You are not logged in.
fvModels is a control file that provides "volume" heating of our 240 meter heating system for the Optical Plane vessel.
Here is what it looks like now. We will likely have to make changes to allow it to run with the new mesh...
cat constant/fvModels
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / Field | OpenFOAM: The Open Source CFD Toolbox |
| \\ / Operation | Version: v12 |
| \\ / And | |
| \\/ Manipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "constant";
object fvModels;
}uniformIntakeHeater
{
type semiImplicitSource;
// type bananaDoesNotExist;
active yes;select cellSet;
cellSet heaterCells;volumeMode absolute; // "absolute" = total quantity over the selected region
sources
{
e
{
explicit
{
type constant;
value 4e7;
}
implicit 0; // 40 MW total over 24,000 cells
}
}
}// Adding new JSON to implement washer to restrict throat
washerRestriction
{
type porosityForce;
active yes;porosityForceCoeffs
{
// IMPORTANT: porosityForce expects selectionMode (cellZone is typical)
selectionMode cellZone;
cellZone washerZone;type DarcyForchheimer;
DarcyForchheimerCoeffs
{
// Start “gentle”, then ramp up by decades until leakage is negligible.
// Strong resistance in x, minimal in y/z: Start 1e8 increment to 1e12
d (1e9 0 0);
f (0 0 0);// Align resistance with x-axis
coordinateSystem
{
type cartesian;
origin (0 0 0);
coordinateRotation
{
type axesRotation;
e1 (1 0 0);
e2 (0 1 0);
}
}
}
}
}
Right off the bat, I can see that we need to remove that washer section.
While we're waiting for ChatGPT5.2 to get back to me, I can toss in an explanation for the banana...
bananaDoesNotExist;
We used this to make sure the fluid solver was picking up fvModels correctly. The confirmation occurred in the form of an error message reporting that bananaDoesNotExist was not found. We saw this error message when we started the case and it hiccuped due to the incorrect name.
Looking ahead, I'm guessing we are going to have to implement cellSet in our new mesh.
That will require adding another control file, and that may be in the system folder which we have not yet addressed, other than for controlDict.
Here is ChatGPT5.2's evaluation: ( I've omitted the confirmation that the washer section needs to go. That section is removed)
One more critical check (because your new mesh is brand new)
Your heater model targets:
select cellSet;
cellSet heaterCells;That means the case will only work if heaterCells exists in the new mesh.
In your new foamWorkroom mesh created by blockMesh, you currently have only:
constant/polyMesh/{boundary,faces,neighbour,owner,points}
No sets/ directory was listed, so you almost certainly do NOT yet have heaterCells. << sets was added
How to confirm
From the case directory:
ls constant/polyMesh/sets
If that directory doesn’t exist, or there’s no heaterCells, then before running you must create it (typically via topoSet using system/topoSetDict, or by switching the model to “all cells” selection).
The two clean ways forward
Option A (recommended, preserves your proven config):
Create heaterCells for the new pipe mesh using topoSet (and any other sets you rely on, like heatedWallFaces, etc.).
This keeps your fvModels exactly compatible with what you already debugged.
The next step is to look at topoSetDict in system on the running case.
(th)
Offline
Like button can go here
ChatGPT5.2 recommended a small adjustment to the control file that configures the heating volume at run time. The new mesh is slightly thinner in Z than the extendedMerlin, so I made that adjustment and ran topoSet. Here is the log of that run:
Create time
Create polyMesh for time = 0
Reading "topoSetDict"
Time = 0s
mesh not changed.
Created faceSet ALL_heated
Clearing faceSet
faceSet ALL_heated now size 0
Read set faceSet ALL_heated with size 0
Applying source patchToFace
Adding all faces of patch heatedWall ...
Found matching patch heatedWall with 480 faces.
faceSet ALL_heated now size 480
Created faceSet HEAT_set
Clearing faceSet
faceSet HEAT_set now size 0
Read set faceSet HEAT_set with size 0
Applying source patchToFace
Adding all faces of patch wallSection ...
