|
[Sponsors] |
Transient Simulation. Wind Tunnel. 2 Cylinders |
![]() |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
![]() |
![]() |
#1 |
New Member
Jésus F. Júnior
Join Date: Jan 2019
Posts: 13
Rep Power: 7 ![]() |
Hello
I'm running a transient simulation on CFX, but it does not come up with Vortex Shedding. It is a simulation of a wind tunnel with 2 cylinders, each cylinder has 29.7mm and the tunnel is 940mm in length and 200 of edges. The first cylinder is 470mm from the inlet and the second cylinder is a center-to-center distance from the first cylinder of 77.22mm. Contour conditions are. *Input: Mass Flow Rate: 0.294 kg -1; * Outlet: Static pressure: 0 pa * Cylinders: No slip wall and smooth wall * Default Domain: Air Ideal Gas; Reference Pressure: 91325.8 Isothermal: 20şC Turbulence SST * Analysis type: Transient Total Time: 5 seconds Timestep: 0.004387 For this timestep, used strouhal number 0.2 and U = 6.77m / s * Output Control Trn Results Selected Variables: Pressure, Velocity, Velocity u, Velocity v, Velocity w Every Timestep * Global Initialization U: 6.77 m / s V: 0 W: 0 Relative Pressure: 0 Could someone help me, please? What am I doing wrong? |
|
![]() |
![]() |
![]() |
![]() |
#2 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,816
Rep Power: 144 ![]() ![]() ![]() ![]() |
Please attach your output file and an image of the results you are getting.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
![]() |
![]() |
![]() |
![]() |
#3 |
New Member
Jésus F. Júnior
Join Date: Jan 2019
Posts: 13
Rep Power: 7 ![]() |
unfortunately, I deleted the results for transient simulation.
For example, when I put Plane1 for speed, it shows the same as the steady state.steady.jpg Thx for reply |
|
![]() |
![]() |
![]() |
![]() |
#4 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,816
Rep Power: 144 ![]() ![]() ![]() ![]() |
By the way, have you done the normal accuracy checks? In particular have you checked your time step, convergence tolerance and mesh size is OK? FAQ: https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F
Please attach your output file. I can't do much without that.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
![]() |
![]() |
![]() |
![]() |
#5 |
New Member
Jésus F. Júnior
Join Date: Jan 2019
Posts: 13
Rep Power: 7 ![]() |
I did my timestep according to strouhal number.
Re=8x10^4 --> St = 0.2 U = 6.77 m / s D = 0.0297m ----> f = 45.5892255892 T = 1/f = 0.0219350074 then, T/n (n = 20) then, timestep = 0.001 is that correct? Last edited by JeJun; January 23, 2019 at 21:40. |
|
![]() |
![]() |
![]() |
![]() |
#9 | |
New Member
Jésus F. Júnior
Join Date: Jan 2019
Posts: 13
Rep Power: 7 ![]() |
Quote:
I'm going to run again to get the output file. Are my steps correct, by the way? |
||
![]() |
![]() |
![]() |
![]() |
#10 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,816
Rep Power: 144 ![]() ![]() ![]() ![]() |
I am not going to check screen dumps of CFX-Pre. When you post the output file I will look at that. If screen dumps of CFX-Pre would be useful I would have asked for them.
Is your time step correct? Almost certainly not. Either do a time step sensitivity check to properly find the time step or use adaptive time steps, homing in on 3-5 coeff loops per iteration. Is your mesh correct? You say it is OK. How do you know? Did you do a sensitivity check?
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
![]() |
![]() |
![]() |
![]() |
#11 | ||
New Member
Jésus F. Júnior
Join Date: Jan 2019
Posts: 13
Rep Power: 7 ![]() |
Thank you so much for the answer.
Quote:
So, I do not know if my Timestep is correct. How do I manage to do that? Quote:
Thank you very much in advance |
|||
![]() |
![]() |
![]() |
![]() |
#12 |
Senior Member
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,885
Rep Power: 27 ![]() |
How difficult can it be.....?.....:
- Change the timestep size multiple times and see if and how it affects your solution - Change the mesh density multiple times and see if and how it affects your solution A single simulation is just a lucky shot. You need to find out how your system reacts upon changes to your model. My motto is: One simulation is not Simulation. Last edited by Gert-Jan; January 25, 2019 at 01:40. |
|
![]() |
![]() |
![]() |
![]() |
#13 | ||
New Member
Jésus F. Júnior
Join Date: Jan 2019
Posts: 13
Rep Power: 7 ![]() |
Quote:
Quote:
Hello. Good night. I did the simulation for a few days, but it ended now a little bit with an error and I do not even know how to see those results, would it have some way? I've attached the output thank you output.docx |
|||
![]() |
![]() |
![]() |
![]() |
#14 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,816
Rep Power: 144 ![]() ![]() ![]() ![]() |
You saved transient results files every time step, but you did not include the mesh. This means they will not be readable by themselves. You need to include the mesh for them to be useful by themselves. Transient results files without the mesh are only readable when a result file is written (or a later transient result file which does include the mesh).
