[knixxor]

Hi guys,

I would like to set-up a 3 stage compressor flow with ANSYS CFX. The rotor speed is 3800 rev/min. My task is to calculate the compressor performance. I am struggeling with the setup of the interfaces and domains and I hope you could help me with this.

I have set the parameters as follows.

Inlet: P-Total= 101325 Pa
Outlet: P-static=170000 Pa
k-e Turb model



My questions are:

• What is the most common approach the simulate a compressor flow in terms of the numerical setup with CFX?
• Is it reasonable to use the fan stator blade as the first passage of the compressor? I did this because the inlet, which is now in a stationary frame and thus the high velocity components at the subsequent 1st rotor would have no effect for the inlet
• Which inital guess for the P-static @ outlet BC would you recommend me? Im still struggeling with too high Mach Numbers and simulations errors
• Do you have any tips for the pitch change? I am not sure if "automatic" is valid for this simulation.
• The mesh size of each component is around 500000-800000 nodes. Is this a reasonable size or should I refine/coarse the mesh?
• I have attached a screenshot for this question: When I set up the compressor in CFX for the first time, I noticed that all rotor passage faces are not aligned with the stator faces. Therefore, I set 2 instances for the rotor passages. Is the a common way for a compressor flow setup? Would you suggest an other setup?

Thank you for your help

[ghorrocks]

I am not a turbomachinery expert but I will answer what I can:

What is the most common approach the simulate a compressor flow in terms of the numerical setup with CFX?

Look at the CFX tutorials. There are several which do turbomachinery.

Is it reasonable to use the fan stator blade as the first passage of the compressor? I did this because the inlet, which is now in a stationary frame and thus the high velocity components at the subsequent 1st rotor would have no effect for the inlet

You need to simulation what you intend to model, obviously. So it sounds like you need it.

Which inital guess for the P-static @ outlet BC would you recommend me? Im still struggeling with too high Mach Numbers and simulations errors

Read the CFX documentation on "Tips for obtaining convergence", especially the section on choice of boundary condition and the best practises guide for turbomachinery.

Do you have any tips for the pitch change? I am not sure if "automatic" is valid for this simulation.

Again - refer to the documentation for a definition of pitch ratio. Have a look to see if the pitch ratio is being calculated correctly by the automatic option. If it is, then you are fine.

The mesh size of each component is around 500000-800000 nodes. Is this a reasonable size or should I refine/coarse the mesh?

You need to do a mesh size sensitivity study to establish whether this is sufficient. You cannot tell by simply the total node count.

I have attached a screenshot for this question: When I set up the compressor in CFX for the first time, I noticed that all rotor passage faces are not aligned with the stator faces. Therefore, I set 2 instances for the rotor passages. Is the a common way for a compressor flow setup? Would you suggest an other setup?

Nothing is attached and I do not understand the question.

[bparrelli]

My answers to your questions are in red below:

Originally Posted by knixxor

Hi guys,

I would like to set-up a 3 stage compressor flow with ANSYS CFX. The rotor speed is 3800 rev/min. My task is to calculate the compressor performance. I am struggeling with the setup of the interfaces and domains and I hope you could help me with this.

I have set the parameters as follows.

Inlet: P-Total= 101325 Pa
Outlet: P-static=170000 Pa
k-e Turb model



My questions are:

• What is the most common approach the simulate a compressor flow in terms of the numerical setup with CFX? Single passage, steady state with stage interfaces between each rotor and stator. Inlet and outlet boundaries depend on the problem, but what you have should be ok. I'd recommend going with a small subsonic pressure ratio to start with as an initialization. Then restart the convergence from that point.
• Is it reasonable to use the fan stator blade as the first passage of the compressor? I did this because the inlet, which is now in a stationary frame and thus the high velocity components at the subsequent 1st rotor would have no effect for the inlet. This is probably ok, but keep in mind that if the flow coming into the stator is non-uniform, then you will either have a difficult time obtaining convergence or not obtain a good solution. The best way to is add a long straight inlet volume upstream of the first stator, as this will guarantee the uniformity of the flow into the stator is unaffected by the inlet boundary.
• Which inital guess for the P-static @ outlet BC would you recommend me? Im still struggeling with too high Mach Numbers and simulations errors. I assume you have a mass flow in mind for these conditions? You can try specifying mass flow at the discharge, but it can be finicky sometimes. Probably the most robust way is to use "opening" boundary types to start with just to get a sense of what the flow is doing. Then change them to inlets/outlets. But inlet total/outlet static should be ok. The key is baby steps in terms of the pressure ratio. Dial it up gradually and reinitialize in successive iterations.
• Do you have any tips for the pitch change? I am not sure if "automatic" is valid for this simulation. This is fine. CFX knows how to interpolate the solution from one domain onto the next based on the area. If the areas don't match (eg. different passages size due to different number of stators/rotors), CFX will average the solution based on the areas at the stage interface.
• The mesh size of each component is around 500000-800000 nodes. Is this a reasonable size or should I refine/coarse the mesh? For a structured turbo mesh (I assume you used Turbogrid?) the general recommendation is 250000-500000 elements per passage depending on the level of turbulence. You definitely should plot yplus on the blade surface of your solution and make sure it's reasonable (less than 100). This will ensure your mesh quality is good.
• I have attached a screenshot for this question: When I set up the compressor in CFX for the first time, I noticed that all rotor passage faces are not aligned with the stator faces. Therefore, I set 2 instances for the rotor passages. Is the a common way for a compressor flow setup? Would you suggest an other setup? This doesn't matter at all. As long as the meshes are all rotating about the same axis, CFX will interpolate between the blade rows correctly. You only need one passage per blade row, and CFX will account for the mass balance of the full 360.

