[Gert-Jan]

i don't think there is a other way. It would be very odd if there were 2 ways to obtain the same result.
Using my ccl, you should get a file named "outlet.csv". Maybe you should look better. Or you have something else wrong.

[Gert-Jan]

What CFX-version are you running?

[usamaperwez]

I am using CFX 15.0. I have set following settings but after completion of run, i dont get any file on my hard disk directory.

[usamaperwez]

After lot of searching, i have found this in official CFX Solver Guide:

"Export tab only apply to transient simulations."

Is it true? If it is true, is there any other way around to get RTD?

[Gert-Jan]

I don't know for CFX-15.0. I use the latest version i.e. 18.2. And there it works for steady state calculation for sure. I suggest to upgrade.

[usamaperwez]

When i made two export results in Output control, it worked. It seems to be a bug.

I found another interesting thing in my case. My problem consist of a serpentine channel which contain bends. For that, you need to activate Schiller Naumann model and then particle started to follow the bend path otherwise it was hitting the wall and bouncing back.

Thanks alot for the help.
Best of luck !

[Suman Sapkota]

Hello,

I am having the same problem. I am conducting a steady state analysis of pump and I am looking to track the particles (more or less same example as butterfly valve with erosion tutorial). The problem is I am only generating blank particle file. The .trk files are simply empty. Also, the .trk file is only created for 1 particle with pT1.trk file. How do I keep track of all the 20 particles? Do anyone has a way around it? or, helpful links?

While I am at it, would it be possible to generate impact velocity data of those particles from CFX?

[Gert-Jan]

In principle, the particles are stored in the results file. So, please first check whether you see particles in CFD-Post...........

(The '1' in the name PT1.trk does not refer to the first particle. Actually, I don't know where it refers to, but I think Lagrangian Phase #1.)

[Gert-Jan]

Moreover, what does the output file tell you about your particles? Do the particles start at your inlet? How many left the domain through the outlet? This should tell you at least if the particle track was succesfull......

[Suman Sapkota]

Hello Gert,

Thank you for the reply. I solved the problem of getting variables in the result file. i am sorry for not replying earlier. Now, what I wanted to see in the simulation of the pump is that: I need to know particle trajectory of each of 100 particles and their velocity of impact at the blade only. I can generate the particle trajectory data with 'x,y,z' position and 'u,v,w' velocity of particles. But I am only getting particle trajectory data in 1 file which I believe is of 1 particle. i even exported to .csv format to only find to me of what it seems like 1 particle data.

Do you have any suggestions to know particle trajectory of each of 100 particles and their velocity of impact at the blade only (without considering the entire domain)? Thanking you.

[Gert-Jan]

Yes. You get the data in 1 file.

Assuming that you use a filter for particles only hitting the pumpblade, it contains the data of all particles that hit the blade. Then you need to extract the required info yourself. You could for example export the time of the particles as well. Then in a spreadsheet look for the velocity in the row prior to the row where time is set to zero again.

Unfortunately CFX does not allow you to export the particle track number, which would facilitate this procedure a lot. Don't ask me why. I have been asking for this functionalty for already 10 years at ANSYS support and somehow, they refuse to implement this functionality.

[Suman Sapkota]

Thank you for the reply. You have been very helpful. So, the data that I am getting is related to which particle? I suppose the data in the result file is not usable then because we do not know which particle the data belong to. Am I correct? But the silver lining is we can set up a condition to know the velocity and position of ''all the particles'' that hit the blade at the time of collision. Then, do i need to extrapolate the data to excel to find the velocity just before? Am I correctly rephrasing you? Do you have any documents or files link or information about this? Thanking you.

[Gert-Jan]

You can obtain a csv-file in two ways. A Pre or a Post way:

Post-way
1) You should open your results file in Post
2) Double click on the particle track (Res PT for .....).
3) Select filter
4) Set End region = your pump blade
5) Set max tracks to 1000 (at least more than the total number of particles to make sure you won't miss one)
6) Hit apply
7) Export to csv. Export variables: x,y,z,u,v,w,Particle Time
(In Post You will only see the particles that hit the pump blade.)

