|
[Sponsors] |
October 12, 2016, 14:48 |
Problem with two meshes in cfx
|
#1 |
New Member
Patryk
Join Date: Apr 2016
Location: Poland
Posts: 11
Rep Power: 10 |
Dear CFX users,
I am new in turbomachinery Ansys CFX, and my question might be silly, but I can't find any help on the internet or documentation. I'm trying to do simulation of jet ski pump which is case of axial pump, I have a rotor and stator models done using bladegen and mesh using turbogrid. My problem is that when I want import this 2 meshes into CFX-pre, they appear in bad position and interference each other. What I need to do to make this meshes appear like : "Outlet of mesh1 sticks to Inlet of mesh2"? Image under the link : https://gyazo.com/75409c478fc2d716f0164adeb84de4fb |
|
November 28, 2016, 04:53 |
|
#2 |
Senior Member
Join Date: Aug 2014
Location: UK
Posts: 213
Rep Power: 13 |
In case if you're still stuck, the problem is simply because of the incorrect coordinates of your rotor and stator geometry in bladegen, i.e. the coordinates of second component should begin exactly from where the previous component ends...
|
|
November 28, 2016, 18:09 |
|
#3 |
New Member
Patryk
Join Date: Apr 2016
Location: Poland
Posts: 11
Rep Power: 10 |
Yes, that was my problem. I have already solved it by myself, but thank you for reply!
|
|
November 28, 2016, 18:15 |
|
#4 |
Member
turbo4life
Join Date: Nov 2016
Posts: 41
Rep Power: 9 |
One way to do it is to change the mesh position from within CFX-Pre. Under "Mesh" in the outline tree, simply right click on the mesh you want to move and click "Transform Mesh". You can then rotate or translate the mesh as necessary.
On another note, if you are modeling a rotor/stator together, the angular position of the meshes doesn't really matter as long as the axis of rotation is the same. You can simply tell CFX to communicate between the two meshes with a "stage" interface, and it will automatically adjust for the pitch change between the meshes. Does that make sense? If not, perhaps a few pictures would help me understand. |
|
November 28, 2016, 18:28 |
|
#5 |
New Member
Patryk
Join Date: Apr 2016
Location: Poland
Posts: 11
Rep Power: 10 |
Thank you, I didn't know that method. I changed coordinates of parts and it works as I want maybe you could tell me If it'll be good to solve this simulation using frozen rotor interface model and homogenous multiphase model for cavitation?
I'm simulating flow in jet ski pump, made from 4 meshes (intake, rotor, stator, nozzle) |
|
November 28, 2016, 18:52 |
|
#6 |
Member
turbo4life
Join Date: Nov 2016
Posts: 41
Rep Power: 9 |
When you have multiple blade rows, it's better to use a "stage" interface, so you capture blade-to-blade interaction. You can start with "frozen rotor" if you want (for ease of convergence), but the final solution should have the "stage" interface.
As for the cavitation model, I'd recommend starting with constant density water as an initial case, and then restarting with the cavitation model turned on. Also, if cavitation behavior is of particular interest, you will need to converge this as an unsteady simulation. If it's just performance, blade loading, and general flow characteristics you are looking for, then you don't need the cavitation model and steady state is fine. |
|
November 29, 2016, 05:57 |
|
#7 |
New Member
Patryk
Join Date: Apr 2016
Location: Poland
Posts: 11
Rep Power: 10 |
Ok, thanks.. I try to solve it using "stage" interface. I'm looking for basic, general flow characteristics and regions where cavitation effect may occur. What do you think about checking this cavitation regions in steady state simulation as a "Water.Vapor.Volume.Fraction" isosurface set to 10% ? (Using multiphase model and cavitation, phase 1: Water at 20C, phase 2: Water vapor. Water changing to vapor at 3457 Pa). I set Opening type of inlet and outlet with 1 atm and give rpm's for rotor.
And second question.. Is it necessary to wait untill simulation finish by itself (convergre)? because i set max. iterations to 1000 and it's taking me 15 hours to solve it, I have low end pc.. Is the solution will be a little close to realistic after this 1000 iterations or I need to give it much more? |
|
November 29, 2016, 11:32 |
|
#8 | |
Member
turbo4life
Join Date: Nov 2016
Posts: 41
Rep Power: 9 |
See my responses below in red.