Found matching patch wallSection with 10 faces.
faceSet HEAT_set now size 10
Read set faceSet HEAT_set with size 10
Applying source boxToFace
Adding faces with centre within boxes 1((-240.5 -10 -10) (-0.4 10 10))
faceSet HEAT_set now size 0
Read set faceSet HEAT_set with size 0
Applying source boundaryToFace
Adding all boundary faces ...
faceSet HEAT_set now size 0
Read set faceSet ALL_heated with size 480
Applying source faceToFace
Adding all faces from faceSet HEAT_set ...
faceSet ALL_heated now size 480
Created cellSet heaterCells
Applying source boxToCell
Adding cells with center within boxes 1((-240.4 -0.2 -0.051) (-0.4 0.2 0.051))This is the revised volume heating box
cellSet heaterCells now size 9600
End
Update: ChatGPT5.2 confirmed that the topoSetDict file was cluttered with leftover configuration for convection heating. Here is what the recommended replacement looks like:
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object topoSetDict;
}actions
(
// Heater volume cellSet for fvModels (semiImplicitSource)
{
name heaterCells;
type cellSet;
action new;source boxToCell;
sourceInfo
{
box (-240.4 -0.2 -0.051) (-0.4 0.2 0.051);
inside true;
}
}
);
And here is what the revised run looks like:
Create time
Create polyMesh for time = 0
Reading "topoSetDict"
Time = 0s
mesh not changed.
Created cellSet heaterCells
Applying source boxToCell
Adding cells with center within boxes 1((-240.4 -0.2 -0.051) (-0.4 0.2 0.051))
cellSet heaterCells now size 9600
End
In our next session, we will look at four more files to be installed in the system folder.
(th)
Offline
Like button can go here
While work is proceeding in development of our new case, I restored the extendedMerlin case to "normal" by removing the washer. I then set the case to run for a second so i can be sure it is heating properly. The long term plan is to replace the Merlin engine with the new one, but that will not happen for a while. We can still run the engine with the 25 centimeter throat if kbd512 or GW Johnson need something from that version.
We have tested that version with 1 kg/s, 2 kg/s and 20 kg/s and it has worked flawlessly.
Here is the status at the end of the first second of the verification run:
ExecutionTime = 19991.43 s ClockTime = 20073 s
volFieldValue p_avg write:
volAverage(heaterCells) of p = 381899.4volFieldValue T_avg write:
volAverage(heaterCells) of T = 311.5977volFieldValue rho_mass write:
volIntegrate(heaterCells) of rho = 3.829058volFieldValue T_min_global write:
min() of T = 1.194984 at location (4.249592 -1.607025 4.607311e-18) in cell 13793volFieldValue T_max_global write:
max() of T = 338.8237 at location (-0.182823 -0.1878 3.407286e-18) in cell 3401surfaceFieldValue massFlow_in write:
sum("inlet") of phi = -1.000001surfaceFieldValue massFlow_out write:
sum("outlet") of phi = 9.772167End
The heater appears to be working properly. Mass flow in is correct as the ramp increases from 0 to 2 over 2 seconds.
Outlet looks reasonable as the system flushes the initial load of hydrogen.
(th)
Offline
Like button can go here
This post is about continuing work on the new OpenFOAM case that is intended to ultimately lead to a well designed 3 centimeter throat rocket nozzle.
As things stand, we have a new mesh in place. It contains the 240 meter heating tube, and the nozzle is missing.
We have inspected a number of control files for the case. We've eliminated some and adjusted others.
Here is the directory listing for the system folder:
ls system
blockMeshDict controlDict fvConstraints fvSchemes fvSolution thrustCalcDict topoSetDict
Of these, we've completed three: blockMeshDict, controlDict and topSetDict.
Here is the work plan ChatGPT5.2 recommends:
Suggested review order after controlDict
Please paste them in this order:
system/controlDict
system/fvSolution (stability + pressure-density coupling settings drive “will it run?”)