Pre-Way
1) Go to Output Control>Export>Export Results 1
2) There set that you want a csv-file at the end of your CFX-run. Select your blade wall as Output Boundary

With your csv-file:
1) Open the csv in a Spreadsheet.
2) Look for the zeros in the Column Particle Time. Say this is row 'n'
3) The velocity in the row 'n-1' is the hit velocity of the previous particle

You can automate this easily in the Spreadsheet, with a simple macro . A challenge is that you don't have the particle number. So you can't directly link the Spreadsheet to what you see in Post.........



Alternatively, you should go to Pre, go to Output Control > Particles and say "Keep Track File". And select "Formatted Track File Format".
This will give you ALL particle track data in plain text format. And then I mean everything so the file can become huge. The advantage is that the particle number is given as well. Unfortunately, the data structure can be vague. Also, it is impossible to tell Pre to only save the tracks that hit the pump blade. So, this alternative route is also not the best.

Maybe you can combine the information of both worlds (Pre and Post) and find your way out.

Good Luck, Gert-Jan

[Suman Sapkota]

Thank you for your support. Now that I have set all the conditions and checked that all the particles leave domain. In the post process, I cannot get the "End Region" as Blade. The picture attached should clear it. Should not the domain of Blade show up in the dialogue box?

[Gert-Jan]

Then you all particles find their way to the outlet. But that is not what you expected, I guess. Probably particles hit the blade but bounce off.
Did you forget to specify that the particles should stick on the blade wall? In Pre you have to set the restitution coefficients to 0.
Then in the CFD-calculation the particles will be eliminated when they hit the blade, allowing you to select the pumpblade as end region in CFD-Post.

[Suman Sapkota]

Yes, when I made the restitution coeff. (both parallel and perpendicular) to zero. The Blade option shows up. Thank you Gert. When I set the export in cfx pre (precisely output boundary as "Blade domain"), the results obtained in .csv file shows 17 data which I presume is the number of particles hitting the blade (out of 1000). In the 'pt1.trk' file, I have data of 998 particles. Now, the question is: when I try to export the particle track, velocity, angle of impact of the particles from the CFD post, it shows the error as indicated in the figure. Can you help me through this?

[Gert-Jan]

I don't know what goes wrong.
Can you view the tracks in the viewer anyway? You have its visibility ticked on, but I don't see them in your window. Can you colour the tracks with their time? Is the variable time present anyway?

[Suman Sapkota]

I have attached the two excel files. one contains the data that i generated from the "pre" that particles hitting the blade and "particles hitting the outlet". i checked with the coordinates and the particles indeed hit the blade. Out of 1000 particles 15-16 particles hit the blade. It may be due to the low mass of particles. But there is something from the pre. However, I do not understand why it does not do the same for the post, only this time it has to transfer the whole trajectory. Anyways, I got the results that I wanted. I am grateful to you Gert. Thank you so much.

[Suman Sapkota]

Hello Gert,
I am here to trouble you again. Sorry.

I am performing steady state analysis of free impeller of centrifugal pump. I am trying to track the particles. That being said, i have attached the geometry picture in here. The problem is when I simulate the 'old moving domain'(which consists of hub+shroud+blade) domain as "rotational" it gives me high efficiency around 85%. Now, when I use particle tracking, I need to create Blade as a separate boundary in the pre because I have to track the particles hitting the blade. Now, my rotational domain is divided into moving (hub+shoud) and blade. (In the end I add up the torque due to both of these components to calculate efficiency) This enables me to select the end region as blade in the post processing. But I am getting low efficiency 77%. This should not be true because it is one way coupling. And when I try to interface it to the (hub+shroud), it shows the error in the picture because I am using periodic boundaries. What should I do to get my efficiency back to 85% with Blade as a separate rotating boundary inside the Moving (also rotating) boundary (hub+shroud) to solve this problem?

[Gert-Jan]

Difficult to say, but you have certain mesh surfaces assigned to more than one boundary. That gives a conflict of course.

Regarding the efficiency loss, also difficult to say. I don't understand why you had to change the setup when creating a unique boundary for the blade. Carefully check all settings. So ask yourself some questions:

- same inlet conditions?
- what is moving?
- what is standing still?
- what is counter rotating?

In Post there is a standard calculator that helps you calculating the efficiency of the pump. Does this calculator give you the same efficiency for both cases?