[NickNosalik]

Hello all,

I currently am trying to simulate air flow within a cross-flow heat xfer system. As I am new to fluent, im having trouble getting proper results.

I cannot seem to simulate the correct pressure drop, I am modeling this simulation as follows;

Velocity inlet:
- velocity = I know this from an experiment
- temperature = I know this from an experiment

I also know the pressure at the inlet but don't understand how to "fix" the pressure at the inlet

pressure outlet:
- gauge pressure = I don't quite understand what to put here as I am looking for the pressure
- mass flow = I know this from an experiment

Pipewall:
- I have calculated the heat transfer coefficient and know the thickness


What am I missing to complete this solution? I get negative pressures all the time but temperature and velocity physically make sense, am I trying to do too much in this simulation?

[MKuhn]

You cannot not fix both, velocity and pressure, at the inlet. It will be overdetermined. You can fix the pressure at the inlet and fluent will calculate the corresponding mass flow or you fix the mass flow and fluent will calculate the pressure drop across your pipe.

[NickNosalik]

Originally Posted by MKuhn

You cannot not fix both, velocity and pressure, at the inlet. It will be overdetermined. You can fix the pressure at the inlet and fluent will calculate the corresponding mass flow or you fix the mass flow and fluent will calculate the pressure drop across your pipe.

So do I set the operating pressure at the inlet? Because I get negative pressures at the outlet for whatever reason when I do not put any pressure anywhere

[MKuhn]

For example: Leave the operating pressure at 101325 Pa (Tab operating conditions). Choose Pressure Inlet as Boundary type and set the gauge pressure close to the inlet pressure like in your experiment. Choose 0 Pa Gauge Pressure at your pressure outlet, that means the pipe is open (atmospheric pressure). In this setup Fluent will calculate the corrosponding mass flow.
Gauge Pressure Inlet minus Gauge Pressure Outlet should be the pressure drop in your experiment.

[NickNosalik]

Originally Posted by MKuhn

For example: Leave the operating pressure at 101325 Pa (Tab operating conditions). Choose Pressure Inlet as Boundary type and set the gauge pressure close to the inlet pressure like in your experiment. Choose 0 Pa Gauge Pressure at your pressure outlet, that means the pipe is open (atmospheric pressure). In this setup Fluent will calculate the corrosponding mass flow.
Gauge Pressure Inlet minus Gauge Pressure Outlet should be the pressure drop in your experiment.

Thank you for your response, things have changed since my initial post and I am supplying a certain mass flow at the inlet and know the inlet pressure, I want to view the outlet pressure and corresponding heat transfer through the walls.

Does this sound like a feasible set up? the pipe is not exiting to the atmosphere and I know the outlet pressure should be in a range of 100-300 psi but do not understand how to get these parameters at once.

Sorry for the long winded response, thank you for your help!

[MKuhn]

Choose mass-flow-inlet for your inlet boundary. Leave the value Supersonic/Inital Gauge Pressure by 0. You don't need it for normal flows.
Choose pressure outlet for your outlet and set the Gauge Pressure to 100 psi.

Run the calculation and check in your results the value for the pressure at your inlet. You can not set massflow and two pressures at in- and outlet at once, as the pressure at the inlet is a result of your calculation, if you fix a massflow. If you have a really good model it will match with the data of your experiment, otherwise not. Or your pressure measurement in your experiment is not precise enough.

[MKuhn]

You can also fix the pressure at the inlet with a pressure inlet. Then use also pressure outlet and set the target mass flow rate to your desired mass flow. In this case fluent will calculate the pressure at your outlet to match your mass flow. Maybe this is the best in your case, because then you will have different outlet pressures for the same massflow depending on your other conditions.

[NickNosalik]

Originally Posted by MKuhn

You can also fix the pressure at the inlet with a pressure inlet. Then use also pressure outlet and set the target mass flow rate to your desired mass flow. In this case fluent will calculate the pressure at your outlet to match your mass flow. Maybe this is the best in your case, because then you will have different outlet pressures for the same massflow depending on your other conditions.

I have ran this test and I have reversed flow on the inlet and the outlet, is there something obvious I could be doing wrong?

[MKuhn]

Reversed flow is not an error, I means that your flow is disturbed at the boundaries, because of swirls or something else. Check

• On how many cells of your boundary you have reversed flow
• If this number is still decreasing with the number of iterations, go further with the solver
• Check if the pressure at the outlet is in the predicted range of your pressure outlet (using the target mass flow option), if not extend the range.
• Check the mass balance between your in- and outlet via Report --> Fluxes it should be near zero. Check also the energy balance.
• If the solution converges anyway and the points above are ok, than you can ignore the reversed flow

To reach a non-disturbed flow, you can extend the pipes at your in- and outlet.

[NickNosalik]

Originally Posted by MKuhn

Reversed flow is not an error, I means that your flow is disturbed at the boundaries, because of swirls or something else. Check

• On how many cells of your boundary you have reversed flow
• If this number is still decreasing with the number of iterations, go further with the solver
• Check if the pressure at the outlet is in the predicted range of your pressure outlet (using the target mass flow option), if not extend the range.
• Check the mass balance between your in- and outlet via Report --> Fluxes it should be near zero. Check also the energy balance.
• If the solution converges anyway and the points above are ok, than you can ignore the reversed flow

To reach a non-disturbed flow, you can extend the pipes at your in- and outlet.

You have been a great help, thank you very much. One question I have is how importance is complete convergence? I have set my residuals to 1e-5 and I am getting flat lined residuals around 1e-3. If my data at the end of the solution is decent can I accept it as true?

This may be an abstract questions but I am just curious based on your knowledge of CFD. Thank you Moritz!

[MKuhn]

Convergance is one issue and could be influenced by reversed flow. In your case, if your results are closed to your experiments and the mass and energy balance are correct, your solution is fine. It depends what you want, which resolution, which accuracy.