Help needed in meshing multi-stage turbine using Workbench
 

Hi all,


I want to simulate a 5-stage gas turbine. The geomerty details are a follows,

• Stage-1 -> Stator - 4 blades, Rotor - 9 blades
• Stage-2to5 -> Stator -7 blades, Rotor - 9 blades

To start with i am planning to use "Mixing Plane Model". I need some help in how to mesh the geometry (particulary defining the interfaces) and is it possible to use periodicity?

Thanks
KGN

General guide lines for simulation:

1.Either use ICEM CFD or Turbogrid (TG is recommended for its easiness) for meshing.

2.To setup case in workbench, you need to select the CFX (Or Fluent, CFX is recommended) and then input the mesh. To create the interfaces, you just need to select the corresponding inlet/outlet faces and you are done.

3.Mixing plane is available there, as well as new transient model which requires few passages.

4. You just need to model only one passage (with periodic boundaries) in ICEM/Turbogrid and you have option in CFX-Pre to select more than one passages. Mesh for other passages shall be created by CFX pre for you.

5. SST model is recommended

6. Boundary conditions >>>>>> What information is available with you?

7. Temperature dependent properties may be required to accurately model the enthalpy/temprature change from stage to stage (error is significant for 5-stage turbine)

What type of help is required in meshing? First decide you want to use ICEM or Turbogrid, because for both software route is different. ICEM requires more efforts and is useful if TG templates are not supporting geometry features you have.

Hi Far,

Thanks for the reply.
I will be using Workbench for meshing and fluent for simulation. I yet to get the boundary condition, and will update once i get.

I need some more details on periodic boundary condition, like deciding the number of passages for my case.

stage 1 -> stator-4 blades, rotor-9 blades
stage 3-5 -> stator-7 blades, rotor-9 blades

Thanks
KGN

you are talking about ansys meshing or turbogrid?

If you are going for mixing plane model, then you just need one passage from each blade row. But mixing plane model has some inherent limitation, such as it does not convect the wake from upstream rows. So if you want to see the effect of upstream disturbances from upstream rows then mixing plane is of no use. But for starters it is recommended step before going for the more complex modules.

For sliding mesh you need more passages to match the pitch of upstream and downstream components. If you decide to go for frozen rotor simulation then you shall get the solution more accurate to mixing plane model but shall be only valid to that relative position of upstream and downstream blade row. You can think of frozen rotor simulation as equivalent to sliding mesh results at some instant.

There is another model (I guess phase shift model) in CFX. http://www.ansys.com/Products/ANSYS+...ase+Highlights.
Quoting some lines here:
Also check this link:
http://www.cfd-online.com/Forums/blo...machinery.html

For meshing i ll be using Ansys workbench meshing tool, not the turbogrid.

This is irrespective of no.of blades in each stage?

Can you give some more information on how to match the pitch with an illustrative example

Thanks
KGN

Well, I don't recommend it. It may be good for fast iteration!!!!! Hexa meshing is possible in ansys meshing?

Yes, this is what it is designed for.

For example if you have 16 passages of rotor and 8 passages of stator then to match the pitch you need two passages of rotor and one passage of stator ((360/16)*2 = ((360/8)*1). For prime number, you may need to scale the some blade rows to match the pitch or go for full wheel simulation. As I already mentioned in previous post, that in ANSYS CFX V 14, you may run the transient simulation (as accurate as sliding mesh) with one passage from each blade row.

I ve to explore!

So based on the no.of blades i ve to change its angular position?

Not necessary, you just ensure that the upstream and downstream components have same axial position at the interface and have same low and high radii. Angular position doesn't matter in mixing plane. Ideally interface should be located midway between upstream and downstream components.

Any further update?

Thanks for the clarification. I am still waiting for the inputs, i ll update u once i get it.

Thanks
KGN

I trust that by angular position you mean the relative position of rotor and stator and not the sector cut for one blade.