system/fvSchemes (div schemes, gradients, limiters — can explain oscillations and spikes)
system/fvConstraints (any leftover constraints from earlier phases)
system/thrustCalcDict (make sure it’s measuring the right patch and axis for this new mesh)
system/blockMeshDict (last, unless you suspect geometry/patch naming mismatch)
What I’ll be checking, specifically (to match your “strip it down” goal)
Since you want only volume heating of the heat pipe (cellSet heaterCells):
fvModels should contain only your semiImplicitSource for e on heaterCells
No porosity / washer / wall heat flux / convective remnants
controlDict functionObjects shouldn’t try to write wall heat fluxes, or reference sets/zones that don’t exist
fvSolution should be consistent with compressible hydrogen + your chosen solver (so the run doesn’t “work” but behave unphysically)
(th)
Offline
Like button can go here
Our review of the system folder begins with controlDict
cat system/controlDict
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 12
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2;
format ascii;
class dictionary;
location "system";
object controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
application foamRun;
libs ( "libfluid.so" "libfvModels.so" );
startFrom latestTime;
startTime 0;
stopAt endTime;
endTime 1.0;
deltaT 5e-06;
adjustTimeStep yes;
maxCo 0.7;
maxDeltaT 1e-05;
writeControl runTime;
writeInterval 0.05;
purgeWrite 0;
writeFormat binary;
writePrecision 7;
writeCompression off;
timeFormat general;
timePrecision 6;
runTimeModifiable true;
writeAndEnd no;
writeNow no;
functions
{
heatBoxStats
{
type volFieldValue;
libs ("libfieldFunctionObjects.so");
writeControl timeStep;
writeInterval 1;
log false;
selectionMode cellSet;
cellSet heaterCells;
// same box as your fvModels selection:
// box (-240.4 -0.2 -0.0630365) (-0.4 0.2 0.0630365);
operation sum;
fields ( e );
writeFields no;
}
// leave heatBoxStats as-is for sum(e)
// NEW: pressure average in heaterCells added 2025/12/19 mid-run
p_avg
{
type volFieldValue;
libs ("libfieldFunctionObjects.so");
writeControl timeStep;
writeInterval 1;
log true;
selectionMode cellSet;
cellSet heaterCells;
operation volAverage;
fields ( p );
writeFields no;
}
T_avg
{
type volFieldValue;
libs ("libfieldFunctionObjects.so");
writeControl timeStep;
writeInterval 1;
log true;
selectionMode cellSet;
cellSet heaterCells;
operation volAverage;
fields ( T );
writeFields no;
}
rho_mass
{
type volFieldValue;
libs ("libfieldFunctionObjects.so"); // sometimes already implied
enabled true;
select cellSet;
cellSet heaterCells;
operation volIntegrate;
fields (rho);
writeControl timeStep; // or runTime, same as your others
writeInterval 1; // match your existing reporting cadence
log true;
writeFields no;
}
// new reporting functions added 2025/12/26
T_min_global
{
type volFieldValue;
libs ("libfieldFunctionObjects.so");
writeControl timeStep;
writeInterval 1;
log true;
writeFields no;
select all;
operation min;
fields (T);
}
T_max_global
{
type volFieldValue;
libs ("libfieldFunctionObjects.so");
writeControl timeStep;
writeInterval 1;
log true;
writeFields no;
select all;
operation max;
fields (T);
}
massFlow_in
{
type surfaceFieldValue;
libs ( "libfieldFunctionObjects.so" );
writeControl writeTime;
regionType patch;
name inlet;
operation sum;
fields ( phi );
writeFields no;
log true;
executeControl writeTime;
}
massFlow_out
{
type surfaceFieldValue;
libs ( "libfieldFunctionObjects.so" );
writeControl writeTime;
regionType patch;
name outlet;
operation sum;
fields ( phi );
writeFields no;
log true;
executeControl writeTime;
}
CourantMax
{
type CourantNo;
writeControl writeTime;
writeInterval 1;
writeFields no;
}
}
DebugSwitches
{
fvModels 1;
semiImplicitSource 1;
}And here is the same file with tiny adjustments that ChatGPT5.2 thought appropriate.
cat system/controlDict
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 12
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2;
format ascii;
class dictionary;
location "system";
object controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
application foamRun;
libs ( "libfluid.so" "libfvModels.so" );
startFrom latestTime;
startTime 0;
stopAt endTime;
endTime 1.0;
deltaT 5e-06;
adjustTimeStep yes;
maxCo 0.7;
maxDeltaT 1e-05;
writeControl runTime;
writeInterval 0.05;
purgeWrite 0;
writeFormat binary;
writePrecision 7;
writeCompression off;
timeFormat general;
timePrecision 6;
runTimeModifiable true;
writeAndEnd no;
writeNow no;
functions
{
heatBoxStats
{
type volFieldValue;
libs ("libfieldFunctionObjects.so");
writeControl timeStep;
writeInterval 1;
log false;
selectionMode cellSet;
cellSet heaterCells;
// same box as your fvModels selection:
// box (-240.4 -0.2 -0.051) (-0.4 0.2 0.051);
operation sum;
fields ( e );
writeFields no;
}
// leave heatBoxStats as-is for sum(e)
// NEW: pressure average in heaterCells added 2025/12/19 mid-run
p_avg
{
type volFieldValue;
libs ("libfieldFunctionObjects.so");
writeControl timeStep;
writeInterval 1;
log true;
selectionMode cellSet;
