Altair RISE

A program to recognize and reward our most engaged community members

Nominate Yourself Now!

Acusolve query

Rahul Rajan_21763

Hi everybody.

I made some attempts on Acuconsole but I obtained wrong numerical results.

The steps I followed were as follow:

- Flow Model: STEADY STATE - THREE DIMENSIONAL - TURBOLENCE (spalart allmaras)

- Incompressible fluid

- thermophysical properties costant

Essentially, sarting from impeller angular velocity and inlet pressure, I'd like to obtain pressure and velocity distributions.

At first I defined the angular velocity in 'Reference Frame' (I assigned rotation center and angular velocity (about 2500 rpm)).

In Acuconsole I assigned the following values:

- As volume I assigned the fluid volume (material:Water, Body Force:None, Reference Frame: angular velocity.

- For the surfaces, after assigning 'simple BC type' for each surface, I assigned:

- Pressure (about 400000 N/m^2) for inlet; a value of eddy viscosity;

- No BC for outflow (I'd like to obtain the outlet pressure!);

- Angular Velocity for wall;

- No BC for wall_2.

Even if the anlysis converges (after several time steps), and even if the velocity distribution seems to be reasonable, the numerical results are completely wrong.

Since I couldn't find neither tutorials, nor videos, nor any other material, my last chance was to ask for your help. I also made the blower workshop with which I was able to understand some issues about Acuconsole.

At last I attach the .hm file and the .acs files.

I really hope you can help me. At least tell me if I'm completely wrong.

Please answer.

Best Regards

Stefano

Unable to find an attachment - read this blog

Find more posts tagged with

AcuSolve

English

Accepted answers

All comments

acupro

Generally you don't just have an impeller sitting in free space, but rather enclosed in some sort of housing, as in the attached picture. Then you'll have a single inlet and a single outlet. As in the tutorial to which you referred, you'll need to create separate volumes so you can assign the reference frame appropriately to the volume near the impeller. You may be better off working with your local HyperWorks support team on this.

<?xml version="1.0" encoding="UTF-8"?>

Altair Forum User

Hi Acupro

Thanks for your reply. Of course I know that usually this kind of CFD analysis is made on a complete stage of the submersible pump (in my case). But I'm only interested in the flow through the rotor. Before starting with attempts I searched material in literature and I found some articles about this kind of analysis.

Furthermore it seems that the situation is not too far from the blower example.

Regards

acupro

If you want to make another attempt, try this.

Inlet: Use inflow type = stagnation_pressure with stagnation_pressure = 0.0. And define the eddy-viscosity to something small, like 1.e-5.

Outlet: Separate each boundary into its own set, and use Simple BC type = outflow, with pressure = 0.0. So you'll have several sets (outlet1, outlet2, etc) all with the same boundary condition.

This may work, but I won't guarantee it. This will give you the mass-flow developed through the device, plus the resultant static pressure difference.

You may also want to cut the geometry/mesh so the volume above the impeller (attached to the inlet) doesn't have the reference frame applied to it. (In this case you would have two Volume sets - one with the reference frame and the other without.

Altair Forum User

Hi acupro

I tried with your hint but it doesn't seem to work: the mass-flow doesn't conserve while the fluid is incompressible.

Anyway I have the mass-flow (I found the datasheet of the pump) and I know the inlet pressure. So I assigned the inlet pressure and the mass-flow at the outlet (by integrated BC).

Then I assigned the reference frame both to fluid and rotating wall.

I obtained some results but I can't say if they are correct.

Furthermore I can't understand if the rotation direction is right: I used the right hand rule, so I defined a positive velocity, but I'm not completely sure.

Regards

acupro

If you have the mass-flow, you'll be better off using the inflow type as mass-flux (really mass flow rate - kg/sec) and using pressure outlet. But still you should separate each outlet into its own set, rather than have all in one. Your simulation results will include the inlet pressure and outlet pressure - from which you can compute the pressure difference. It won't matter that the actual value of the pressure at the inlet is different from your known pressure - the pressure difference will be correct for that given mass flow rate.

However - with as coarse as the mesh is/was, I would not expect very good accuracy.

Also, I can't picture how this device would actually be built. I can see what would likely represent the blades - with the reference frame applied to the surfaces of the blades. But the boundaries between the blades also have the reference frame applied. Are there actual walls between the blades that spin with the blades?

You may be better off interacting with your local HyperWorks support team in Italy.

Altair Forum User

Hi acupro

Thanks for your reply.

The mesh I attached was the first I made. Now the mesh is better.

The impeller is the rotating component of a submersible pump stage, so all the surfaces are rotating walls. I attach an image of the stage.

Regards

<?xml version="1.0" encoding="UTF-8"?>