In other words, you will not be able to read the results files from this run. You are going to have to do the run again. To stop this happening again select the "Add Mesh" option in the transient results file.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
![]() |
![]() |
![]() |
![]() |
#15 |
Senior Member
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,885
Rep Power: 27 ![]() |
It would not add the mesh to the transient files (.trn). There is no rotation, no mesh deformation. Why add a lot of unchanged mesh info (2M nodes) to each transient file? I would save a backup file every now and then (e.g. every 100 iterations?). Unless you change it, the contents of this .bak-file is equal to the final results file (with mesh) and allows you to open the intermediate transient files.
Since you forgot these backups, and have no results file, you cannot open the intermediate transient files. They contain data of the selected variables, but not mesh. What you can try is to create a short transient run (2 timesteps?) then open this results file in Post and add the transient results manually. It might work. I strongly recommend to try this outside Workbench: open CFD-Post from the CFX-launcher. Moreover, copy the files to a unique folder to not screw-up your workbench structure. |
|
![]() |
![]() |
![]() |
![]() |
#16 |
New Member
Jésus F. Júnior
Join Date: Jan 2019
Posts: 13
Rep Power: 7 ![]() |
Thank you both for the help.
My problem was the timestep. I did with 0.001 and it worked. Thank you very much |
|
![]() |
![]() |
![]() |
![]() |
#17 |
New Member
Jésus F. Júnior
Join Date: Jan 2019
Posts: 13
Rep Power: 7 ![]() |
Hello again.
I am running a similar simulation presented here again. the only difference is the position of the second cylinder relative to the first, the second cylinder is positioned a center-to-center distance of 1.1 diameter of the first. Diameter of both cylinders = 0.0297m Center-to-center distance between the two cylinders = 0.0297m x 1.1 = 0.03267m I ran different positions for the second cylinder and all went well, except this distance of 1.1. I could not catch the oscillation of the vortices. I used ADAPTIVE TIMESTEP as indicated and also used timestep found with strouhal number (0.2), but still could not reach. What can it be? Thank you very much in advance output file aa.txt |
|
![]() |
![]() |
![]() |
![]() |
#18 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,816
Rep Power: 144 ![]() ![]() ![]() ![]() |
FAQ: https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F
Do a sensitivity analysis on mesh size, time step size and convergence criteria to check your simulation is accurate. A quick look at your output file, I see an arbitrary time step size (was this determined correctly?) and max coeff loops of 5 (why so low?) and every time step it hits 5 coeff loops, so it is not reaching your convergence criteria. This is not a good way to set things up. Make the coeff loops much bigger (maybe 10), and the time step size smaller so it converges in 3-5 coeff loops. Or use adaptive time stepping to do it for you.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
![]() |
![]() |
![]() |
![]() |
#19 | |
New Member
Jésus F. Júnior
Join Date: Jan 2019
Posts: 13
Rep Power: 7 ![]() |
Quote:
![]() |
||
![]() |
![]() |
![]() |
![]() |
#20 |
New Member
Jésus F. Júnior
Join Date: Jan 2019
Posts: 13
Rep Power: 7 ![]() |
Now I'm in the post-processing in the cfx-post.
I wanna pick up the vorticity. So I'm doing vortex core region. But the vorticity is missing from "METHOD" I've done the same process in the steady method and it was alright. How to solve this problem? thanks |
|
![]() |
![]() |
![]() |
|
|
![]() |
||||
Thread | Thread Starter | Forum | Replies | Last Post |
Atmospheric BL simulation in a Wind Tunnel | mtrmasuko | FLUENT | 10 | January 15, 2019 08:59 |
[How to obtain supersonic flow inside a supersonic wind tunnel ?] | yx213 | Siemens | 1 | September 17, 2014 13:52 |
Wind Tunnel Simulation: How to measure the downforce? | luckyrob | STAR-CCM+ | 14 | September 8, 2014 12:34 |
Wind Tunnel Flow Simulation Mass Flow BC Issue | ledelman | SU2 | 4 | August 3, 2014 18:38 |
wind tunnel results vs fluent | pixie | Main CFD Forum | 1 | August 20, 2009 08:02 |