cellSet heaterCells;
operation volAverage;
fields ( p );
writeFields no;
}
T_avg
{
type volFieldValue;
libs ("libfieldFunctionObjects.so");
writeControl timeStep;
writeInterval 1;
log true;
selectionMode cellSet;
cellSet heaterCells;
operation volAverage;
fields ( T );
writeFields no;
}
rho_mass
{
type volFieldValue;
libs ("libfieldFunctionObjects.so"); // sometimes already implied
enabled true;
log true;
writeFields no;
selectionMode cellSet;
cellSet heaterCells;
operation volIntegrate;
fields (rho);
writeControl timeStep; // or runTime, same as your others
writeInterval 1; // match your existing reporting cadence
}
// new reporting functions added 2025/12/26
T_min_global
{
type volFieldValue;
libs ("libfieldFunctionObjects.so");
writeControl timeStep;
writeInterval 1;
log true;
writeFields no;
select all;
operation min;
fields (T);
}
T_max_global
{
type volFieldValue;
libs ("libfieldFunctionObjects.so");
writeControl timeStep;
writeInterval 1;
log true;
writeFields no;
select all;
operation max;
fields (T);
}
massFlow_in
{
type surfaceFieldValue;
libs ( "libfieldFunctionObjects.so" );
writeControl writeTime;
regionType patch;
name inlet;
operation sum;
fields ( phi );
writeFields no;
log true;
executeControl writeTime;
}
massFlow_out
{
type surfaceFieldValue;
libs ( "libfieldFunctionObjects.so" );
writeControl writeTime;
regionType patch;
name outlet;
operation sum;
fields ( phi );
writeFields no;
log true;
executeControl writeTime;
}
CourantMax
{
type CourantNo;
writeControl writeTime;
writeInterval 1;
writeFields no;
}
}
DebugSwitches
{
fvModels 1;
semiImplicitSource 1;
}
// ************************************************************************* //The changes were primarily intended to improve consistency of format of parameters.
Functionality did not change.
(th)
Offline
Like button can go here
ChatGPT5.2 asked to look at fvSolutions and fvSchemes next ...
We reviewed both files and only added a comment line at the bottom to insure the end normally.
cat system/fvSchemes
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 12
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
class dictionary;
location "system";
object fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //ddtSchemes
{
default Euler;
}//gradSchemes
//{
// default cellLimited Gauss linear 1;
//}divSchemes
{
// // your energy variable is e; this covers e or h..
// REQUIRED by rhoPimpleFoam lookup (regex-like keys; must be quoted)
"div(phi,(p|rho))" Gauss upwind;
"div(phi,(e|h))" Gauss upwind;
"div(phid,p)" Gauss upwind; // <-- new line
div(phi,U) Gauss upwind;
div(phi,p) Gauss upwind;
div(phi,e) Gauss upwind;
div(phi,rho) Gauss upwind;
div(phi,K) Gauss upwind;
div(U) Gauss Linear;
div((muEff*dev2(T(grad(U))))) Gauss linear;
}gradSchemes
{
default cellLimited Gauss linear 0.5; // a bit more limiting
}//divSchemes
//{
// div(phi,U) Gauss vanLeer;
// div(phi,e) Gauss vanLeer;
// div(phi,K) Gauss vanLeer;
// div(U) Gauss linear;
//}laplacianSchemes
{
default Gauss linear corrected;
}interpolationSchemes
{
default linear;
}snGradSchemes
{
default corrected;
}fluxRequired
{
p;
rho;
}
// ************************************************************************* //
And Solutions...
cat system/fvSolution
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 12
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
class dictionary;
location "system";
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //solvers
{
p
{
solver PBiCGStab;
preconditioner DILU; // <-- add this line (or DIC)
tolerance 1e-8;
relTol 0.1;
}
pFinal
{
solver PBiCGStab;
preconditioner DILU; // <-- add this line (or DIC)
tolerance 1e-8;
relTol 0;
}U
{
solver smoothSolver;
smoother symGaussSeidel;
nSweeps 1;
tolerance 1e-8;
relTol 0.1;
}
UFinal
{
solver smoothSolver;
smoother symGaussSeidel;
nSweeps 1;
tolerance 1e-8;
relTol 0;
}"(T|h|rho)"
{
solver smoothSolver;
smoother symGaussSeidel;
nSweeps 1;
tolerance 1e-8;
relTol 0.1;
}
"(T|h|rho)Final"
{
solver smoothSolver;
smoother symGaussSeidel;
nSweeps 1;
tolerance 1e-8;
relTol 0;
}
e
{
solver smoothSolver;
smoother symGaussSeidel;
nSweeps 2;
tolerance 1e-8;
relTol 0.05; // stop 5%
maxIter 200;
}
eFinal
{
solver smoothSolver;
smoother symGaussSeidel;
nSweeps 2; // same as e (you can tighten to 3 later if needed)
tolerance 1e-9; // a touch tighter for the final call
relTol 0.01; // 1% of initial
maxIter 200;
}
}
relaxationFactors
{
fields { p 0.9; rho 0.9; }
equations { U 0.7; e 0.7; }
}
PIMPLE
{
nOuterCorrectors 1;
nCorrectors 2;
nNonOrthogonalCorrectors 0;transonic yes; // ok for compressible/shock cases
momentumPredictor yes;}
// ************************************************************************* //
(th)
Offline
Like button can go here
This post will be about fvConstraints ... this is where the "training wheels" reside. We got into trouble with extendedMerlin because a training wheel we installed to get the model working was still there when we were trying to run the models for real, and the result was "magic" heating we did not want or need.
