Altair RISE

A program to recognize and reward our most engaged community members

Nominate Yourself Now!

Air Ideal Gas Flow. type

I'm modeling natural convection of Electric motor with temperature difference around 100K. My model doesn't have inlet and outlet. There is a box of air Volume around it.

Should I specify air's density as ideal gas and if so should I activate mildly incompressible flow? Please help.

NaturalConvection.inp

Find more posts tagged with

English

HyperMesh CFD

v2022

Accepted answers

All comments

acupro

These kinds of NC flows within a closed chamber are inherently unstable, transient flows. I typically recommend a geometry like below:

You would have a low velocity inlet at the bottom - like 0.1 or 0.01 m/s - with the far/room temperature, and an outlet at the top. This assumes gravity is down in that image. The other boundaries of that chamber can be slip. You should be fine with Boussinesq density rather than Ideal gas, as there will be very little effect of pressure - no high-speed flow.

If you do decide to go with the enclosed chamber, you would still probably just use Boussinesq, but most likely it's a transient flow. You would still use standard N-S flow, even if you decide to use Ideal Gas density. Mildly compressible would be for transonic flows, without shock formation.

Jagan

i got negative temperature for using ideal gas in enclosed chamber and acusolve stopped.

I have used Boussinesq approximation previously but its only valid where density difference is negligible but its not the case here. So should I proceed with thermal flow activated, Ideal gas density and small velocity inlet?

And Instead of small velocity inlet is it possible to use stagnation pressure inlet?

Thank you.

acupro

i got negative temperature for using ideal gas in enclosed chamber and acusolve stopped.

I have used Boussinesq approximation previously but its only valid where density difference is negligible but its not the case here. So should I proceed with thermal flow activated, Ideal gas density and small velocity inlet?

And Instead of small velocity inlet is it possible to use stagnation pressure inlet?

Thank you.

Yes - there is some limit to the temperature difference (or density variation) where the Boussinesq approximation may be less than valid.

For the enclosed chamber, you need to make sure the initial conditions make sense physically. I would typically run that with absolute pressure offset 0, initial pressure to 101325, zero velocity, and room temperature. Probably need to run transient, too.

You could try with small velocity or stagnation pressure. If you use stagnation pressure, you may want to set the cross-direction velocity components to zero.

Jagan

Thank you

Could you please explain the significance of keeping absolute pressure offset 0 and initial pressure to 1atm.

And steady state is not recommended even with inlet and outlet model?

and lastly what if I feed density wrt temperature data without disturbing pressure?

acupro

Thank you

Could you please explain the significance of keeping absolute pressure offset 0 and initial pressure to 1atm.

And steady state is not recommended even with inlet and outlet model?

and lastly what if I feed density wrt temperature data without disturbing pressure?

When density is dependent on absolute pressure, you need to make sure all pressures are absolute. One way is to leave absolute pressure offset as zero, then use absolute pressure values everywhere. The other way is to give a non-zero absolute pressure offset, then all pressures are relative to that offset value.

With inlet and outlet, in many cases steady would be possible. It depends on the actual case - but more likely to have a steady state solution than with a closed domain.

You could also use piecewise linear density as a function of temperature - but there's probably not much benefit of that versus ideal gas.

Jagan

When density is dependent on absolute pressure, you need to make sure all pressures are absolute. One way is to leave absolute pressure offset as zero, then use absolute pressure values everywhere. The other way is to give a non-zero absolute pressure offset, then all pressures are relative to that offset value.

With inlet and outlet, in many cases steady would be possible. It depends on the actual case - but more likely to have a steady state solution than with a closed domain.

You could also use piecewise linear density as a function of temperature - but there's probably not much benefit of that versus ideal gas.

I'm solving Steady State with a inlet velocity of 0.1m/s and I'm getting a "WARNING: inflow at outflow boundary: Outlet (mass/time: in=-8.018705e-03, out=1.250770e-01)".

I have attached my input file for reference, please let me know what could be the reason for this. Thank you.

NaturalConvection.inp

acupro

I'm solving Steady State with a inlet velocity of 0.1m/s and I'm getting a "WARNING: inflow at outflow boundary: Outlet (mass/time: in=-8.018705e-03, out=1.250770e-01)".

I have attached my input file for reference, please let me know what could be the reason for this. Thank you.

Have you also added the contraction to the outlet to your domain? Depending on the velocity produced from the NC flow, that eventual outlet may need to be fairly small. The large area inlet with small velocity plus the small area outlet helps to keep that balanced without reverse flow at the outlet. Otherwise, to keep conservation, additional flow will need to be introduced - and that is through the outlet.

Jagan

Have you also added the contraction to the outlet to your domain? Depending on the velocity produced from the NC flow, that eventual outlet may need to be fairly small. The large area inlet with small velocity plus the small area outlet helps to keep that balanced without reverse flow at the outlet. Otherwise, to keep conservation, additional flow will need to be introduced - and that is through the outlet.

hello, I have modeled this based on your instructions and these are my results. kindly seeking your opinion about this.

Thank you.

pnc.1.Log

pnc.inp

acupro

hello, I have modeled this based on your instructions and these are my results. kindly seeking your opinion about this.

Thank you.

I see you've reduced the convergence tolerance from 1.e-3 to 1.e-4. With the default 1.e-3, the simulation would have stopped after time step 78. There is still some small percentage of change in the temperature solutions in the images. You'll have to decide if that difference is worth the extra runtime.

It seems the model has converged nicely.

Ovando_RBB

Hi there,

I just saw another post similar to this one and below was my feedback:

While analyzing oil cooled electrical transformers it has worked for me to define as walls all the boundaries around the assembly where the buoyancy takes effect. For this approach you need to make sure that you use the Boussinesq approximation (variable mass density with temperature, gravitational effects activated).

You also will need to create a volume of air whose height is at least 5 to 10 times longer than the outer diameter of the motor to properly capture the plume of the free convection.

Hope this kind of combination helps!