[Jessica@123]

Hey folks, I'm doing a 2D CFD simulation of a bell nozzle using Fluent and comparing my results with RPA outputs. I've triple-checked all the thermodynamic and flow properties from RPA — things like Cp, density, Mach number, pressures at throat and exit — and I’m trying to match them in Fluent.

I tested three boundary condition setups and got really weird results:

🔹 Case 1:

Operating Pressure (OP) = 0

Inlet and outlet set directly from RPA absolute values
→ This gives me the worst match to RPA (exit pressure error > 80%)

🔹 Case 2:

OP = 101325 Pa

Inlet and outlet adjusted by subtracting OP (i.e., using gauge values)
→ Result is better than Case 1, but still not great.

🔹 Case 3 (the “wrong” one):

OP = 101325 Pa

I directly entered RPA absolute pressures into the gauge pressure fields, without adjusting them
→ This gives me the best match — exit pressure and Mach number are nearly identical to RPA.

Now here's the thing: Case 3 is technically incorrect, right? Fluent expects gauge pressures if OP ≠ 0. So I should be subtracting 1 atm from RPA absolute values — but oddly enough, not doing that gives me the most accurate results.

I’ve checked everything: mesh, solver settings, turbulence model, initialization, all looks good. The only thing I’m changing is these pressure inputs and OP settings — and it totally changes the outcome.

Has anyone else experienced this?
Is there some known quirk in Fluent’s pressure solver when handling compressible flows with different OP values?
Should I just go with Case 3 even if it’s not theoretically correct?

Would love to hear what others have done in RPA-to-CFD nozzle validation. 🙏

[lolno]

Can you share your whole sim setting in fluent?

IMG_2216.jpg

[Jessica@123]

Here are my simulation settings:

Solver type: Pressure-based (steady)

Material: Species transport without chemical reactions

Density: Ideal gas

Cp model: NASA 9 polynomial

Viscosity: Inviscid

Pressure inlet species fractions: Mass fractions from RPA (sum to 1)

Initialization: Hybrid initialization with FMG initialization turned on

Iterations: 1000

Boundary conditions:

Inlet and outlet pressures set as described in my original post (depending on the case)

Everything else is kept as default in Fluent

Now, here’s the strange part:

Even though Case 1 (where Operating Pressure = 0 and I use RPA’s absolute values directly) matches RPA perfectly at the throat, it gives a ~90% discrepancy in exit pressure and about 15% error in exit density. These values are taken using surface integrals with area-weighted averages at the exit plane.

So far, I can't pinpoint why Case 1 — which should theoretically be correct — behaves this way, while the "less correct" Case 3 performs better.

[Jessica@123]

Originally Posted by lolno

Can you share your whole sim setting in fluent?

Attachment 103328

@lolno Here are my simulation settings:

Solver type: Pressure-based (steady)

Material: Species transport without chemical reactions

Density: Ideal gas

Cp model: NASA 9 polynomial

Viscosity: Inviscid

Pressure inlet species fractions: Mass fractions from RPA (sum to 1)

Initialization: Hybrid initialization with FMG initialization turned on

Iterations: 1000

Boundary conditions:

Inlet and outlet pressures set as described in my original post (depending on the case)

Everything else is kept as default in Fluent

Now, here’s the strange part:

Even though Case 1 (where Operating Pressure = 0 and I use RPA’s absolute values directly) matches RPA perfectly at the throat, it gives a ~90% discrepancy in exit pressure and about 15% error in exit density. These values are taken using surface integrals with area-weighted averages at the exit plane.

So far, I can't pinpoint why Case 1 — which should theoretically be correct — behaves this way, while the "less correct" Case 3 performs better.

Case 1: Operating Pressure 0 Pa
Pressure Inlet Gauge Total Pressure =10 bar absolute
Pressure Outlet Gauge Pressure = 90 kPa absolute

Case 2: Operating Pressure 101325 Pa (1 atm)
Pressure Inlet Gauge Total Pressure = 1000000 Pa - 101325 = 898675 Pa
Pressure Outlet Gauge Pressure = 90000 Pa - 101325 = -11325 Pa

Case 3: Operating Pressure 101325 Pa
Pressure Inlet Gauge Total Pressure = 1000000 Pa (same as absolute)
Pressure Outlet Gauge Pressure = 90000 Pa (same as absolute)

[Jessica@123]

Originally Posted by lolno

Can you share your whole sim setting in fluent?