The change to fvConstraints was small...
// Your existing U limiter:
limitU
{
type limitMag;
field U;
select all;
max 4000;
}// Added 2025/12/26 to prevent temperature below 0 K in expansion bell
limitT
{
type limitTemperature;selectionMode all;
// Optional: name of the energy/temperature field to constrain.
// Since your solver is "Solving for e", be explicit:
// field e;// Prevent tiny numerical undershoots below 0 K.
// Start gentle so you don't clip real expansion cooling too early:
min 0.5;
max 5000;
}
The change was to the word select. It was changed to selectionMode.
I think we may be ready to try our first run with the new case.
As a reminder, we are testing with the heat pipe ONLY! We have NO nozzle installed.
My assumption is that if we get the model working without the nozzle, then any problems that occur will be related to the nozzle.
(th)
Offline
Like button can go here
Sounds like progress.
Hopefully this might help
Calculating thrust in a Nuclear Thermal Propulsion (NTP) system—where hydrogen gas is heated by a reactor and expanded through a nozzle—requires determining the energy added to the hydrogen, the resulting mass flow rate, and the exit velocity.
Core Equations The fundamental equation for thrust (\(F\)) is:\(F=\.{m}\cdot v_{e}+(p_{e}-p_{a})A_{e}\)Where: \(\.{m}\) = mass flow rate (kg/s)\(v_{e}\) = exit velocity of exhaust (m/s)\(p_{e},p_{a}\) = exit pressure and ambient pressure (Pa)\(A_{e}\) = exit area of the nozzle (\(m^{2}\)) For a simplified estimation, if the nozzle is perfectly expanded (\(p_{e}=p_{a}\)), the formula simplifies to:\(F=\.{m}\cdot v_{e}\)
Step-by-Step Calculation Guide
1. Determine Mass Flow Rate (\(\.{m}\))You must know how much hydrogen is passing through the tube per second. If not given, this is determined by the input pressure, pipe diameter, and density.\(\.{m}=\rho \cdot A\cdot v\)(where \(\rho \) is density, \(A\) is cross-sectional area of tube, \(v\) is flow velocity)2. Calculate Exit Velocity (\(v_{e}\)) from WattageThe electrical power (wattage, \(P\)) or thermal power heats the hydrogen, converting electrical energy into kinetic energy (assuming high efficiency):\(P=\eta \cdot \frac{1}{2}\.{m}v_{e}^{2}\)Assuming an efficiency (\(\eta \)) of the system, rearranging for \(v_{e}\):\(v_{e}=\sqrt{\frac{2P}{\eta \.{m}}}\)Note: In actual NTP, power is thermal (MW) from a reactor, not just electric wattage.
3. Apply Tube Length (Thermal Efficiency & Pressure Drop) Heating (Length): Longer tubes allow higher hydrogen temperature (\(T_{exit}\)) up to material limits, increasing \(v_{e}\) and Specific Impulse (\(I_{sp}\)).Friction (Length): Longer tubes increase frictional pressure losses (\(-\Delta p\)), which can reduce exit velocity.Effect: The length must be optimized to maximize \(T_{exit}\) without excessive pressure drop. A longer tube generally increases the temperature and thus the thrust, provided the heat input continues along the length.
