CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

Problem with two meshes in cfx

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

Like Tree6Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   October 12, 2016, 14:48
Default Problem with two meshes in cfx
  #1
New Member
 
Patryk
Join Date: Apr 2016
Location: Poland
Posts: 8
Rep Power: 3
FeveR is on a distinguished road
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
FeveR is offline   Reply With Quote

Old   November 28, 2016, 05:53
Default
  #2
Senior Member
 
Join Date: Aug 2014
Posts: 178
Rep Power: 4
fresty is on a distinguished road
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...
FeveR likes this.
fresty is offline   Reply With Quote

Old   November 28, 2016, 19:09
Default
  #3
New Member
 
Patryk
Join Date: Apr 2016
Location: Poland
Posts: 8
Rep Power: 3
FeveR is on a distinguished road
Yes, that was my problem. I have already solved it by myself, but thank you for reply!
FeveR is offline   Reply With Quote

Old   November 28, 2016, 19:15
Default
  #4
Member
 
Brian Parrelli
Join Date: Nov 2016
Location: Southern California
Posts: 41
Rep Power: 2
bparrelli is on a distinguished road
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.
fresty, unclewallcn and FeveR like this.
__________________
Brian Parrelli
Specialties: Turbomachinery, CFD
Professional Profile: Click Here

Do you want to become better at CFX? Sign up for my virtual course through SolidProfessor: "Introduction to ANSYS CFX" >>>
Click Here
bparrelli is offline   Reply With Quote

Old   November 28, 2016, 19:28
Default
  #5
New Member
 
Patryk
Join Date: Apr 2016
Location: Poland
Posts: 8
Rep Power: 3
FeveR is on a distinguished road
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)
FeveR is offline   Reply With Quote

Old   November 28, 2016, 19:52
Default
  #6
Member
 
Brian Parrelli
Join Date: Nov 2016
Location: Southern California
Posts: 41
Rep Power: 2
bparrelli is on a distinguished road
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.
__________________
Brian Parrelli
Specialties: Turbomachinery, CFD
Professional Profile: Click Here

Do you want to become better at CFX? Sign up for my virtual course through SolidProfessor: "Introduction to ANSYS CFX" >>>
Click Here
bparrelli is offline   Reply With Quote

Old   November 29, 2016, 06:57
Default
  #7
New Member
 
Patryk
Join Date: Apr 2016
Location: Poland
Posts: 8
Rep Power: 3
FeveR is on a distinguished road
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?
FeveR is offline   Reply With Quote

Old   November 29, 2016, 12:32
Default
  #8
Member
 
Brian Parrelli
Join Date: Nov 2016
Location: Southern California
Posts: 41
Rep Power: 2
bparrelli is on a distinguished road
See my responses below in red.

Quote:
Originally Posted by FeveR View Post
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.
I would recommend simply turning off all cavitation models and plotting static pressure throughout the model. You can track local regions where the static pressure falls below the water vapor pressure in the solution. This is where cavitation would occur. In my experience, this is a much more reliable and easily understood way to present this type of information. If further understanding of the cavitation behavior is needed, then turning on the cavitation models and reconverging from that point is recommended.

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?
Yes. This is always recommended. I would generate an imbalance plot of mass, momentum and energy in the CFX solver manager. Everything should converge to 0%. This is how you ensure you have a good solution. Furthermore, I recommend plotting y-plus on the blade surfaces to ensure you are adequately capturing the turbulence. Y-plus should be low (less than 100) in these regions, or you need to further refine you mesh.
__________________
Brian Parrelli
Specialties: Turbomachinery, CFD
Professional Profile: Click Here

Do you want to become better at CFX? Sign up for my virtual course through SolidProfessor: "Introduction to ANSYS CFX" >>>
Click Here
bparrelli is offline   Reply With Quote

Old   November 29, 2016, 14:40
Default
  #9
New Member
 
Patryk
Join Date: Apr 2016
Location: Poland
Posts: 8
Rep Power: 3
FeveR is on a distinguished road
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?
FeveR is offline   Reply With Quote

Old   November 29, 2016, 17:12
Default
  #10
Member
 
Brian Parrelli
Join Date: Nov 2016
Location: Southern California
Posts: 41
Rep Power: 2
bparrelli is on a distinguished road
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.
__________________
Brian Parrelli
Specialties: Turbomachinery, CFD
Professional Profile: Click Here

Do you want to become better at CFX? Sign up for my virtual course through SolidProfessor: "Introduction to ANSYS CFX" >>>
Click Here
bparrelli is offline   Reply With Quote