Attachment 103328

@lolno Case 1: Operating Pressure 0 Pa
Pressure Inlet Gauge Total Pressure =10 bar absolute
Pressure Outlet Gauge Pressure = 90 kPa absolute

Case 2: Operating Pressure 101325 Pa (1 atm)
Pressure Inlet Gauge Total Pressure = 1000000 Pa - 101325 = 898675 Pa
Pressure Outlet Gauge Pressure = 90000 Pa - 101325 = -11325 Pa

Case 3: Operating Pressure 101325 Pa
Pressure Inlet Gauge Total Pressure = 1000000 Pa (same as absolute)
Pressure Outlet Gauge Pressure = 90000 Pa (same as absolute)

[lolno]

sorry, i'm having hard time visualizing your simulation setup. Could you just screenshot the modified list setting and post the screenshot here along with pic of your domain? when you doing analysis in RPA, were there any combustion process in the nozzle?did you exclude that process in the fluent simulation?

[Jessica@123]

Originally Posted by lolno

sorry, i'm having hard time visualizing your simulation setup. Could you just screenshot the modified list setting and post the screenshot here along with pic of your domain? when you doing analysis in RPA, were there any combustion process in the nozzle?did you exclude that process in the fluent simulation?

Sorry for the confusion. Here are the system settings you requested. I just noticed that I haven't turned on the frozen equilibrium in RPA. I have also attached a screenshot of the same. In my CFD setup, I am considering the frozen flow from the inlet itself, but I don't think RPA provides that option. It only considers frozen equilibrium from the throat onward toward the nozzle exit and for the Fluent, I have turned off volumetric for any chemical reactions after inlet itself. Thank you.

[lolno]

Thanks for the additional information. Assuming the RPA simulation was done in vacuum where P_atm=0Pa, i think the appropriate boundary condition in fluent should be as per attached image. RPA only gave you the nozzle exit pressure where in your domain you set that pressure to your ambient outlet which is at different location.



Also i think it's more appropriate to use density based solver for this kind of simulation as it will solve species equation simultaneously vs pressure based solver.

density based solver
https://ansyshelp.ansys.com/public/a...ased%20density

pressure based solver
https://ansyshelp.ansys.com/public/a...ns_scheme.html

& also maybe you need to rerun RPA with frozen equilibrium nozzle flow since you aren't modeling combustion process in fluent

[Jessica@123]

Originally Posted by lolno

Thanks for the additional information. Assuming the RPA simulation was done in vacuum where P_atm=0Pa, i think the appropriate boundary condition in fluent should be as per attached image. RPA only gave you the nozzle exit pressure where in your domain you set that pressure to your ambient outlet which is at different location.



Also i think it's more appropriate to use density based solver for this kind of simulation as it will solve species equation simultaneously vs pressure based solver.

density based solver
https://ansyshelp.ansys.com/public/a...ased%20density

pressure based solver
https://ansyshelp.ansys.com/public/a...ns_scheme.html

& also maybe you need to rerun RPA with frozen equilibrium nozzle flow since you aren't modeling combustion process in fluent

This was really helpful. I have now attached the RPA inputs I provided in the standard version. I set the ambient pressure to 90 kPa and used the same value for the nozzle exit condition. Since I want an optimal nozzle design, I matched the exit condition to the ambient pressure.

[lolno]

Originally Posted by Jessica@123

This was really helpful. I have now attached the RPA inputs I provided in the standard version. I set the ambient pressure to 90 kPa and used the same value for the nozzle exit condition. Since I want an optimal nozzle design, I matched the exit condition to the ambient pressure.

So based on this, the appropriate boundary condition is as follow:

Operating pressure = 90kPa
Pressure Inlet @ nozzle inlet (gauge total pressure) = 1000kPa
Pressure outlet @ ambient outlet (gauge pressure) = 0kPa

[Jessica@123]

Originally Posted by lolno

So based on this, the appropriate boundary condition is as follow:

Operating pressure = 90kPa
Pressure Inlet @ nozzle inlet (gauge total pressure) = 1000kPa
Pressure outlet @ ambient outlet (gauge pressure) = 0kPa

This works. Based on this discussion by someone on the same topic static vs. total pressure , is Fluent assuming the gauge starts from 90 kPa (operating pressure), because of the value I provide in RPA for a nominal thrust of 1 kN at 90 kPa ambient pressure, or is it considering the nozzle exit condition of 90 kPa? Thank you for clarifying my doubts.

[lolno]

Maybe we need some clarification from RPA software. Normally in rocket propulsion analysis, the nozzle exit pressure is always referred to as static pressure, while for the nozzle inlet, total pressure definition is commonly used. It’s always important to have clear definition of which pressure definition used so it can be modeled correctly.

Fluent gauge pressure is set based on the operational pressure.

https://www.afs.enea.it/project/nept...ug/node330.htm