[Sakun]

Hi,



I am running the 3D model of my previous case as mentioned in this thread Bad Match Turbomachinery. It is an infinite blade so I just extruded in the z-direction (spanwise direction) by 100 layers. 2D case was well converged but 3D case just failed without a proper error explanation. I have attached the console outcome in the txt file (info.txt file).



By the information from it, I am not quite sure is it because of the negative minimum orthogonal angle.


Much appreciate for the help.

[bigfootedrockmidget]

How large is your mesh now? Can you monitor the memory consumption while it runs?
It might be that you just start to run out of memory and the linux memory manager decided to kill the process.

[Sakun]

Hi bigfoot,

Well coarse mesh size around 6 million. Tried to run in my laptop before running in the cluster so that I can confirm my .cfg file would work without an issue.
Basically, my laptop has 14 physical cores and 16 GB of RAM.

[bigfootedrockmidget]

A 2.6M elements case on my machine used between 12G and 14G of memory, so I do not think you would be able to run a 6M cell case with 16Gb. Maybe you can run first with 10 layers as a test.
But a negative orthogonal angle also does not sound correct.

[Sakun]

Hi,

So I was trying to run the case in the cluster for 10 iterations but after 6min later I got this “nan in mixing process routine for iSpan: 75 in marker INLET” and then “SU2 has diverged (NaN detected)” error. (error was repeated for 128 times, i had to delete some lines to reduce the file size) No data were recorded in the “History.csv” as well.

I have attached the full console details with this reply.

[EvertBunschoten]

It looks like there are some warnings in the output regarding the mesh quality when loading the geometry:

There has been a re-orientation of 2079 HEXAHEDRON volume elements.
>>> WARNING: 4225 HEXAHEDRON, volume elements are distorted.
It was not possible to determine if their orientation is correct.
There has been a re-orientation of 88 QUADRILATERAL surface elements.
>>> WARNING: 38 QUADRILATERAL surface elements are distorted.
It was not possible to determine if their orientation is correct.

This may be the cause of the problem. Can you run one iteration at a very low CFL and check the volume output? Perhaps there you may be able to find out which areas in the domain are problematic.

[Sakun]

Hi Evert,

Really appreciate for the reply,

I am using ansys ICEM to generate the mesh, so in order to define periodicity I have to use vertices method. After applying that method edges that associated with vertices would incline and mesh cell become skewed (attached a picture with white arrows).

To tackle this, I have merged couple of blocks from top and bottom (merged blocks and mesh attachment) and applied tri/hex mesh cells. Then tried to run 1 iteration in the cluster and I got an error (simulation_update attachment).

[EvertBunschoten]

The error you get now is related to your boundary conditions. It means that not all outer surface elements in your mesh file have been assigned a boundary condition. Make sure that when generating your mesh file in ICEM all outer surfaces have been assigned to a named selection.

[Sakun]

Hi,

I just went back to the 2D mesh, where I didn’t do any treatments for inclined mesh cells and ran 5000 iterations without an issue (attached 2D simulation output file).
So I used the 2D mesh to create 3D mesh where I just transform both geometry and blocks to the spanwise direction (+Z direction). Then I got and error called “nan in mixing process…….” (attached 3D simulation output file with the error). Also, i made sure proper edge, vertices association and mesh allocation done for both 2D and 3D before running the simulation.

Many thanks for your help and time.

[EvertBunschoten]

Hi,
Three things:
1: As of yet, SU2 assumes the axial flow path to go in the +Z direction. We are working on making the axial flow path more general, but this is still in early stages. Therefore, your mesh should be oriented accordingly. If you have a 2D mesh defined on the XY plane and extrude it in the Z direction, SU2 still assumes a +Z axial flow path, which may be the reason why your simulation crashes in 3D.



2: Even though your 2D simulation runs, it doesn't seem to converge very well (residual of > +1.0 is not desirable). If you include RESIDUAL in the option for VOLUME_OUTPUT in your configuration file and visualize the volume field in your post-processor of choice, you can locate the areas where SU2 has trouble converging.


3: My advice is to use Ansys TurboGrid for the mesh generation rather than ICEM. TurboGrid generates meshes dedicated for turbomachinery applications and is less prone to user error than ICEM is (saves you a lot of time too).

[Sakun]

Hi,

At the moment I am using following settings in the .cfg file (3D_sim.txt file). I guess 3D turbomachinery flow simulation possible in SU2 right ?, cause i have seen some people have published similar cases to mine with 3D simulations and seen in the SU2 conference videos as well.

I have specified 3rd axis faces as BACK [ MARKER_HEATFLUX= (BLADE, 0.0, BACK, 0.0 ) ] and FRONT [MARKER_SYM= ( FRONT )] .
Do I have to add anything special to define the flow direction ? or 3rd axis.

Yeah, I am figuring out TGrid at the moment, it is bit confusing to learn that. hopefully I will be able to.

Thanks for the advice on the convergence and your time spend on this,

[EvertBunschoten]

Hi Sakun,


3D turbomachinery simulations are definitely possible in SU2. You need to make sure however that your mesh is oriented correctly. Here, the rotation axis of the machine should be the z-axis. If that's not the case, rotate your mesh accordingly before initiating the simulation. The z-axis is currently hard-coded in SU2 to be the rotation axis for 3D simulations.
From my understanding, you took a 2D blade mesh defined on the xy plane and extruded it in the z-direction to generate a 3D mesh. This will not work in SU2, for the reason I mentioned earlier. If you switch the x- and z- coordinates of the nodes in the mesh file, I suspect your simulation will run much better.

[joshkellyjak]

Originally Posted by Sakun

Hi,

At the moment I am using following settings in the .cfg file (3D_sim.txt file). I guess 3D turbomachinery flow simulation possible in SU2 right ?, cause i have seen some people have published similar cases to mine with 3D simulations and seen in the SU2 conference videos as well.