Quote:
|
||
November 29, 2016, 13:40 |
|
#9 |
New Member
Patryk
Join Date: Apr 2016
Location: Poland
Posts: 11
Rep Power: 10 |
okay, I will solve it without cavitation models and plot static pressure throughout the model and give it more iterations.. hope it converge and won't take me whole week
What you think, how many iterations it'll need untill converge? about 5000 or even more? And do you know how can I check area occupied by pressure under 3574Pa on rotor blades in CFD Post? |
|
November 29, 2016, 16:12 |
|
#10 |
Member
turbo4life
Join Date: Nov 2016
Posts: 41
Rep Power: 9 |
Every problem is different. You need to look at the imbalances to determine level of convergence. One way to speed up convergence is to manually increase the time step after the problem has converged a bit. This can be done within the solver manager.
|
|
November 29, 2016, 16:19 |
|
#11 |
New Member
Patryk
Join Date: Apr 2016
Location: Poland
Posts: 11
Rep Power: 10 |
And what about checking area on rotor blades where pressure is under 3574Pa? How to do that in CFD Post?
|
|
December 2, 2016, 08:46 |
|
#12 |
Member
Alex
Join Date: Feb 2016
Posts: 81
Rep Power: 10 |
||
December 2, 2016, 08:49 |
|
#13 |
Member
Alex
Join Date: Feb 2016
Posts: 81
Rep Power: 10 |
||
December 2, 2016, 12:23 |
|
#14 |
Member
turbo4life
Join Date: Nov 2016
Posts: 41
Rep Power: 9 |
Yes, I mean for k-epsilon. SST is great and I use it too, but only for final solutions, because it requires a very fine mesh and is not practical for many users with limited computing resources.
|
|
December 2, 2016, 14:50 |
|
#15 |
Senior Member
Join Date: Feb 2011
Posts: 496
Rep Power: 18 |
||
December 2, 2016, 15:05 |
|
#16 | |
Member
turbo4life
Join Date: Nov 2016
Posts: 41
Rep Power: 9 |
Quote:
What I meant by my comment was that to realize any benefit from SST over k-epsilon, a very fine mesh is required, and most users don't have the resources available to them to be running simulations of this size with reasonable turnaround time. Therefore, unless you want to resolve extremely fine boundary layers, SST is not necessary and k-epsilon will give you a perfectly good solution in less time. That's why I usually recommend it. |
||
December 3, 2016, 01:49 |
|
#17 | |
Senior Member
Join Date: Feb 2011
Posts: 496
Rep Power: 18 |
Quote:
|
||
December 3, 2016, 10:44 |
|
#18 |
Member
turbo4life
Join Date: Nov 2016
Posts: 41
Rep Power: 9 |
In my experience, if you run the same mesh with SST and k-epsilon, with no previous solution to start from, SST is less stable and takes more time to achieve the same level of convergence. This is especially true for transonic and supersonic flows.
|
|
December 5, 2016, 09:25 |
|
#19 |
Senior Member
Maxim
Join Date: Aug 2015
Location: Germany
Posts: 415
Rep Power: 13 |
I wonder what Florian Menter would say to that
|
|
December 5, 2016, 10:49 |
|
#20 |
Member
turbo4life
Join Date: Nov 2016
Posts: 41
Rep Power: 9 |
Ha. That's a good one . Before I upset the turbulence police any more than I already have, please allow me to further explain my position. In all seriousness, I understand why many people prefer SST over k-epsilon, and honestly, I probably would too if I could figure out a way to overcome the convergence problems I experience when starting from the default CFX initialization (no previous solution). I primarily use CFX for radial inflow turbine CFD, and oftentimes, there is supersonic and/or transonic flow bleeding into the mixing plane interface between the nozzles and the rotor wheel. I find that when starting a case like this with the SST model, it never makes it very far before crashing. Yet, if I first converge the case with k-epsilon, and then re-converge with SST, it works fine. However, after close inspection of the 2 solutions, k-epsilon turns out to be perfectly fine for getting me the critical information I need (blade loading, performance, small flow separations, etc). Therefore, the SST solution often becomes an unnecessary step in my process. I have used CFX for many years, but I am a turbomachinery designer first, and need fast design cycle time for CFD to be viable in my process flow. For the record though, I think Florian Menter is a god in this field. K-epsilon has just worked out better for me.
|
|
Tags |
turbomachinery mesh cfx |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Convergence problem of CFX when comparing with FLUENT with same mesh | guxin7005 | CFX | 8 | May 22, 2014 15:13 |
CFX pressure in Simulations problem | nasdak | CFX | 1 | April 14, 2010 13:22 |
Problems with adding two meshes together in CFX Pre | peterputer1 | CFX | 2 | September 23, 2009 08:08 |
Ansys Workbench (CFX) bucket problem | njsavage | CFX | 1 | April 30, 2009 09:51 |
Urgent Problem with Hypermesh and CFX | Luk | CFX | 5 | March 14, 2008 04:59 |