[joshkellyjak]

Originally Posted by Sakun

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.

Can you include your config file for both these tests as well please?

[Sakun]

Hi Josh,

Many thanks for the reply,

I have uploaded 1st and 2nd meshes .cfg files as “1st mesh” and ”2nd Mesh” in a google drive folder, cause forum didn’t allow me to upload .cfg files.

Google folder link;https://drive.google.com/drive/folde...usp=drive_link

Also apologies, I have drawn periodic faces in wrong places in the previous post.
So the correct periodic faces (TOP & BOTTOM) are defined as shown in attached pictures. WALL (BACK) is defined on the right.

Thank you very much for your time,

[joshkellyjak]

Nothing immediately sticking out but I would say you should initialise your simulation first order and then restart second order. Roe + SST can be quite rigid, I don't know how Roe + SST + LM performs with the turbo stuff but try first order and see what happens. If the early divergence persists then set the volume output to once every 10 iterations or so and inspect the flow field at the final output before crashing to see where residuals are highest, this is normally the best way to debug issues with any boundaries. The output says the linear solver is diverging, so it may be a good idea to include the linear solver output in the history to see how it is behaving. You can add additional options for volume and history output using the options VOLUME_OUTPUT and HISTORY_OUTPUT respectively. Run SU2_CFD -d <your_config_here> to see all the available options. I suspect if you can run first order and restart then the case is fine, if you can't then there is a problem with your mesh.



Also please remove the option "NUM_SPANWISE_SECTIONS" it does nothing in this case.

[Sakun]

Really appreciate for all the suggestions Josh,

I was using the same .cfg file that been used for my 2D simulations, and it gave a good stability with good convergence, so I thought same would apply for 3D as well.

Sure, I follow up every suggestion, thank you very much again.

I have suspected more about the flow angle honestly, because I have never defined an angle in z-direction. In the reference paper flow inlet angle defined as 50.83 degrees So, it worked for my 2D case in xy directions (for x-direction cos alpha and y direction sin alpha), since the mesh generated in zx plane I am still bit confuse with flow definition in MARKER_GILES. At the moment it is defined as follows:

MARKER_GILES= (INLET, TOTAL_CONDITIONS_PT, 115775, 340.2, 0.0, -0.7752, -0.6316, 0.7, 1.0, OUTLET, STATIC_PRESSURE, 97251, 0.0, 0.0, 0.0, 0.0, 0.7, 1.0)

Hope this is correct.

I had a similar error like below from the mesh I made in xy plane, so is this error related to my mesh generation as well?

negative density or pressure in mixing process routine for iSpan: 71 in marker INLET

Also, any idea about my 2nd mesh error ? where y-axis is getting a zero in “Area projection, Max. coordinate, and Min. coordinate” under Geometry Preprocessing section.

Many thanks for the help.

[joshkellyjak]

The flow angle in the Giles marker is not specified using cartesian coordinates, it is specified in the frame of reference of that boundary. From config_template.cfg:

% Giles boundary condition for inflow, outflow and mixing-plane
% Format inlet:  ( marker, TOTAL_CONDITIONS_PT, Total Pressure , Total Temperature,
% Flow dir-norm, Flow dir-tang, Flow dir-span, under-relax-avg, under-relax-fourier)
% Format outlet: ( marker, STATIC_PRESSURE, Static Pressure value, -, -, -, -, under-relax-avg, under-relax-fourier)
% Format mixing-plane in and out: ( marker, MIXING_IN or MIXING_OUT, -, -, -, -, -, -, under-relax-avg, under-relax-fourier)

It should be the same in the 2D case unless you want to add some span-wise angle.

Not sure about the geometry preprocessing error but without the mesh file and some further testing with a debugger I would guess SU2 is not reading the mesh correctly. An easy way to check this would be to run for one iteration and check the volume output to see if the mesh looks as you expect. It could also just be a bug, if the volume output has the correct mesh I wouldn't be too worried about it.