I have specified 3rd axis faces as BACK [ MARKER_HEATFLUX= (BLADE, 0.0, BACK, 0.0 ) ] and FRONT [MARKER_SYM= ( FRONT )] .
Do I have to add anything special to define the flow direction ? or 3rd axis.

Yeah, I am figuring out TGrid at the moment, it is bit confusing to learn that. hopefully I will be able to.

Thanks for the advice on the convergence and your time spend on this,

You should remove the option NUM_SPANWISE_SECTIONS.

Maybe add some more linear solver iterations to help the solver out in the early iterations where your solution is crashing.

Is this geometry representative of an experimental case? Your outlet static pressure is lower than the inlet total pressure for a compressor case, but I'm not sure if the inlet static pressure would be lower at the inlet than the outlet (i.e. is it compressing?)

Try running first order ROE first and restarting, or using JST. JST can be a bit more stable in some cases.

[bigfootedrockmidget]

If only we had a couple of tutorials that shows the correct/preferred settings :-)

[joshkellyjak]

Originally Posted by bigfootedrockmidget

If only we had a couple of tutorials that shows the correct/preferred settings :-)

I have been assured they are on the way

[Sakun]

Originally Posted by EvertBunschoten

Hi Sakun,


3D turbomachinery simulations are definitely possible in SU2. You need to make sure however that your mesh is oriented correctly. Here, the rotation axis of the machine should be the z-axis. If that's not the case, rotate your mesh accordingly before initiating the simulation. The z-axis is currently hard-coded in SU2 to be the rotation axis for 3D simulations.
From my understanding, you took a 2D blade mesh defined on the xy plane and extruded it in the z-direction to generate a 3D mesh. This will not work in SU2, for the reason I mentioned earlier. If you switch the x- and z- coordinates of the nodes in the mesh file, I suspect your simulation will run much better.

Hi Evert,

Many thanks for the reply and confirmation,

Yeah that’s the method I have used but I have simulated a 3D airfoil case using the same method (2D mesh defined on the xy plane and extruded that in the z-direction to generate a 3D mesh) and simulation ran without an issue for 30000 iterations and got well converged as well (attachment).

I suspect something wrong in the mesh, like highly skewed mesh cell.

[Sakun]

Originally Posted by joshkellyjak

You should remove the option NUM_SPANWISE_SECTIONS.

Maybe add some more linear solver iterations to help the solver out in the early iterations where your solution is crashing.

Is this geometry representative of an experimental case? Your outlet static pressure is lower than the inlet total pressure for a compressor case, but I'm not sure if the inlet static pressure would be lower at the inlet than the outlet (i.e. is it compressing?)

Try running first order ROE first and restarting, or using JST. JST can be a bit more stable in some cases.

Hi Josh,

Appreciate for the suggestions,

I have tried every suggestion one at a time and had the same error (error message attached).

So this case from a journal paper (yes, it represent both numerical and experimental case ) to use for validation (paper values are attached ). I have calculated the INLET static pressure using INLET total pressure, Mach number and OUTLET static pressure.

[EvertBunschoten]

Originally Posted by Sakun

Hi Evert,

Many thanks for the reply and confirmation,

Yeah that’s the method I have used but I have simulated a 3D airfoil case using the same method (2D mesh defined on the xy plane and extruded that in the z-direction to generate a 3D mesh) and simulation ran without an issue for 30000 iterations and got well converged as well (attachment).

I suspect something wrong in the mesh, like highly skewed mesh cell.

This mesh orientation (2D xy, extruded into the +z-direction) is fine for any simulation OTHER than turbomachinery simulations. The moment you define a turbomachinery simulation in SU2 (through MARKER_TURBOMACHINERY), SU2 will assume the z-axis to be the axis of rotation and your current set-up will not run properly.

[Sakun]

Originally Posted by EvertBunschoten

This mesh orientation (2D xy, extruded into the +z-direction) is fine for any simulation OTHER than turbomachinery simulations. The moment you define a turbomachinery simulation in SU2 (through MARKER_TURBOMACHINERY), SU2 will assume the z-axis to be the axis of rotation and your current set-up will not run properly.

Hi Evert,

So I have to recreate my 2D mesh in zx axis (previously xy axis) and extrude in +y direction (previously +z direction) for 3D mesh (correct me if I am wrong). And leave the .cfg as it is or do I have to do some changes to that as well.

Thanks for your valuable time,

[Sakun]

Originally Posted by EvertBunschoten

This mesh orientation (2D xy, extruded into the +z-direction) is fine for any simulation OTHER than turbomachinery simulations. The moment you define a turbomachinery simulation in SU2 (through MARKER_TURBOMACHINERY), SU2 will assume the z-axis to be the axis of rotation and your current set-up will not run properly.

Hi Evert,

I have created 2 types of meshes where rotation axis to be in z-direction.

1st mesh was created in ZY plane and extruded in x direction for the 3D (wide mesh).
2nd mesh was created in ZX plane and extruded in Y direction for the 3D (Tall mesh).

With the 1st mesh tried to set up the simulation with suitable inflow angle but it crashes after few iterations with an error saying negative density or pressure in mixing process routine for iSpan: 70 in marker INLET (attached the error file, named 1st Mesh).

2nd mesh gives a different sort of error (error file attached, named 2nd Mesh). Apparently it does not read y-axis cells/geometry components (correct me if I am wrong), zero is shown in the y-axis at “Area projection, Max. coordinate, Min. coordinate”, under Geometry Preprocessing section.

I think 2nd mesh is appropriate for the simulation my understanding, but I don’t know why y-axis isn’t reading by the solver.

Highly appreciate if you can help me on this.