[JeJun]

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: 20ºC
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?

[ghorrocks]

Please attach your output file and an image of the results you are getting.

[JeJun]

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

[ghorrocks]

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.

[JeJun]

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?

[JeJun]

my mesh is ok. The same mesh ran steady and get 10^-6

let me show you my steps in images:


Note:
ENTRADA=INLET
SAIDA=OUTLET
CILINDROS=CYLINDERS
PAREDES=WALLS


1.jpg

2a.jpg

2b.jpg

2c.jpg

3.jpg

[JeJun]

4.jpg

5.jpg

6a.jpg

6b.jpg

7a.jpg

[JeJun]

7b.jpg



sorry about multiples messages

[JeJun]

Originally Posted by ghorrocks

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.

I'm going to run again to get the output file.

Are my steps correct, by the way?

[ghorrocks]

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?

[JeJun]

Thank you so much for the answer.

Originally Posted by ghorrocks

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.

So, I do not know if my Timestep is correct. How do I manage to do that?

Originally Posted by ghorrocks

Is your mesh correct? You say it is OK. How do you know? Did you do a sensitivity check?

ok, I don't. How do I manage to do that sensitivity check?




Thank you very much in advance

[Gert-Jan]

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.

[JeJun]

Originally Posted by Gert-Jan

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

I changed the timestep a few times. It turns out I do not know if I'm doing right in the other steps either.

Originally Posted by Gert-Jan

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.

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

[ghorrocks]

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.

[Gert-Jan]

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.

[JeJun]

Thank you both for the help.
My problem was the timestep.
I did with 0.001 and it worked. Thank you very much

[JeJun]

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

[ghorrocks]

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.

[JeJun]

Originally Posted by ghorrocks

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.

thx, i made it.

[JeJun]

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