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

Simulation of a 3D air nozzle

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 5, 2021, 08:16
Default Simulation of a 3D air nozzle
  #1
New Member
 
Francesca Giusti
Join Date: Dec 2020
Location: Italy
Posts: 7
Rep Power: 2
France94 is on a distinguished road
Good morning everybody!
I'm trying to simulate the internal and external flow of the 3D nozzle attached and compare the results with an experimental setup that we have in our labs.
From the experiments we know that the nozzle is fed from a pressure vessel at 6.5 bar with a flow rate of 435 l/min. The simulation should be steady state.
I would really appreciate all your suggestions on how to perform this activity since it is the first time i'm approaching these simulations.
In particular i would like to have some advices regarding:
1. Solver type: pressure or density based?
2. Model: energy eq. on or off? which viscous model should I choose?
3. Material: the fluid is air, should I consider it as an ideal gas?
4. BCs: I have a symmetry plan, one nozzle inlet face (pressure or velocity inlet?) and multiple faces of the enclosure box surrounding the nozzle (which BCs should I impose here?)
5. Methods: which solution methods should I apply?
6. Initialization: hybrid or standard? and from where should the solver be initialized?
7. Calculation: how many iterations do you suggest to perform at the beginning?

I apologize for all these questions but, again, it is the first time form me and i'm a bit lost. I would like to thank everybody in advance.
Best regards,
Francesca
Attached Images
File Type: png Nozzle.PNG (95.0 KB, 17 views)
File Type: png Mesh.png (64.3 KB, 26 views)
France94 is offline   Reply With Quote

Old   February 6, 2021, 06:07
Default
  #2
Senior Member
 
Lorenzo Galieti
Join Date: Mar 2018
Posts: 121
Rep Power: 7
LoGaL is on a distinguished road
Hi
1) both are fine, I would stick with pressure solver just because it has more options and is more used. For very high Mach number instead, density based is better.
2)energy equation On, otherwise you can't assign equations of state. (Try to believe it, if you select ideal gas, it will turn energy equation on)
3) Yes, use ideal gas
4)The boundary conditions you use depend on the data you have. I suppose you have 6.5bar at the inlet of the nozzle and 1 bar at the outlet? If yes, use those. Do you know the mass flow? Then assign pressure on one side and mass flow on the other.
Remember that on the same side, you either impose mass flow or pressure, can't do both. Whichever is not imposed, must be matched by your solution.Y.e. if you impose the experimental pressure and not the experimental mass flow rate, your solution must give you back a correct mass flow rate.
5) What do you mean?
6) You can use hybrid for this case. Also standard will work.
7) The iterations to perform are based on when the solution converges. You put points in the domain where you monitor the solution (Temperature, velocity ecc), when those stabilize and your residuals are low, you can say it's converged.

Btw, I think the mesh is super good quality wise, but is not fine enough near the walls and in the nozzle section. Are you solving both solid and fluid?
LoGaL is offline   Reply With Quote

Old   February 6, 2021, 12:13
Default
  #3
New Member
 
Francesca Giusti
Join Date: Dec 2020
Location: Italy
Posts: 7
Rep Power: 2
France94 is on a distinguished road
Hi Lorenzo,
Thanks a lot for the support and the very complete answer. I am not interested in solving the solid domain since i am only interested in studying how the flow develops in ambient air outside the nozzle.
I totally agree with you: in order to catch the boundary layer inside the nozzle I was planning to insert an inflation for the internal walls of it. For what concerns the external walls Iím not sure that it is relevant. What do you think?