4. Final Thrust CalculationOnce \(v_{e}\) and \(\.{m}\) are determined, substitute them back into \(F=\.{m}\cdot v_{e}\). Key Parameters at NTP (Normal Temperature and Pressure) Propellant: Hydrogen (\(H_{2}\))Efficiency: Realistic NTP systems aim for high temperatures, often resulting in specific impulses (\(I_{sp}\)) around 800–900 seconds
Thrust Calculation (NTP) based on Power and Tube Dimensions To calculate the thrust (\(F\)) generated by a nuclear thermal propulsion (NTP) system using a hydrogen tube, you need to calculate the mass flow rate (\(\.{m}\)) based on the heating of the hydrogen (wattage) and determine the exit velocity (\(V_{e}\)) based on the tube length and operating temperature. Fundamental Equations
Thrust (F) = m_dot * V_eMass Flow Rate (m_dot) = P_in / ΔhStep-by-Step Calculation Formula Determine Exhaust Velocity (\(V_{e}\)):Assuming a simple, idealized expansion where the hydrogen is heated by a heat source:
V_e = sqrt( (2 * γ * R * T_chamber) / (γ - 1) )\(\gamma \) = Ratio of specific heats for Hydrogen (~1.4)\(R\) = Specific gas constant for Hydrogen (4124 J/kg·K)\(T_{c}\) = Chamber temperature (K)Determine Mass Flow Rate (\(\.{m}\)):
m_dot = W / (Cp * ΔT)\(W\) = Power/Wattage applied to the hydrogen (Watts)\(Cp\) = Specific heat capacity of Hydrogen (~14300 J/kg·K)\(\Delta T\) = Temperature increase of hydrogen (K)Calculate Thrust (\(F\)) in Newtons:
F = m_dot * V_eBBcode Formula for Inputting into Calculators
[b]Thrust (N)[/b] = (Watts / (14300 * ΔT)) * sqrt( (2 * 1.4 * 4124 * T_chamber) / (1.4 - 1) )Variables Definitions Wattage (\(W\)): Total power input into the hydrogen gas.Tube Length (\(L\)): Affects the residence time and heating efficiency, typically increasing \(\Delta T\) and \(T_{c}\).\(T_{c}\): Chamber temperature (K).\(\Delta T\): Temperature rise of hydrogen (K). Note: Hydrogen NTP systems typically achieve a specific impulse (Isp) of 850–1000 s. High thrust-to-weight ratios are possible compared to electric propulsion.
Offline
Like button can go here
For SpaceNut re #258
Thank you for this helpful contribution to the topic! I added it to the Index post #2.
This post is to announce the first run for the NewNozzle topic... Here is the head of the log...
head -n150 log01.NewNozzle-2kg-0-1
/*---------------------------------------------------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 12
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
Build : 12-86e126a7bc4d
Exec : foamRun -solver fluid
Date : Jan 18 2026
Time : 21:08:15 <<
Host : "tom-GA-78LMT-01"
PID : 3885495
I/O : uncollated
Case : /home/tahanson/OpenFOAM/tahanson-v2306/run/foamWorkroom
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10)
allowSystemOperations : Allowing user-supplied system call operations// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create timeCreate mesh for time = 0
Selecting solver fluid
Selecting thermodynamics package
{
type hePsiThermo;
mixture pureMixture;
transport const;
thermo eConst;
equationOfState perfectGas;
specie specie;
energy sensibleInternalEnergy;
}Selecting turbulence model type laminar
Selecting laminar stress model Stokes
No MRF models presentCourant Number mean: 0 max: 0
Creating fvModels from "constant/fvModels" <<Selecting finite volume model type semiImplicitSource
Name: uniformIntakeHeater
- selecting cells using cellSet heaterCells <<
- selected 9600 cell(s) with volume 9.6
Selecting thermophysical transport type laminar
Selecting default laminar thermophysical transport model unityLewisFourier
fluid(user): accessing fvModels <<
Creating fvConstraints from "system/fvConstraints" <<Selecting finite volume constraint type limitMag
Name: limitU
- selecting all cells
- selected 9800 cell(s) with volume 9.8 <<
Selecting finite volume constraint type limitTemperature
Name: limitT
- selecting all cells
- selected 9800 cell(s) with volume 9.8 <<PIMPLE: No convergence criteria found
PIMPLE: Operating solver in transient mode with 1 outer corrector
PIMPLE: Operating solver in PISO modeStarting time loop
- selecting cells using cellSet heaterCells <<
- selected 9600 cell(s) with volume 9.6- selecting cells using cellSet heaterCells
- selected 9600 cell(s) with volume 9.6- selecting cells using cellSet heaterCells
- selected 9600 cell(s) with volume 9.6- selecting cells using cellSet heaterCells
- selected 9600 cell(s) with volume 9.6- selecting all cells
- selected 9800 cell(s) with volume 9.8 <<- selecting all cells
- selected 9800 cell(s) with volume 9.8surfaceFieldValue massFlow_in: <<
total faces = 40
total area = 0.04surfaceFieldValue massFlow_out: <<
total faces = 40
total area = 0.04volFieldValue p_avg write:
volAverage(heaterCells) of p = 101325 <<volFieldValue T_avg write:
volAverage(heaterCells) of T = 21 <<volFieldValue rho_mass write:
volIntegrate(heaterCells) of rho = 11.23116 <<volFieldValue T_min_global write:
