[Far]

1) To create the limit edges in order to design the same structure that shows the picture added by mAx some anwers before, Have I to create manually those boundaries (both stator and rotor) and then import them into fluent or is some automatically function/option?

yes, you can create these bounaries manually and it is much easier. However in 3d when you have twist in blade, it is difficult to make the periodice boundaries and in that case automatic meshers (turbogrid in ANSYS or turbomode in gambit) are handy to use.

T

o activate the option that the rotor blades get moving and then simulate/evaluate what happen, for instance, with temperature through the set, this is in fluent right?

Yes this is done in Fluent.
There are three options to model rotor stator interaction (some more are also added in CFX)
1. Multiple reference frame: (aka frozen rotor ) This model will model turbomachinery simulation in steady state manner. It is accurate and will convecte wakes and other non linearities in flow as it is. But the problem is that it gives you solution for that particular relative position.

2. Mixing plane (aka stage model). It is steady state model. It averages parameters at interface (mixing plane, typically at mid of both components) and it is its strong and weak point. It is strong point in a sense that you need one blade passage from both rows and at design conditions it gives very good solution. But it can not model the wake boundary layer or wake shock effects in downstream component as everything is averaged at interface

3. sliding mesh: this is true unsteady model. It includes all effects you would get in turbomachinery except the approximation you will have due to turbulence modeling. It is accurate but reqires equal pitch on both sides and you may end up modeling the full blade row on both sides and it makes it tough on computer memory, cpu and time it takes to solve.

Just to give an example of difference in mixing plane and siding mesh requirements. I have solved rotor stator 3d model with around 1 million mesh nodes and it takes around 12-18 hours to converge. But the 2d case (0.112 million nodes) it takes me around 4-6 days to get meaningful results

3) Then... Have I to create the blade cascade in Gambit and then export to Fluent or using this last one there is an option to duplicate your blades (either rotor or stator)?

No need to create real cascade in gambit or fluent (7 - 9 blades in cascade tunnel), this is where periodic boundaries come to rescue you. It will give same effect including bleed, boundary suction etc.

4) Is it possible to export to fluent two diferent geometries (since rotor and stator blades are differents) comming from two different gambit files? (To create the same layout that the image before)

Yes and it is the standard procedure unless you need conformal mesh in both components to model the turbo-machinery frozen rotor mode. Even for that case, non-conformal mesh is sufficient/accurate to get the same results.

you have to import them in Fluent, but watch out in the picture it seems to be sliding mesh (Far should correct me). That means you will import 2 separated fluid domain with 2 interfaces (one interface per domain)

This is prerequisite for sliding mesh model.

Yes in fluent. Far should tell me more about sliding mesh /SRF / MRF (I only know sliding mesh)

Periodicity should help
Far is experienced in this area

Yes for cascade there is no need to model all 7 or 9 blades. Only thing is that you need translational periodic boundary condition.

4) yes it is: http://aerojet.engr.ucdavis.edu/flue...e171.htm#20871[/QUOTE]

[zobydusantos]

Dear -mAx- and Far,

I have been busy working in my thesis during this last month and I wanted to tell you my most sincerelly thanks for your help!! It was really helpful, and with all of your information I could solve all my doubts!!

Sincerely, thanks for help the people via internet! It was a pleasure.
A greeting!

[SAJADHUSSEEN]

Originally Posted by zobydusantos

Hello,

Currently I'm doing my Master thesis about the fluid behavior through an Axial Gas Micro Turbine and I'm trying to reproduce one physic prototipe (with its specific parameters) using Gambit (Geometry and Mesh). I'm following the tutorial "Basic Turbo Model with Unstructured Mesh" since I need to represent in 3D the model and generate in 2D the surface in order to study the changes of differents parametres through the rotor and the stator.

The problem is when I generate the turbo and I want to define to control volume appears that message

"ERROR: ACIS error 8030: inconsistent face-body relationships. A valid flow volume could not be constructed. Ensure that a valid turbo profile has been constructed with mean edges and hub and casing edges. Geometric modifications of this data, including vertex slides or edge repositioning, may be required for a succesful flow volume construction."

Of course I understand the message but I don't already know what more can I try to do. Any idea?

BTW: In the beginning I had one problem that shows this message: "Ensure all blades/splitter section tip vertices are connected to only 2 edges" and, only for it useful for someone, that means that it is impossible to use turbo model if each vertex has associated more than two edges, i.e., take care if you have something hidden. That was my mystake.

PS: I attached the pictures of what I want to do/get and the step where I have the problem with the error mentioned above (mine and the same steps of tutorial). My last picture it seems that Gambit generate the volume control but it is only a Screenshot, automatically then disapears.Attachment 22849

Attachment 22850

Attachment 22851

Attachment 22852

Hello
we need the file turbo-basic.tur which is used in the tutorial of turbo model. I do not have this file in my gambit help.I will be very thanks for help

[-mAx-]

check here:
https://www.sharcnet.ca/Software/Gam...s/tutfiles.htm