[funnier]

I am running transident CFD simulation of rocket. the simulation time was given 58 second but it failed in 8 second. Can anyone help me to understand the reason of faliure?

Rocket dimenssion

The length of rocket is 5.1 meter and base diameter is 559 mm.




Fuid domain

36 meter and width 41 meter, and downstream length is 20.8 meter.

CFX Boundary Condition


The geometry is 2d planner and extrude distance is 0.5.

Boundary condition is Inlet, Outlet, Fahrfield, Fluid Symmetry(both side selected as one symmetry), Rocket Symmetry(both side selected as one symmetry), Inner wall of rocket, and Interface (for both fluid and rocket).

Pressure, velocity and Temperature function is asssigned

In the expert parameter > Convergence control > Max continuity loop is set to 2.


Here is the OutFile (Whole OutFile Download)


COEFFICIENT LOOP ITERATION = 97 CPU SECONDS = 8.597E+05
----------------------------------------------------------------------
| Equation | Rate | RMS Res | Max Res | Linear Solution |
+----------------------+------+---------+---------+------------------+
| U-Mom | 0.51 | 4.1E-04 | 1.2E-01 | 2.5E-03 OK|
| V-Mom | 0.93 | 1.9E-05 | 4.3E-03 | 8.7E-02 OK|
| W-Mom | 0.00 | 0.0E+00 | 0.0E+00 | 0.0E+00 OK|
| P-Mass | 0.88 | 2.3E-04 | 7.7E-02 | 5.1 1.1E-02 OK|
+----------------------+------+---------+---------+------------------+
| H-Energy | 0.70 | 1.3E-04 | 1.4E-02 | 7.8E-04 OK|
| T-Energy | 1.08 | 2.4E-06 | 9.5E-05 | 5.9 7.8E-04 OK|
+----------------------+------+---------+---------+------------------+
| K-TurbKE | 1.09 | 9.6E-06 | 9.7E-04 | 15.4 7.9E-02 OK|
| O-TurbFreq | 1.01 | 8.1E-06 | 1.1E-03 | 10.8 6.2E-05 OK|
+----------------------+------+---------+---------+------------------+
----------------------------------------------------------------------
| Equation | Rate | RMS Res | Max Res | Linear Solution |
+----------------------+------+---------+---------+------------------+
| P-Mass | 0.37 | 8.3E-05 | 2.1E-02 | 5.1 2.5E-02 OK|
+----------------------+------+---------+---------+------------------+
----------------------------------------------------------------------
COEFFICIENT LOOP ITERATION = 98 CPU SECONDS = 8.598E+05
----------------------------------------------------------------------
| Equation | Rate | RMS Res | Max Res | Linear Solution |
+----------------------+------+---------+---------+------------------+
| U-Mom | 1.38 | 5.7E-04 | 1.5E-01 | 1.0E-02 OK|
| V-Mom | 0.55 | 1.1E-05 | 2.1E-03 | 1.4E+01 F |
| W-Mom | 0.00 | 0.0E+00 | 0.0E+00 | 0.0E+00 OK|
| P-Mass | 0.03 | 7.9E-06 | 1.6E-03 | 13.3 2.9E-01 ok|
+----------------------+------+---------+---------+------------------+
| H-Energy | 1.71 | 2.2E-04 | 4.7E-02 | 2.0E-03 OK|
| T-Energy | 4.45 | 1.1E-05 | 1.3E-03 | 5.9 2.0E-03 OK|
+----------------------+------+---------+---------+------------------+
| K-TurbKE | 2.90 | 2.8E-05 | 4.0E-03 | 10.6 4.8E-02 OK|
| O-TurbFreq | 4.88 | 3.9E-05 | 2.9E-02 | 10.8 2.3E-05 OK|
+----------------------+------+---------+---------+------------------+
----------------------------------------------------------------------
| Equation | Rate | RMS Res | Max Res | Linear Solution |
+----------------------+------+---------+---------+------------------+
| P-Mass | 0.04 | 2.8E-07 | 4.5E-05 | 9.2 1.4E+01 F |
+----------------------+------+---------+---------+------------------+
----------------------------------------------------------------------
COEFFICIENT LOOP ITERATION = 99 CPU SECONDS = 8.598E+05
----------------------------------------------------------------------
| Equation | Rate | RMS Res | Max Res | Linear Solution |
+----------------------+------+---------+---------+------------------+
| U-Mom | 0.62 | 3.5E-04 | 5.3E-02 | 1.2E-01 ok|
| V-Mom |13.64 | 1.5E-04 | 2.1E-02 | 1.8E-01 ok|
| W-Mom | 0.00 | 0.0E+00 | 0.0E+00 | 0.0E+00 OK|
| P-Mass |30.23 | 2.4E-04 | 4.3E-02 | 9.2 1.0E+00 F |
+----------------------+------+---------+---------+------------------+
+--------------------------------------------------------------------+
| ****** Notice ****** |
| The non-dimensional near wall temperature (T+) has been clipped |
| for calculation of Wall Heat Transfer Coefficient. |
| |
| Boundary Condition : FluidSolid Side 2 |
| T+ clip value = 1.0000E-10 |
| |
| If this situation persists and you are using the High Speed Model, |
| consider enabling Mach number based blending between low speed and |
| high speed wall functions. You can do so by specifying a Mach |
| number threshold as follows: |
| |
| EXPERT PARAMETERS: |
| highspeed wf mach threshold = 0.1 # default=0.0 (off) |
| END |
+--------------------------------------------------------------------+
| H-Energy | 6.63 | 1.5E-03 | 6.0E-01 | 9.9E-02 OK|
| T-Energy |99.99 | 7.7E-03 | 9.6E-01 | 5.9 9.9E-02 OK|
+----------------------+------+---------+---------+------------------+
| K-TurbKE |50.37 | 1.4E-03 | 2.6E-01 | 5.8 1.4E-05 OK|
| O-TurbFreq |70.02 | 2.8E-03 | 6.9E-01 | 10.8 1.5E-09 OK|
+----------------------+------+---------+---------+------------------+