min() of T = 21 at location (-239.5 -0.195 0) in cell 0 <<volFieldValue T_max_global write:
max() of T = 21 at location (-239.5 -0.195 0) in cell 0 <<surfaceFieldValue massFlow_in write:
sum("inlet") of phi = 0surfaceFieldValue massFlow_out write:
sum("outlet") of phi = 0Courant Number mean: 0 max: 0
deltaT = 1.2e-06
Time = 1.2e-06sdiagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver: Solving for Ux, Initial residual = 1, Final residual = 4.041553e-15, No Iterations 1
smoothSolver: Solving for Uy, Initial residual = 1, Final residual = 3.837991e-15, No Iterations 1
Applying model uniformIntakeHeater to field e
smoothSolver: Solving for e, Initial residual = 1, Final residual = 4.420088e-11, No Iterations 2
DILUPBiCGStab: Solving for p, Initial residual = 1, Final residual = 8.6153e-12, No Iterations 1
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 1.371513e-06, global = 1.371513e-06, cumulative = 1.371513e-06
DILUPBiCGStab: Solving for p, Initial residual = 0.7210587, Final residual = 6.198841e-12, No Iterations 1
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 2.605976e-07, global = 2.605976e-07, cumulative = 1.632111e-06
ExecutionTime = 0.299823 s ClockTime = 0 s <<volFieldValue p_avg write:
volAverage(heaterCells) of p = 101326.3 <<volFieldValue T_avg write:
volAverage(heaterCells) of T = 21.00029 <<
I was astonished when the case ran the first time. ChatGPT5.2 agonized over every word in every command and configuration file. In the case of fvConstraints, it argued with itself through four iterations before it finally settled on the configuration that is in effect, and that solution turns out to be correct. I suspect that the argument arose because OpenFOAM has so many versions now, and also because ChatGPT5.2 cannot remember everything between sessions. I've seen this many times over the past year of working with ChatGPT4o and then ChatGPT5, and now this latest version. A paying customer like me is granted a small amount of "permanent" storage somewhere in the cloud, but it is obviously insufficient. On top of that, each iteration (instance) of ChatGPT has to study everything in the customer stored memory plus the latest query, and then try to make sense of the situation, and ** then ** say something useful or at least meaningful.
it is truly amazing how well ChatGPT performs given these challenges.
However, in the mean time, Gemini seems able to respond far more quickly than ChatGPT5.2 is able to do. That may be partly because I am a bottom tier customer for ChatGPT, whereas Gemini is operating at the free level, where Google may be trying to impress me with it's performance so I subscribe as a paying customer.
(th)
Offline
Like button can go here
I am happy to be able to report that the first run of the NewNozzle OpenFOAM case just ended normally.
ExecutionTime = 3274.708 s ClockTime = 3340 s << 1 second of sim time took 3340 seconds (less than 1 hour)
volFieldValue p_avg write:
volAverage(heaterCells) of p = 490282 << Pressure started at 1 bar and rose to nearly 5 with heatingvolFieldValue T_avg write:
volAverage(heaterCells) of T = 402.8296 << We are definitely seeing heating because we started at 21 KelvinvolFieldValue rho_mass write:
volIntegrate(heaterCells) of rho = 3.048076 << Mass is presumably falling from the initial loadvolFieldValue T_min_global write:
min() of T = 40.38589 at location (-239.5 -0.005 0) in cell 4560 << The minimum is higher than I expectedvolFieldValue T_max_global write:
max() of T = 440.7536 at location (-0.5 -0.195 -2.162287e-17) in cell 239 << Maximum is just ahead of the exitsurfaceFieldValue massFlow_in write:
sum("inlet") of phi = -0.9999951 << We are 1 second into the run - inlet is ramping to 2 kg/s over 2 secondssurfaceFieldValue massFlow_out write:
sum("outlet") of phi = 4.657116 << We are seeing a high value because we are flushing the initial loadEnd << A normal end on the FIRST run of the new case! Amazing!
I'll launch a continuation to 4 seconds from here. That should be enough time to have something useful to study. Plus, we will have enough data to exercise the multiple plot programs we've developed over the past 8 months.
(th)
Offline
Like button can go here
And here is ChatGPT5.2's summary of the good news of the successful run of our brand new case:
Thank you (again) for your constant assistance over the past year... we've certainly dealt with a range of problems, but you and your predecessor ChatGPT4o always won through the difficulty. We have just achieved something I could only hope for when we started. We designed a new case and it ran immediately ** and ** it finished with a normal end. I have ** just ** restarted the run to go all the way to four seconds. At that point we'll have enough data to justify stopping to generate some plots. I am ** really ** happy. Adding the nozzle should be easy compared to what we've been through.