I would like to ask you further regarding the following points:
2) As solution model, I was thinking about standard K-eps, but gain Iím not familiar with the models so Iím not sure at all that is the more suitable one.
4) The only data that I know are the air pressure (6.5 Bar) inside the vessel that is feeding the nozzle and the volumetric flow rate (435 liter/minute) measured at the inlet of the nozzle with a sensor. The problem is that fluent requires a mass flow rate as inlet BC and I have estimated that at the inlet (7 mm in diameter) the velocity is ~190 m/s, so compressibility effects are relevant and i doní t know the density to pass from volumetric to mass flow rate. On the other side if I choose to use a pressure inlet BC i am not absolutely sure about its value at the inlet due to the losses in the piping that connect the vessel with the nozzle.
My idea, in conclusion, was to use a pressure inlet BC, letís say starting with 6.2 Bars, and keep on decreasing it until Iím able to Match the calculated volumetric mass flow rate at the inlet with the experimental one. What do you think?
Moreover my simulation takes place in a ďboxĒ with 5 faces (1 on the back of the nozzle, one on the front and 3 lateral faces) and 1 symmetry face since Iím studying only half flow. Which BC should I apply on the 5 faces? Maybe pressure outlet with 0 gauge pressure?
5) Here I was referring to the tab solution methods where I have to singularly choose the ones for pressure, density and so on.

Thanks again for your kind feedback. Best regards,
Francesca
France94 is offline   Reply With Quote

Old   February 6, 2021, 13:37
Default
  #4
Senior Member
 
Lorenzo Galieti
Join Date: Mar 2018
Posts: 121
Rep Power: 7
LoGaL is on a distinguished road
Hi francesca,

2) I would use K-omega SST. Standard k-epsilon is not good for wall bounded flows. Maybe you can first get a semi-converged solution with k-epsilon then switch to SST.
4) At the outlet (as posted in the picture) it is safe to assume there's 1 bar. For the inlet, more or less 6.5 bar. Now, fluent for numerical reasons works with operating pressures and gauge pressures.
You have that real pressure = operating pressure + gauge pressure.
If your operating pressure is 0 bar, then pressure inlet 6.5 bar, pressure outlet 1 bar
if your operating pressure is 1 bar, then pressure inlet 5.5 bar, pressure outlet 0 bar.
Keep in mind that you can change the boundary condition type, not sure if you understood that. Mass flow is the default one, but you can assign pressure

Concerning adjusting the inlet pressure to match the volumetric flow rate,I see the point but I would be careful with it, because many other things can make so that your simulation gives wrong flow rate. Think about it before deliberately adding uncertainty to your solution. If you are unsure of how much the pressure drop is, better to include part of the upstream geometry.


In any case, you should extend the inlet nozzle, even if it is not like this in the real geometry. The point is that the "numerical flow" needs space to develop. What you have in reality where you placed your inlet is a nice developed pipe flow, what you will have in the CFD if you don't extend the inlet is some flat profile garbage. Instead, if you extend the inlet, there's some fake geometry where the flow develops, so that at the point of interest it will be physically reasonable.


5) Aim for second order schemes for all quantities. If you give Fluent a good mesh, nothing should go wrong. Perhaps, you may initiate the simulation using the standard pressure scheme and then switch to second order one.

I once again stress that you will have to work a lot on your mesh and geometry, otherwise you will match nothing. Settings in the solver is the easy part
LoGaL is offline   Reply With Quote

Old   February 7, 2021, 15:22
Default
  #5
New Member
 
Francesca Giusti
Join Date: Dec 2020
Location: Italy
Posts: 7
Rep Power: 2
France94 is on a distinguished road
Hi Lorenzo,
Thanks again for your advices: as you suggested I have elongated the inlet section of the nozzle and i tried to insert an inflation for the inner walls but apparently it is incompatible with the hex dominant mesh that I choose for the enclosure outside the nozzle. I modified the mesh method there in tethra and tried to run the solver but during the initialization I was notified that the converge tolerance was not reached and if I tried to run the calculations I received the error "error at node 0 0 failed to allocate"

Just to see a result I went back to hex dominant mesh in the enclosure and no inflation layers but during the calculations I received multiple warnings regarding reversed flow on 100% area of the back and lateral surfaces of the enclosure and on 50% area of the front surface of it. I think it is related to the BC for the enclosure surfaces.I have understood that I have to work more on the mesh, but do you have any suggestion on how to improve the situation?