Parallel run: Received message from follower
--------------------------------------------
Follower partition: 2
Follower routine : get_TWFTFC
Leader location : End of Continuity Loop
Message label : 009100015
Message follows below - :
+--------------------------------------------------------------------+
| ****** Notice ****** |
| The non-dimensional near wall temperature (T+) has been clipped |
| for calculation of Wall Heat Transfer Coefficient. |
| |
| Boundary Condition : FluidSolid Side 2 |
| T+ clip value = 1.0000E-10 |
| |
| If this situation persists and you are using the High Speed Model, |
| consider enabling Mach number based blending between low speed and |
| high speed wall functions. You can do so by specifying a Mach |
| number threshold as follows: |
| |
| EXPERT PARAMETERS: |
| highspeed wf mach threshold = 0.1 # default=0.0 (off) |
| END |
+--------------------------------------------------------------------+

Parallel run: Received message from follower
--------------------------------------------
Follower partition: 3
Follower routine : get_TWFTFC
Leader location : End of Continuity Loop
Message label : 009100015
Message follows below - :
+--------------------------------------------------------------------+
| ****** Notice ****** |
| The non-dimensional near wall temperature (T+) has been clipped |
| for calculation of Wall Heat Transfer Coefficient. |
| |
| Boundary Condition : FluidSolid Side 2 |
| T+ clip value = 1.0000E-10 |
| |
| If this situation persists and you are using the High Speed Model, |
| consider enabling Mach number based blending between low speed and |
| high speed wall functions. You can do so by specifying a Mach |
| number threshold as follows: |
| |
| EXPERT PARAMETERS: |
| highspeed wf mach threshold = 0.1 # default=0.0 (off) |
| END |
+--------------------------------------------------------------------+
----------------------------------------------------------------------
| Equation | Rate | RMS Res | Max Res | Linear Solution |
+----------------------+------+---------+---------+------------------+

+--------------------------------------------------------------------+
| ERROR #004100018 has occurred in subroutine FINMES. |
| Message: |
| Fatal overflow in linear solver. |
+--------------------------------------------------------------------+
End of solution stage.

