CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > FLUENT

Convergent Divergent Rocket Nozzle Simulation Problem!

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree4Likes

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 27, 2020, 01:06
Exclamation Convergent Divergent Rocket Nozzle Simulation Problem!
  #1
New Member
 
Join Date: Feb 2020
Posts: 13
Rep Power: 4
a7medalsalmi is on a distinguished road
Hello,

I have been trying to simulate an axisymmetric CD nozzle with an atmospheric domain to observe the flow after the exit area. I am trying to replicate the problem shown in: https://pp.bme.hu/tr/article/view/11490/7907 with the same Boundary Conditions (Pressure Inlet, Pressure Outlet, Farfield Pressure, Free slip wall, and axis).

Although, I have faced multiple warnings in console when running the calculations such as:
*.temperature limited to 5.000000e+03
*.absolute pressure limited to 5.000000e+10
*.time step reduced in 133 cells due to excessive temperature change
*.turbulent viscosity limited to viscosity ratio of 1.000000e+05

I am not sure what exactly is the problem as I tried to change the Boundary conditions multiple times to investigate what would work. I am pretty sure my mesh is accurate as well with skewness below 0.3, with clustered cells near the nozzle wall which is the area of interest.

I would really appreciate if someone could point me in the right direction.
a7medalsalmi is offline   Reply With Quote

Old   February 27, 2020, 03:32
Default
  #2
Senior Member
 
Alexander
Join Date: Apr 2013
Posts: 2,249
Rep Power: 32
AlexanderZ will become famous soon enoughAlexanderZ will become famous soon enough
there are several tutorials regarding this simulation on youtube
first recommendation (besides mesh quality) patch pressure in chamber,
start with small pressure, converge, increase pressure, and so on
__________________
best regards


******************************
press LIKE if this message was helpful
AlexanderZ is offline   Reply With Quote

Old   February 27, 2020, 03:45
Default Material
  #3
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 34
vinerm will become famous soon enough
What I would doubt are not the boundary conditions or the mesh rather the material properties and operating conditions. Could you share a snapshot of material and operating conditions panel?

Assuming that everything is setup correctly, try fmg-initialization. This works like a test for such cases. If the fmg-initialization is successful, then the case is setup properly, else you need to modify something.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   February 27, 2020, 04:12
Default
  #4
New Member
 
Join Date: Feb 2020
Posts: 13
Rep Power: 4
a7medalsalmi is on a distinguished road
Hello Alexanderz I appreciate the quick reply.

I have been through the tutorials online, however, most of these tutorials simulate the CD Nozzle without an atmospheric domain. I could get the simulation to converge if I replicate their method, but I am also interested in simulating the flow after it exits the nozzle in an atmospheric layer.

I am not sure exactly what I am doing wrong as I have followed every step mentioned in the paper I mentioned previously, and I also tried using different Boundary conditions such as the mass inlet flow rate to get the calculations to converge but unfortunately, nothing worked thus far.
a7medalsalmi is offline   Reply With Quote

Old   February 27, 2020, 04:16
Default
  #5
New Member
 
Join Date: Feb 2020
Posts: 13
Rep Power: 4
a7medalsalmi is on a distinguished road
The material properties I used: Ideal Gas, Sutherland viscosity. The operating conditions I changed to 0.

I'm still somewhat a beginner in CFD, but I'll try and learn how fmg-initialization would work. Thank you for your quick reply.

Hopefully I'll figure out what I am doing wrong! Would it be possible if I uploaded the files so you could take a look at my simulation? Currently using Ansys version 19.2.
a7medalsalmi is offline   Reply With Quote

Old   February 27, 2020, 04:20
Default fmg-init
  #6
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 34
vinerm will become famous soon enough
If operating pressure and operating density, both are set to 0 values, then you have to ensure that at the inlet and outlet boundaries, absolute pressure values are used. So, even if you give mass flow inlet at the inlet you have to ensure some positive value in Supersonic/Initial Gauge Pressure. Similarly, outlet should have 101325 Pa.

For fmg initialization, you need to use commands

solve init fmg-init
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   February 27, 2020, 04:35
Default
  #7
New Member
 
Join Date: Feb 2020
Posts: 13
Rep Power: 4
a7medalsalmi is on a distinguished road
I haven't thought about operating density tbh. I am not sure how to change that but I'll figure it out. I'll try fmg-initialization and I'll get back to you. Thanks!
a7medalsalmi is offline   Reply With Quote

Old   February 27, 2020, 04:44
Default Operating Density
  #8
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 34
vinerm will become famous soon enough
Operating conditions panel has both, operating pressure and operating density. Both should be set to 0
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   February 27, 2020, 22:48
Default
  #9
Senior Member
 