I attach the results on the symmetry and axis planes.
Best regards,
Francesca
Attached Images
File Type: jpg symmetry.jpg (32.4 KB, 11 views)
File Type: jpg axis.jpg (29.5 KB, 6 views)
France94 is offline   Reply With Quote

Old   February 8, 2021, 04:36
Default
  #6
Senior Member
 
Lorenzo Galieti
Join Date: Mar 2018
Posts: 121
Rep Power: 7
LoGaL is on a distinguished road
Hi Francesca,

You need the inflation layers, it's not possible to escape from that.

Also, I still don't get why it's meshing the solid, this should be avoided. Can't you suppress all the solid bodies? (Right click--> suppress)

I am surprised you say inflation layer is not compatible with hex dominant mesh, I alwais used that. Isn't it possible at all, or you assigned the nozzle walls and the inflation was not generated? If it is the second option, you should include all the walls, not only the nozzle ones.

You should definitely be able to generate a good tetra mesh (to be later converted into polyhedra in fluent by pushing a button). That is what i would aim for. You received that warning because, most probably, the mesh is trash, so the solver had issues converging, even in initialization stages where it solves something like potential flow.

Coming back to generating the tetra mesh ( or also the hexa one, if you prefer, but I wouldn't recommend it), you want three ingredients:
1) inflation layers on all the walls (i.e. all the faces where you assign a no slip wall condition--> all the faces but inlets and outlets). This cannot be avoided, and if you use k-omega SST (as you should) it has to be well done.
2) body of influence (BOI) sizings https://www.youtube.com/watch?v=3E1p1w32jt0 . Basically you create a secondary body (with the CAD) which defines a zone in your geometry where you want elements of a certain size ( usually smaller than the general size).
3) polyhedra mesh. once you read the mesh in fluent, you go in top left: setting up domain --> make polyhedra. Push the button and wait. If the tetra mesh is good, you geed a good polyhedra mesh. No tinkering required.

The final mesh I would recommend to have is
1) for each small passage in the nozzle: on the diameter 8-10 elements (control with BOI) + 8-10 inflation layers. At the moment, one is with 4 elements and the other i think 7-8, and no inflation (verrrrrrryy bad)
2) a BOI more or less overlapping with the jet in the chamber. You want a lot of resolution there

Keep in mind, I am not saying your mesh is bad, what I am saying is that at the moment you are far away from having enough resolution to capture what is going on inside. (Per capirci se puntiamo all'equivalente di un video in Hd, al momento stiamo vedendo un video sfocato nel peggior sito di streaming)

Once you get the hang of 1-2, I guarantee you it's going to get pretty easy. Maybe also very boring, but meshing is like ironing shirts, nobody likes it but if you do it badly, the result is shitty no matter what.
LoGaL is offline   Reply With Quote

Old   February 9, 2021, 19:01
Default
  #7
New Member
 
Francesca Giusti
Join Date: Dec 2020
Location: Italy
Posts: 7
Rep Power: 2
France94 is on a distinguished road
Hi Lorenzo,
Thanks again for your time and your clear answer!

The solid body of the nozzle is not meshed, i have extracted only the internal and external walls.
I used tetra mesh for the enclosure and for the "chamber" of the nozzle, while hexa mesh for the circular inlet and rectangular outlets of it.
I also inserted inflation layers on the inlet and outlet walls but not on the chamber walls because otherwise I received a warning regarding the creation of staircase mesh there and consequently the solver was crashing while converting tetras to polyhedras.
I inserted a BoI aligned with the flow and a sphere of influence just outside the outlets of the nozzle.

After the conversion in polyhedras I checked the quality of the mesh but I received a warning regarding the presence of a lot of left/right handed faces: I have seen that there are some commands to try to correct them so, if you don't have any other suggestion, i'll try to solve the issue in this way.
The real problem is in the hybrid initialization: if I try it I receive the warning "Divergence detected in AMG Solver" and after few iterations more an error regarding floating point. Do you think it is still an issue with the mesh? i'll attach some pictures of the refined mesh, tell me please what you think about it.