Old   November 29, 2016, 17:19
Default
  #11
New Member
 
Patryk
Join Date: Apr 2016
Location: Poland
Posts: 8
Rep Power: 3
FeveR is on a distinguished road
And what about checking area on rotor blades where pressure is under 3574Pa? How to do that in CFD Post?
FeveR is offline   Reply With Quote

Old   December 2, 2016, 09:46
Default
  #12
Member
 
Alex
Join Date: Feb 2016
Posts: 79
Rep Power: 3
Red Ember is on a distinguished road
Quote:
Originally Posted by FeveR View Post
And what about checking area on rotor blades where pressure is under 3574Pa? How to do that in CFD Post?
Just have a look at CFD-Post manuals (e.g. ANSYS Help). Use isoclip.
Red Ember is offline   Reply With Quote

Old   December 2, 2016, 09:49
Default
  #13
Member
 
Alex
Join Date: Feb 2016
Posts: 79
Rep Power: 3
Red Ember is on a distinguished road
Quote:
Originally Posted by bparrelli View Post

Y-plus should be low (less than 100) in these regions, or you need to further refine you mesh.
For k-e model you mean, I suppose? I got used to SST and it easily takes 2 mln nodes for rotor blade...
Red Ember is offline   Reply With Quote

Old   December 2, 2016, 13:23
Default
  #14
Member
 
Brian Parrelli
Join Date: Nov 2016
Location: Southern California
Posts: 41
Rep Power: 2
bparrelli is on a distinguished road
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.
__________________
Brian Parrelli
Specialties: Turbomachinery, CFD
Professional Profile: Click Here

Do you want to become better at CFX? Sign up for my virtual course through SolidProfessor: "Introduction to ANSYS CFX" >>>
Click Here
bparrelli is offline   Reply With Quote

Old   December 2, 2016, 15:50
Default
  #15
Senior Member
 
Join Date: Feb 2011
Posts: 456
Rep Power: 11
Antanas is on a distinguished road
Quote:
Originally Posted by bparrelli View Post
... because it requires a very fine mesh and is not practical for many users with limited computing resources.
This is not true. SST handles fine near wall mesh, but don't require it.
Antanas is offline   Reply With Quote

Old   December 2, 2016, 16:05
Default
  #16
Member
 
Brian Parrelli
Join Date: Nov 2016
Location: Southern California
Posts: 41
Rep Power: 2
bparrelli is on a distinguished road
Quote:
Originally Posted by Antanas View Post
This is not true. SST handles fine near wall mesh, but don't require it.

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.
__________________
Brian Parrelli
Specialties: Turbomachinery, CFD
Professional Profile: Click Here

Do you want to become better at CFX? Sign up for my virtual course through SolidProfessor: "Introduction to ANSYS CFX" >>>
Click Here
bparrelli is offline   Reply With Quote

Old   December 3, 2016, 02:49
Default
  #17
Senior Member
 
Join Date: Feb 2011
Posts: 456
Rep Power: 11
Antanas is on a distinguished road
Quote:
Originally Posted by bparrelli View Post
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.
In less time? Well, not always, IMO. SST is two equation model just like k-e and if your mesh is not fine enough then SST will use wall functions as well as k-e. In this case times should be similar.
fresty likes this.
Antanas is offline   Reply With Quote

Old   December 3, 2016, 11:44
Default
  #18
Member
 
Brian Parrelli
Join Date: Nov 2016
Location: Southern California
Posts: 41
Rep Power: 2
bparrelli is on a distinguished road
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.
__________________
Brian Parrelli
Specialties: Turbomachinery, CFD
Professional Profile: Click Here

Do you want to become better at CFX? Sign up for my virtual course through SolidProfessor: "Introduction to ANSYS CFX" >>>
Click Here
bparrelli is offline   Reply With Quote

Old   December 5, 2016, 10:25
Default
  #19
Senior Member
 
Maxim
Join Date: Aug 2015
Location: Germany
Posts: 373
Rep Power: 4
-Maxim- is on a distinguished road
Quote:
Originally Posted by bparrelli View Post
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.
I wonder what Florian Menter would say to that
-Maxim- is offline   Reply With Quote

Old   December 5, 2016, 11:49
Default
  #20
Member
 
Brian Parrelli
Join Date: Nov 2016
Location: Southern California
Posts: 41
Rep Power: 2
bparrelli is on a distinguished road
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.
Red Ember likes this.
__________________
Brian Parrelli
Specialties: Turbomachinery, CFD
Professional Profile: Click Here

Do you want to become better at CFX? Sign up for my virtual course through SolidProfessor: "Introduction to ANSYS CFX" >>>
Click Here
bparrelli is offline   Reply With Quote

Reply

Tags
turbomachinery mesh cfx

Thread Tools
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 On
Pingbacks are On
Refbacks are On


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 05:59


All times are GMT -4. The time now is 07:10.