Alexander
Join Date: Apr 2013
Posts: 2,249
Rep Power: 32
AlexanderZ will become famous soon enoughAlexanderZ will become famous soon enough
it took 10 sec to find this link
https://www.youtube.com/watch?v=oY_3_c0rDiw

everything had been done already, search
__________________
best regards


******************************
press LIKE if this message was helpful
AlexanderZ is offline   Reply With Quote

Old   February 27, 2020, 22:54
Default
  #10
New Member
 
Join Date: Feb 2020
Posts: 13
Rep Power: 4
a7medalsalmi is on a distinguished road
Yes and I told you, I have been through these videos. I already saw the video that you linked, and I tried to replicate everything he's done as well but to no avail. I still get divergence when running calculations. I am not sure what I am doing wrong.
a7medalsalmi is offline   Reply With Quote

Old   February 28, 2020, 04:14
Default Initialization
  #11
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 34
vinerm will become famous soon enough
Was it successful with the fmg-initialization?
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   February 28, 2020, 12:51
Default
  #12
New Member
 
Join Date: Feb 2020
Posts: 13
Rep Power: 4
a7medalsalmi is on a distinguished road
Hey vinerm.

Unfortunately, it was not successful. The solution was diverging once again. Below was the output I got after the command:

" solve init fmg-init
Enable FMG initialization? [no] yes

Creating multigrid levels...
Grid Level 0: 97750 cells, 196311 faces, 98562 nodes; 2 clusters
Grid Level 1: 24487 cells, 98674 faces, 98562 nodes; 2 clusters
Grid Level 1: 24487 cells, 49810 faces, 0 nodes
Grid Level 2: 6216 cells, 50159 faces, 98562 nodes; 2 clusters
Grid Level 2: 6216 cells, 13175 faces, 0 nodes
Grid Level 3: 1568 cells, 25641 faces, 98562 nodes; 2 clusters
Grid Level 3: 1568 cells, 3807 faces, 0 nodes
Grid Level 4: 413 cells, 13619 faces, 98562 nodes; 2 clusters
Grid Level 4: 413 cells, 1467 faces, 0 nodes
Grid Level 5: 106 cells, 7363 faces, 98562 nodes; 2 clusters
Grid Level 5: 106 cells, 836 faces, 0 nodes
Done.

absolute pressure limited to 5.000000e+10 in 4 cells on zone 3

temperature limited to 5.000000e+03 in 27 cells on zone 3


FMG: Converge FAS on level 5


FMG: Converge FAS on level 4


FMG: Converge FAS on level 3


FMG: Converge FAS on level 2


FMG: Converge FAS on level 1
0.
Reversed flow in 150 faces on pressure-inlet 6.

reversed flow in 3 faces on pressure-outlet 10.

time step reduced in 536 cells due to excessive temperature change

absolute pressure limited to 1.000000e+00 in 2 cells on zone 3

absolute pressure limited to 5.000000e+10 in 869 cells on zone 3

temperature limited to 5.000000e+03 in 2514 cells on zone 3
->1.->2.->3.->4.->5.<<<<<

turbulent viscosity limited to viscosity ratio of 1.000000e+06 in 117 cells

turbulent viscosity limited to viscosity ratio of 1.000000e+06 in 116 cells"
a7medalsalmi is offline   Reply With Quote

Old   February 28, 2020, 12:58
Default fmg-initialization
  #13
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 34
vinerm will become famous soon enough
Well, that explains it. As stated, if the fmg-initialization is not successful, there is something wrong with the setup. Could you share snapshots of material properties, boundary conditions, and operating conditions? Solver settings and mesh quality would also be useful.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   February 28, 2020, 13:09
Default
  #14
New Member
 
Join Date: Feb 2020
Posts: 13
Rep Power: 4
a7medalsalmi is on a distinguished road
Sure no problem.

solver settings: https://postimg.cc/KR5f78jN
Boundary conditions: https://postimg.cc/ThfWVqDz
material properties: https://postimg.cc/nsfq68Xz
operating conditions: https://postimg.cc/JyHdQC9z
mesh: https://postimg.cc/RWk2y01H (skewness below 0.4)
https://postimg.cc/9DLBKm6B

Thank you!
a7medalsalmi is offline   Reply With Quote

Old   February 28, 2020, 13:18
Default Boundary Conditions
  #15
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 34
vinerm will become famous soon enough
Rest appear to be good but there are two things

1. By boundary conditions, I mean the conditions applied at the boundary; images from Fluent. And you seem to have a mix of the conditions. Such as far field and free-slip. Furthermore, you have far-field attached to the wall. This is not allowed and supposedly the reason for fmg-initialization failure. Best would be to make all of these pressure outlet, i.e., C, D, and E, all should be pressure outlet.