Yes I meant the relative position of rotor and stator.

You can start your meshing with the geometry files, boundary conditions may be applied at latter stage.

i have the CAD geometry, i am trying to extract the fluid volume, then i ll start meshing.

Hi Far,

While cleaning up the geometry for extracting the fluid volume, i noticed a clearnace between the rotor blade tip and the housing. Plz c the attached picture for better understanding.

So my question is, while specfying the rotating region (rotor blade+fluid) whether we ve to include that in the fluid region or we ve separate it and specify it as stationary region.

Sorry i cant include the actual geometry because of NDA (Non-Diclosure aggrement) :(

Also can u tell what is the best strategy to extract the fluid volume

Regards
KGN

It is included.
So you have three walls : hub, blade and casing. In blade there is also wall parallel to casing that is top of blade (no wall if no tip clearance). Also you have one fluid region that includes the fluid in blade region as well as in tip region. Separate fluid regions are necessary when you are studying some stall concepts in compressor or tip recess in turbine. If needed I can provide you details how to do this.

To specify which is rotating or not rotating is done in CFX Pre. Meshing should be done in Turbogrid for each component. You should include the axial extent up to mid way between two components in .curve files.

Generally we give these boundary conditions
1. Fluid rotating.
2. hub is fixed relative to fluid (so in inertial frame it is moving, but in rotating frame is stationary). So you will not specify no motion condition for hub.
3. Blade: Same as hub
4. Casing : counter rotating wall. It is stationary in inertial reference frame but rotating in rotating reference frame, but in opposite direction.
5. Inlet: Total pressure, velocity components (normally axial =1, radial = 0 and tangential = 0 for axial inflow)
6. Outlet : static pressure.

Can u provide me some more information, it will help in preparing proposal once i get the Statement of work.

It is bit confusing, wat to specify ?

Also if u can provide me some link to multi-stage turbine both tutorial and journal paper, It will be more helpful.

Thanks
KGN

Here are some clarifications:

Actually we shall use the rotating reference frame for rotor. So instead of inertial or stationary reference frame, we are now with moving reference frame. In this reference frame (rotation speed equal to rotor and hub speed), hub and blade (we will specify them as no slip walls) are stationary and on the other hand casing is moving in opposite direction with equal speed (counter rotating wall in CFX pre).

There is no difference in handling the meshing part for single blade row, stage or multistage. There is additional specification of interface plane related to solver where we specify it as mixing plane, frozen rotor or sliding mesh depending on the requirements.

PS : We should discuss this on CFX or Fluent forum (according to forum policy we can only discuss meshing and geometry )

I am cleaning up the geometry for extracting the fluid volume. I have the solidwork model, so whats the best strategy to extract the fluid volume.

(or), we can just import the model into the workbench and then mesh the surface and fluid volume.

You should only keep the hub surface, blade and casing surface. Delete all unnecessary details related to manufacturing like bolts, shaft etc.

If you can post pic, then I can tell you exactly what to keep and what to delete!!!

Sorry I cant post the geometry, bcz of NDA(Non-disclosure aggreement) :(
I cleaned the geometry, now i have only hub, blade and casing. As i mentioned earlier there is a tip clearance between rotor blade and casing, also between stator blade and casing.
I want to the study the effect of tip clearance, So could you please explain how to mesh.

I am going to use Ansys Workbench for meshing, so whether i can directly export the geometry to the workbench or extract the fluid volume and then export only the fluid volume for meshing. Which is the best strategy?

Regards
KGN

This all can be done in Workbench Design modeler. You can put the enclosure (fluid volume) in DM.

I can send ANSYS meshing 14 tutorials if needed.


Just mesh the complete volume from hub to casing, no need to segregate the tip clearance volume from main fluid.

Could you please send me the Ansys tutorial

Thanks
Regards

Sent. check PM

Thank you very much

Regards
KGN