Thanks again, I really appreciate you support.
Best regards,
Francesca
Attached Images
File Type: jpg BoI.jpg (203.2 KB, 6 views)
File Type: jpg Nozzle_refinement.jpg (205.4 KB, 10 views)
File Type: jpg Flow_Axis.jpg (200.9 KB, 5 views)
File Type: png Polyhedra.PNG (174.0 KB, 6 views)
France94 is offline   Reply With Quote

Old   February 10, 2021, 04:22
Default
  #8
Senior Member
 
Lorenzo Galieti
Join Date: Mar 2018
Posts: 121
Rep Power: 7
LoGaL is on a distinguished road
Hi francesca,

Good work with bodies of influence and for trying around all the bunch of stuff I wrote in the message.

yes, believe me, either you are simulating super complicated physics, or fluent complains only if you give it a bad mesh. No, i don't think correcting them in fluent is a good idea, the mesh has to be good on it's own. I see it is boring and I agree, especially for an experimental, that is why I am spending time trying to help xD.
Bear in mind, we waste time with the mesh so that when we have a good one, you go to fluent, push the button and obtain results, zero problems.

You can check mesh quality in the mesher by watching this https://www.youtube.com/watch?v=vgLSfbo0I0o. I would suggest to check skeweness on top of orthogonal quality. Sometimes, one is better, sometimes the other. Anything you get above 0.97 is very bad. The average has to be also much much lower than 0.97. As you will see in the video, it is possible to visualize cell elements with low quality. Near the instogram in the video, there's also the "controls" button, which allows you to set the range of the instogram, so as to focus only on the crap part.

I attached a screenshot to this message: the green zones of the mesh are were I think it is good, yellow zones is where you need some work , mainly lack of inflation layers.
Red is only the small pipe that dumps the flow into the chamber ( if i understood correctly the geometry). Without inflation layers, your resolution is very low, so you don't capture the correct flow inside. If then the flow inside is not physically sound, the jet in the chamber is not correct as well, so on and so forth.

As I said
1) I want inflation layers on each single wall --> need to understand where staircase cells are generated (usually they will have very high skewness or very low orthogonal quality). My guess is in the region pointed by the white arrow in the screenshot. There the wall turns by 270 degrees, so perhaps the mesher doesn't manage to propagate the inflation through. Somehow it has to stop the inflation, so it generates staircase elements. If it is as I am saying, you may want to add a small fillet to the geometry, so that the turn is smooth, not sharp. This won't change anything in terms of results.

2) All this mesh warnings need to be fixed--> need to understand where bad elements are created. Again they will have very high skewness or very low orthogonal quality

So, check the mesh quality, spot the bad elements and their location, then we may want to make educated guesses of what is the problem. As a rule of thumb, sharp angles and relatively tiny geometry features both give problems.
very sharp angles --> round them with fillet
tiny geometry features --> either put BOI around and use a lot of elements to represent them, or delete them. If possible, do the second option,
Attached Images
File Type: jpg Mesh.jpg (199.5 KB, 5 views)
LoGaL is offline   Reply With Quote

Reply

Tags
fluent, nozzle, solver, viscous

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
Irrational results with perfectly expanded nozzle simulation Vishnu Sankar SU2 3 November 10, 2020 06:20
CFD Simulation and Optimization of Swirl nozzle AS_Aero CFD Freelancers 2 June 2, 2020 07:10
Basic Nozzle-Expander Design karmavatar CFX 20 March 20, 2016 08:44
Condition of Air velocity in Open Channel simulation wes1204 OpenFOAM Running, Solving & CFD 0 May 9, 2014 05:08
3D-Simulation of Water Flow From Nozzle into Air Navin Sampath FLOW-3D 2 February 26, 2009 10:46


All times are GMT -4. The time now is 21:52.