2. Secondly, what is the Mach number for your case? If it is less than 2, I'd recommend using pressure-based solver with pseudo-transient coupled solver.
a7medalsalmi likes this.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   February 28, 2020, 13:38
Default
  #16
New Member
 
Join Date: Feb 2020
Posts: 13
Rep Power: 4
a7medalsalmi is on a distinguished road
Pressure inlet (Temperature=400K): https://postimg.cc/BtrCDw3J
Pressure outlet (Temperature=300K): https://postimg.cc/ygzZx29G

I also attached the initial values from inlet: https://postimg.cc/2bF2SQq4

I tried changing the boundary conditions as you suggested. A divergence is still occurring when running the calculations. This is what was prompted in the console:

"solve init fmg-init
Enable FMG initialization? [no] yes

Creating multigrid levels...
Grid Level 0: 97750 cells, 196311 faces, 98562 nodes; 2 clusters
Grid Level 1: 24487 cells, 98674 faces, 98562 nodes; 2 clusters
Grid Level 1: 24487 cells, 49810 faces, 0 nodes
Grid Level 2: 6216 cells, 50159 faces, 98562 nodes; 2 clusters
Grid Level 2: 6216 cells, 13175 faces, 0 nodes
Grid Level 3: 1568 cells, 25641 faces, 98562 nodes; 2 clusters
Grid Level 3: 1568 cells, 3807 faces, 0 nodes
Grid Level 4: 413 cells, 13619 faces, 98562 nodes; 2 clusters
Grid Level 4: 413 cells, 1467 faces, 0 nodes
Grid Level 5: 106 cells, 7363 faces, 98562 nodes; 2 clusters
Grid Level 5: 106 cells, 836 faces, 0 nodes
Done.


FMG: Converge FAS on level 5


FMG: Converge FAS on level 4


FMG: Converge FAS on level 3


FMG: Converge FAS on level 2


FMG: Converge FAS on level 1
0.
reversed flow in 28 faces on pressure-outlet 8.

reversed flow in 26 faces on pressure-outlet 9.

reversed flow in 14 faces on pressure-outlet 10.

time step reduced in 16 cells due to excessive temperature change

absolute pressure limited to 1.000000e+00 in 1 cells on zone 3
->1.->2.->3.->4.->5.<<<<<"
a7medalsalmi is offline   Reply With Quote

Old   February 28, 2020, 13:39
Default
  #17
New Member
 
Join Date: Feb 2020
Posts: 13
Rep Power: 4
a7medalsalmi is on a distinguished road
The mach number for my problem would around 4.2. Thus, a density-based solver seems more appropriate.
a7medalsalmi is offline   Reply With Quote

Old   February 28, 2020, 15:04
Default Temperature gradient
  #18
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 34
vinerm will become famous soon enough
With pressure outlet, fmg initialization seems to be better. There is only one cell that has temperature limit applied. To improve this, you can disable secondary temperature gradients using following command

(rpsetvar 'temperature/secondary-gradients? #f)

One more thing, is it Implicit method you are using or Explicit? Usually, such high Mach number simulations require proper solution steering.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   March 1, 2020, 19:04
Default
  #19
Senior Member
 
Alexander
Join Date: Apr 2013
Posts: 2,249
Rep Power: 32
AlexanderZ will become famous soon enoughAlexanderZ will become famous soon enough
increase pressure in chamber gradually, start with low value
when you are talking about Mach number do you mean external flow? If so, increase speed of external flow gradully too
__________________
best regards


******************************
press LIKE if this message was helpful
AlexanderZ is offline   Reply With Quote

Old   July 5, 2020, 03:28
Smile Solution
  #20
New Member
 
Join Date: Feb 2020
Posts: 13
Rep Power: 4
a7medalsalmi is on a distinguished road
Alright, for those of you who are approaching this CFD problem and are undergoing similar issues, I managed to solve it by applying a combination of solutions:

1. Make sure that you adhere to good meshing habits, even though your mesh might be very fine and clustered along the nozzle wall, the cells shouldn't jump in size suddenly so be careful when using the hard biased cells option. Also, read on the y plus value and make sure for this specific problem to have the y plus be less than 1 to get accurate results regarding the shock placement along the nozzle wall.
2. Specify the hydraulic diameter as the nozzle inlet to ensure an accurate representation of the inflow duct of the experimental equipment.
3. Try a range of courant numbers starting from the default number of 5 and lowering it up to 1 and less and observe which courant number provides the best convergence.
4. Try a Spalart All-maras turbulence model first as it is a simpler one equation model which takes less time for the solution to converge, if you are interested in capturing the flow separation accurately you can try the k-w SST model later on.
steadyman likes this.

Last edited by a7medalsalmi; July 27, 2020 at 07:08.
a7medalsalmi is offline   Reply With Quote

Reply

Tags
boundary condition, c-d nozzle, compressible, convergent-divergent, rocket nozzle

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
shocks in convergent divergent nozzle, convergence issue yogeshghadge314@gmail.com Main CFD Forum 19 January 2, 2020 17:54
Inverse Design Optimization khavart SU2 Shape Design 0 June 20, 2019 04:37
compressible, rhoSimpleFoam, multi-species, steady state, rocket nozzle David_C OpenFOAM Running, Solving & CFD 1 April 18, 2017 12:01
mass flow rate issue in supersonic nozzle simulation xkang FLUENT 0 July 31, 2014 17:06
Supersonic Nozzle Exhaust Simulation mikeh FLUENT 0 May 1, 2014 22:28


All times are GMT -4. The time now is 02:41.