|
[Sponsors] |
Create a Surface between two adjacent blade in CFD-Post |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
September 2, 2020, 10:58 |
Create a Surface between two adjacent blade in CFD-Post
|
#1 |
New Member
Join Date: Apr 2016
Posts: 4
Rep Power: 10 |
Hello all,
I have simulated a flow in a centrifugal turbomachine with ANSYS CFX. The simulation is done using periodic boundary conditions, thus is done for only one blade. I would like to create a Surface starting from a Pressure suction of one blade to the suction side of the adjacent blade to display a velocity vector, however, using tools in CFD-Post, I am only able to create the surface from one periodic boundary to the next periodic boundary. I would like to ask if any one has an idea how to define a blade between two adjacent blade? Thanks |
|
September 2, 2020, 12:03 |
|
#2 |
Senior Member
Join Date: Jun 2009
Posts: 1,860
Rep Power: 33 |
Have you tried instancing the passage?
Go to your Domain, and activate instancing. Create one instance of the passage, and the surface you created will span from suction to pressure side of the instanced blade.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
September 2, 2020, 12:50 |
|
#3 |
New Member
Join Date: Apr 2016
Posts: 4
Rep Power: 10 |
Hello,
Thank you for your reply. I have tried this suggestion before and this is not working unfortunately. It just rotate the surface for one periodic angle. Attached are pictures showing the initial plane and the other is what I got doing the instance. Maybe something like Data Instancing would work but this feature is only available for Transient Blade Row simulation |
|
September 2, 2020, 15:40 |
|
#4 |
Senior Member
Join Date: Jun 2009
Posts: 1,860
Rep Power: 33 |
Do you want to visualize a plane in a radial machine? or a cylinder?
I would have created a surface of revolution instead of a plane, or a constant span surface. If you want to visualize what is happening across a rotational periodic surface a cylinder will show what is happening at a constant radius. Not certain what information you are looking for.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
September 2, 2020, 15:57 |
|
#5 |
New Member
Join Date: Apr 2016
Posts: 4
Rep Power: 10 |
Thanks for your reply.
Unfortunately I am not looking for a constant radius surface, or a surface at constant span or streamwise. What I am looking for is a flat surface that is defined with a point (at the center of passage) and a normal direction (which is in direction of the core flow in center) so that's why I need it to be defined in one passage from PS to SS. I think it can not be easily done with POST-CFD, however, I appreciate your time and reply. |
|
September 2, 2020, 17:09 |
|
#6 |
Senior Member
Join Date: Jun 2009
Posts: 1,860
Rep Power: 33 |
There is always a harder way to do things, right? Assuming it is a steady-state simulation, here is a workaround
Since you already got a converged solution (the hard work is done), you can double the model, i.e. replicate the passage in CFX-Pre and set it up with two sectors instead. Restart the solution using the single passage results and instance the solution for the initial values file, the solver will interpolate/copy the data on the passages and it should converge quickly for the two passage setup. Now create a plane across the two passages and it should work, correct?
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
September 3, 2020, 03:44 |
|
#7 |
New Member
Join Date: Apr 2016
Posts: 4
Rep Power: 10 |
Yes, I guess this suggestion plus using appropriate plane bounds might work... Will try it out but hope I can find other solution since it is a dozen of simulations Thank you for your reply.
Cheers |
|
Tags |
ansys, cfd-post, cfx, plane, vector |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Surface Heat Transfer Coefficient CFD Post | MJ1105 | Visualization & Post-Processing | 0 | February 19, 2016 04:57 |
Beginner to CFD: how to create a triangular surface in Star CCM+? | mona.16nitr | STAR-CCM+ | 2 | October 30, 2015 14:44 |
[Gmsh] Error : Self intersecting surface mesh, computing intersections & Error : Impossible | velan | OpenFOAM Meshing & Mesh Conversion | 3 | October 22, 2015 11:05 |
CFD Post Expression creation | jasonbot | CFX | 2 | July 15, 2015 06:21 |
Where's the singularity/mesh flaw? | audrich | FLUENT | 3 | August 4, 2009 01:07 |