time steps, homing in of 3-5 coeff loops per iteration. Then the solver will find its own time step size.

But you should do a sensitivity analysis on mesh size and convergence criteria first, so you know what settings you need for the accuracy you require.

Thank you, the transient simulation worked. Does the result look alright for now? My project supervisor asked me to increase decrease the time step to enhance the convergence. I will repeat it again to get a better result.

It should be noted that the output normal force is high mainly due to the centrifugal pump which has high volume flow rate and output discharge pressure.

[ghorrocks]

I have no idea what you are looking for so cannot say if those results are OK. The main thing you do to check a simulation is OK is:
* validate against a benchmark result or experiment results.
* Do sensitivity analyses of mesh size, convergence criteria and time step size to check they are OK
* Other considerations are listed in the FAQ.

[DKY2Y]

Originally Posted by ghorrocks

I have no idea what you are looking for so cannot say if those results are OK. The main thing you do to check a simulation is OK is:
* validate against a benchmark result or experiment results.
* Do sensitivity analyses of mesh size, convergence criteria and time step size to check they are OK
* Other considerations are listed in the FAQ.

Hi, thank you for assistance. I have a question regarding writing an expression on CFX Pre. This is for NPSHA. The journal article I am using defines NPSHA as :
NPSHA= Pinlet - (Pv/ Density *g)

The vapor pressure is 3170 Pa at 25 degrees. I have written the following expression if you could check if it is correct as I am not too sure if I should input my vapour pressure as Pa or another unit within the expression:
massFlowAve(Total Pressure in Stn Frame )@ R1 Inlet-(3170/(1000*9.81))

[ghorrocks]

I would recommend:

areaAve(p)@ R1 Inlet-(3170[Pa]/(areaAve(Density)@ R1 Inlet*g))

You should use static pressure, not total pressure; you should get density from the simulation rather than hard coding it; might as well use the internal variable "g" for gravity; and you should define units for quantities with units.

[DKY2Y]

Originally Posted by ghorrocks

I would recommend:

areaAve(p)@ R1 Inlet-(3170[Pa]/(areaAve(Density)@ R1 Inlet*g))

You should use static pressure, not total pressure; you should get density from the simulation rather than hard coding it; might as well use the internal variable "g" for gravity; and you should define units for quantities with units.

Thank you. Before I start the simulation, I have used the following boundary conditions for the inlet pressure. I used 1.63 Pa static pressure with respect to 0 atm Reference Pressure. Outlet is given by mass flow rate obtained from the journal.

I obtained the value for the inlet pressure by working it out from the NPSHa formula since one of the NPSH values given in the journal article was 1.31 m. Is this a good way for obtaining the inlet pressure boundary condition in order to get 1.31 m NPSH?

[ghorrocks]

The inlet at 1.63Pa with a reference pressure of 0 atm does like an extreme vacuum to me. Does this pump operate in a vacuum environment?

Most of the time you want to set the inlet pressure to 0 [Pa] and you use the reference pressure to set the pressure level.

But I cannot answer your last question without further information: Is this a incompressible or compressible simulation? Are you modelling cavitation?

[DKY2Y]

Originally Posted by ghorrocks

The inlet at 1.63Pa with a reference pressure of 0 atm does like an extreme vacuum to me. Does this pump operate in a vacuum environment?

Most of the time you want to set the inlet pressure to 0 [Pa] and you use the reference pressure to set the pressure level.

But I cannot answer your last question without further information: Is this a incompressible or compressible simulation? Are you modelling cavitation?

The experimental setup of the pump is shown in the attached picture which indicates that it works in a vacuum environment.

I am modelling cavitation and I am assuming that it is a homogenous model.

[ghorrocks]

For your model where the pressure is very close to absolute zero anyway then using a zero reference pressure is OK.

[DKY2Y]

Originally Posted by ghorrocks

For your model where the pressure is very close to absolute zero anyway then using a zero reference pressure is OK.

Oh sorry my fault, the actual equation for the NPSH is:

NPSHA= (Pinlet - Pv)/ Density *g)

So I wrote it down the way you showed me:

(areaAve(p)@ R1 Inlet-3170[Pa])/((areaAve(Density)@ R1 Inlet*g))

Hence from calculations and from the change in formula the inlet pressure changed to 1602.1 kg/m3. Does it sound sensible to use this for my boundary condition since it increased?

[ghorrocks]

kg/m3 is the units for density. Please check your units.

And if you meant 1602 Pa then your pressure is less than the vapour pressure of your liquid. Is this what you intended? Does the fluid enter your domain already as a vapour?

[DKY2Y]

Originally Posted by ghorrocks

kg/m3 is the units for density. Please check your units.

And if you meant 1602 Pa then your pressure is less than the vapour pressure of your liquid. Is this what you intended? Does the fluid enter your domain already as a vapour?

Sorry, I meant 16021 Pa. I set up my inlet conditions as the following:
Volume fraction: Water=1 And Vapor 0. The picture shows the cavitation effect for NPSH of 1.31 m from the journal article.

[ghorrocks]

That is sounding more realistic.

[DKY2Y]

Originally Posted by ghorrocks

That is sounding more realistic.

Something does not seem right with the convergence since the NPSH monitor point is going negative at this point. It must stay steady at a value close to 1.31 m.

[ghorrocks]

What does the convergence looks like? Is it still converged?

What does the flow field look like? Have a look in CFD-Post.

[DKY2Y]

Originally Posted by ghorrocks

What does the convergence looks like? Is it still converged?

What does the flow field look like? Have a look in CFD-Post.

It has converged however the solution looks wrong as shown in the attached pictures.

I think the boundary conditions are incorrect.

[ghorrocks]

Have you read the best practices guide for cavitation modelling in the CFX documentation? That gives a lot of background in how to make cavitation models work properly.