Thank you for your help

[bparrelli]

If you are interested in getting better at CFX, I would recommend signing up for my course at Solid Professor. https://app.solidprofessor.com/lmsap...20/lessons/501

[knixxor]

Thank you guys,

I will take your tips into account for the setup. However, maybe you can help me with another issue regarding a similiar setup.

In addition, I have to simulate the flow through the fan + compressor and bypass as well. Of course, the fan blades, the splitter (bypass flow) geometry are larger than the compressor blades. And now I am struggeling with the meshing of all components. I have meshed all blades with TurboGrid and in TG they look fine for me. But when I put all blades + splitter together in CFX they are great differences in the mesh sizes. The fan blade is round about 10 times larger than the compressor blades, which means the mesh cells of the fan and the compressor blades have a 10:1 ratio and I think this will definitely lead to numerical issues. The splitters is meshed with ICEM and in the global view it has nearly the same size as the fan blade domain.

What is the common way to connect large and small geometries? Should I refine the fan blade mesh and the splitter in order to get the same cell-size in global? If yes, I would have a extremely fine mesh for the fan and a medium mesh for the compressor. Or it is ok for CFX to have great differences of the mesh density in one simulation?

Can you follow my question? I would be rather happy, if you can help with this.

[bparrelli]

This is a very good question, and the answer is "it depends". Since you are already using a stage interface, the rotor/stator interaction is captured, but depending on the spacing between the blade rows, the relative mesh densities can have anywhere from a minimal to a significant impact. Since you will have vortex shedding after each blade row likely bleeding into the interface, my recommendation would be to build a small stationary volume (between the large and small rows) that you can mesh independently using ANSYS meshing or ICEM. That way you can control the density in and out to match what you have from turbogrid without sacrificing too much in terms of computational cost. Does that make sense?

[knixxor]

Originally Posted by bparrelli

This is a very good question, and the answer is "it depends". Since you are already using a stage interface, the rotor/stator interaction is captured, but depending on the spacing between the blade rows, the relative mesh densities can have anywhere from a minimal to a significant impact. Since you will have vortex shedding after each blade row likely bleeding into the interface, my recommendation would be to build a small stationary volume (between the large and small rows) that you can mesh independently using ANSYS meshing or ICEM. That way you can control the density in and out to match what you have from turbogrid without sacrificing too much in terms of computational cost. Does that make sense?

Thank you, yeah it definitely makes sense. The stationary volume, you mentioned above, exists already. I have attached a sketch of the setup. As you may see, the splitter domain connects the fan blade with the compressor and provides the bypass outlet. If I understood you correctly, I will have to re-mesh the splitter coming with a coarse mesh from the fan and ending with a fine mesh at the fan stator inlet?

[bparrelli]

Originally Posted by knixxor

Thank you, yeah it definitely makes sense. The stationary volume, you mentioned above, exists already. I have attached a sketch of the setup. As you may see, the splitter domain connects the fan blade with the compressor and provides the bypass outlet. If I understood you correctly, I will have to re-mesh the splitter coming with a coarse mesh from the fan and ending with a fine mesh at the fan stator inlet?

Yes, I think this would be the best way to minimize any numerical errors between the blade rows. Just make sure your wall boundary layer refinement at the hub and shroud is consistent between the fan and stator.

[knixxor]

Okay, perfect. Thank you for your help .

Before I start meshing: In my opinion, creating an unstructured mesh would be a better option to take the gradient in mesh density into account. Am I correct?

[turbo]

Originally Posted by knixxor

Okay, perfect. Thank you for your help .

Before I start meshing: In my opinion, creating an unstructured mesh would be a better option to take the gradient in mesh density into account. Am I correct?

The single CFD shot of your turbofan compressor domains will require a lot of computing resources because of required mesh quality. One bottom line is to keep the similar mesh density near all of the endwalls including the fan and bypass passage for an acceptable yplus, and also at every interface of different domains. One tip is to allow quite larger cells away from walls in the inlet, fan and bypass to save resources. You need to get a smooth transition from fine to coarse grids, of course.