That’s fantastic news — congratulations. ?
You’ve crossed a genuinely important milestone.What you just achieved is not “just another run”:
You built a new case from scratch (foamWorkroom),
With a clean, minimal mesh,
Using volume heating only (no legacy convective artifacts),
Correctly wired fvModels, fvConstraints, controlDict, and functionObjects,
And the solver started cleanly, marched forward, and terminated normally.
That combination is rare even for experienced OpenFOAM users. You’ve essentially reclaimed control of the model after months of inherited complexity.
A few things worth explicitly acknowledging:
Why this success matters
1. The solver behavior is textbook-correctFrom the log head you posted:
Courant starts at zero ✔️
rho, U, e, p all converge cleanly ✔️
semiImplicitSource activates correctly on heaterCells ✔️
Constraints are applied to the intended regions ✔️
No runaway deltaT, no continuity explosion ✔️
This tells us the physics, numerics, and bookkeeping are aligned — which was never guaranteed with the inherited Merlin mesh.
2. You now own the geometry–physics contract
This is the big one.
Previously:
Geometry dictated physics (and often fought it)
The “box” injected unintended reflections
The washer introduced artificial turbulence
Debugging mixed mesh artifacts with real physics
Now:
Geometry is simple and intentional
Heating is exactly where you think it is
Flow paths are unambiguous
Any oscillation you see is real physics or numerics, not legacy geometry noise
That’s the point at which engineering starts replacing forensics.
3. Adding a nozzle really will be easier
You’re absolutely right here.
Compared to:
Rehabilitating a legacy mesh
Debugging pressure BCs against a “box”
Reconciling solver expectations with half-dead dictionaries
Chasing instabilities caused by geometry you didn’t design
…adding a nozzle is now a controlled geometry refinement problem:
Same patches
Same BCs
Same fvModels
Same diagnostics
Same plotting pipeline
You already proved that swapping meshes without touching physics works. That’s the hardest conceptual step — and you’ve done it.
What I’d suggest while the 4 s run proceeds
No action required right now, but mentally queue these:
Baseline plots
When you stop at 4 s:p_avg, T_avg, rho_mass
massFlow_in vs massFlow_out
thrust vs time
This becomes your gold reference for:
“Straight heated pipe, no nozzle”
Watch for absence of pathologies
In particular:No 7 Hz pulsing
No deltaT spikes
No T_max excursions to nonsense values
Quiet plots are a success, not a failure.
Freeze this case
Make a read-only archive copy once plots are generated.
This becomes:foamWorkroom_pipe_baseline
Every future nozzle experiment will be compared to this.
A personal note
You weren’t exaggerating earlier: this has been an eight-month engineering recovery effort, not a casual CFD exercise. The persistence it took to:
Question the inherited model,
Accept partial success without stopping,
Build tooling (logs → CSV → plots),
And then decide to start over cleanly —
…that’s exactly how real aerospace modeling work progresses.
You earned the right to be really happy about this result.
When the 4-second run finishes and you’re ready to look at plots — or when you want to sketch the nozzle insertion strategy — I’ll be here.
(th)
Offline
Like button can go here
The run of NewNozzle is under way to 4 seconds. Here is a snapshot of the run in progress:
ExecutionTime = 2311.764 s ClockTime = 2320 s << less than one hour
volFieldValue p_avg write:
volAverage(heaterCells) of p = 625723.5 << We are still flushing initial load so six barvolFieldValue T_avg write:
volAverage(heaterCells) of T = 1459.301 << Heating is happening in a smaller volume 9600 vs 24000volFieldValue rho_mass write:
volIntegrate(heaterCells) of rho = 2.155162 << flush is proceeding nicely while we ramp up to 2 kg/svolFieldValue T_min_global write:
min() of T = 28.56966 at location (-239.5 -0.005 0) in cell 4560 << Minimum is starting to fall toward intake of 21 KelvinvolFieldValue T_max_global write:
max() of T = 1748.856 at location (-0.5 -0.195 -2.162287e-17) in cell 239 << Maximum is just ahead of exitCourant Number mean: 0.001769359 max: 0.003112839 << I've not seen Courant this low .. the equations are loafing
deltaT = 1e-05
Time = 1.80177s
That low Courant number is because we have no nozzle to impede gas flow.
(th)
Offline
Like button can go here