+--------------------------------------------------------------------+
| The following transient and backup files written by the ANSYS CFX |
| solver have been saved in the directory |
| C:/Project/bluntnodegree_pending/dp0_CFX_Solution-1/RocketWithExpP- |
| aTrans_001: |
| |
| 929_full.trn, 732_full.trn, 58_full.trn, 549_full.trn, |
| 381_full.trn, 3048_full.trn, 3000_full.bak, 2725_full.trn, |
| 2420_full.trn, 241_full.trn, 2132_full.trn, 1860_full.trn, |
| 1605_full.trn, 14_full.trn, 1365_full.trn, 134_full.trn, |
| 1140_full.trn, 0_full.trn |
+--------------------------------------------------------------------+


+--------------------------------------------------------------------+
| The following user files have been saved in the directory |
| C:/Project/bluntnodegree_pending/dp0_CFX_Solution-1/RocketWithExpP- |
| aTrans_001: |
| |
| pids, mon |
+--------------------------------------------------------------------+


+--------------------------------------------------------------------+
| For CFX runs launched from Workbench, the final locations of |
| directories and files generated may differ from those shown. |
+--------------------------------------------------------------------+


+--------------------------------------------------------------------+
| Warning! |
| |
| After waiting for 60 seconds, 1 solver manager process(es) appear |
| not to have noticed that this run has ended. You may get errors |
| removing some files if they are still open in the solver manager. |
+--------------------------------------------------------------------+


This run of the ANSYS CFX Solver has finished.

[Opaque]

Are you running a transient model?

did you run the steady model as an initial condition?

Which timestep did you use for integration?

97 coefficient loop iterations indicate the setup is incorrect somewhere.

[Gert-Jan]

- Lets start basic: What question do you want to answer when doing CFD on the rocket?
- Why do you include the solid domain?
- Why do you run transient? Did you try steady state as Opaque already asked?
- It looks like you select all relevant physics starting from the first step. Why do you try to hit the roof in one step? WHy not step by step?
- Did you try a simple case first, Meaning: Steady state, only air at a low velocity?
- It this runs, did you increase the velocity further and further, restarting from a converged case?

[funnier]

Are you running a transient model? - Yes

did you run the steady model as an initial condition? - No

Which timestep did you use for integration? - 0.07

97 coefficient loop iterations indicate the setup is incorrect somewhere. - My previous simulation with 10 degree angle of attack was converged with same setup. and in that setup my mesh was also poor.

[funnier]

- Lets start basic: What question do you want to answer when doing CFD on the rocket?
To monitor temp inside rocket wall

- Why do you include the solid domain?

to monitor temperature inside of rocket wall

- Why do you run transient? Did you try steady state as Opaque already asked?

because it is an extended study of previous simulation. I used temp, velocity , and pressure functions

- It looks like you select all relevant physics starting from the first step. Why do you try to hit the roof in one step? WHy not step by step?

be cause i performed same simulation with 10 degree angle of attack and it converged at first try. now i am doing the simulation with no angle of attack and it failed.

- Did you try a simple case first, Meaning: Steady state, only air at a low velocity? - NO

- It this runs, did you increase the velocity further and further, restarting from a converged case? - NO

[ghorrocks]

Please do not use third party download sites. Can you attach your output file directly to the forum?

As Opaque and Gert-Jan have said, this model appears to be poorly set up:
* CFX works best with 3-5 coeff loops per iteration, maybe up to 10 for tricky cases. 97 coeff loops means something is very wrong. That something is almost certainly your time step is far too big - reduce your time step until you get 3-5 coeff loops per iteration. Adaptive time stepping can be useful to automatically do this for you.
* What is transient about this simulation? I suspect the fluid is steady state but the solid thermal condition is transient (it will heat up over time). If this is the case then a much more effective way of doing it is to do the fluids model as steady state, and then impose the heat load from that model as a boundary condition on a transient model of just the solid thermal simulation. This simulation will be much more manageable.