[Sakun]

Hi Josh,

Sorry Josh I quite did not get by “The flow angle in the Giles marker is not specified using cartesian coordinates, it is specified in the frame of reference of that boundary.” Statement.

Basically 1st mesh in 2D created in ZY axis’s and extruded in +X direction for the 3D. since periodic faces are in top and bottom (according to the attached pictures), don’t I have to specify the inlet flow angle in -Y and -Z direction (correct me if I am wrong ) and blue arrows are angled inlet flow direction towards blade leading edge.

As for the 1st order, I could possibly think the closest one is LAX-FRIEDRICH, since Roe + SST is rigid. So can lax-friedrich go as 1st order scheme with just SST model (with no transitional model)?

Thanks for your valuable time Josh,

[joshkellyjak]

Each boundary of your mesh is defined by a surface, or in the case of a 2D mesh a line. The Giles boundary, rather than define the flow angle in cartesian frame of reference, defines the flow angle in the given surfaces frame of reference. The three components of the vector that define the flow angle are the normal, tangential, and spanwise components. Flow with a flow angle of 0 degrees would have the components (1, 0, 0) as the flow is entirely parallel with the normal vector in the boundary surfaces frame of reference. We do this as it means you do not have to spend time figuring out which way your flow needs to point at the boundary when defining the boundary condition and makes the calculation process much simpler. As such, normally it is typical to compute your flow angle in the normal and tangential directions unless you don't want the incoming flow to travel perpendicular to the blades span. The flow direction is not specified in the cartesian coordinates, it is specified in the frame of reference of the boundary surface. Please refer to my very crude sketch.

First order Roe will be fine, just disable MUSCL_FLOW.

[Sakun]

Ohhh…. I get it now, you’re a lifesaver. Highly appreciate for the explanation and everything was making sense thanks to your sketch.

(*fingers cross to my simulations)

Many thanks again, Josh

[EvertBunschoten]

Hi Sakun,

Apologies for the late reply. In the output I see that the initial velocity component in the z-direction is negative. This is probably the reason why your simulation crashes as the turbmachinery solver is unable to properly initialize.

I see that the total pressure computed at the outlet is actually higher than that at the inlet. Perhaps you should try this simulation with a pressure ramp, starting with an outlet static pressure lower than the inlet pressure and ramping to the target pressure.

I also see that the solver was able to write a volume solution file. My advice is to load it into ParaView and visualize the flow field and residuals (if they were included in the volume outputs). That way, we may be able to figure out where the high residuals come from.

[Sakun]

Originally Posted by EvertBunschoten

Hi Sakun,

Apologies for the late reply. In the output I see that the initial velocity component in the z-direction is negative. This is probably the reason why your simulation crashes as the turbmachinery solver is unable to properly initialize.

I see that the total pressure computed at the outlet is actually higher than that at the inlet. Perhaps you should try this simulation with a pressure ramp, starting with an outlet static pressure lower than the inlet pressure and ramping to the target pressure.

I also see that the solver was able to write a volume solution file. My advice is to load it into ParaView and visualize the flow field and residuals (if they were included in the volume outputs). That way, we may be able to figure out where the high residuals come from.

Hi Evert,


That’s totally fine, thank you very much for coming back,

So past few days I was trying to figure out the flow direction in the domain and how it goes around the blade (brain is fried at the moment ).



I was following josh’s suggestions on the 1st mesh and the just flow literally coming out from the HUB (attached 1st numbered Mesh pictures). Then I have re-oriented the geometry according to the flow path and started to run some simulations (2nd numbered mesh).



To identify the flow path (as josh mentioned above) , I have zeroed AOA and defined the INLET flow angle which is 50.83 to the x (0.6316) and y (-0.7752) directions.



So far 500 iterations ran without an issue but my concern is, when I look from above (PER1), the flow path angle different than from the front.


Thanks for your time for looking at this issue,