In this week’s blog post we are looking closer at features for turbomachinery which can be (extra) useful when running simulations for one section. In the newest version of Simcenter STAR-CCM+, version 2210, structured meshing for turbomachinery was introduced. Turbomachinery has been a hot topic at Siemens for a while now, introducing many features and also the turbomachinery workflow. Now, structured meshing is also introduced, which is something that hopefully many users will benefit from in their daily simulation work. This week we will also look at some post-processing tricks which might be helpful when your sector analysis (or rotating machinery simulation) is calculated.
Structured meshing in Simcenter STAR-CCM+
Structured meshing is popular to use when it comes to sector analyses for turbomachinery. Using structured meshing, when having flow that is aligned with the mesh cells, induces less numerical diffusion. Also, structured meshing requires less cells to discretize the computational domain, which makes the simulation quicker to run and requires less RAM.
With the new Turbomachinery mesh operation, you specify the surfaces in the picture below. Blade tip surface is optional to specify and should only be specified if you have a tip gap clearance. The other surfaces are required as input. If you have a radius in the transition from the blade to the hub/shroud surface you should include the radii surfaces in the input for Blade surface. The mesh operation supports dynamic queries.
For the mesh settings you specify the Near wall thickness (first cell thickness in the fluid domain counted from the wall) together with the number of cells in the specific direction. So, in the axial direction (named Blade parameters) you specify the number of cells from inlet to outlet, and in the radial direction (named Spanwise settings) you go from the hub (inner-most surface, closest to the rotational axis) to the shroud (the outer-most surface from the rotational axis). When defining mesh settings between the periodic surfaces (named Pitchwise settings) you only specify the number of cells and not the near wall thickness since you do not need finer cells on the periodic boundaries. See picture below for how a structured mesh using turbomachinery mesh in Simcenter STAR-CCM+ can look.
When working with simulations that involve blades or guide vanes you usually plot your mesh or fluid properties on a meridional, spanwise or pitchwise coordinate. If we take the spanwise coordinate as example, this means that you typically want to normalize the distance between the hub and the shroud from 0 to 1. For example, in this way a span coordinate of 0.5 is always at the plane that in all locations are in the middle of the hub and shroud. One way of creating spanwise plots in Simcenter STAR-CCM+ is to use a Block-mapped coordinate system. Create a block–mapped coordinate system, like in the picture below, and set up:
- Umin = inlet
- Umax = outlet
- Vmin = periodic boundary 1
- Vmax = periodic boundary 2
- Wmin = hub
- Wmax = shroud
Use this coordinate system in a derived part of type isosurface, where you use the fluid region of interest, and as the field function “Name_of_block-mapped_coordinate_system: Wmin to Wmax” at a spanwise coordinate (for example 0.5 for the middle span). The definition of the spanwise coordinate can be set as a parameter so that you easily can change this value, and there is also a possibility to define the isosurface with a number of isosurfaces at a range. See picture below for a velocity plot at five spans, [0.1, 0.3, 0.5, 0.7, 0.9]. Note that the spans are not at a constant y-coordinate.
One additional visualization of results that is commonly used in turbomachinery is plotting values at the blade, on a specific span, which is normalized in length from 0 to 1 (from leading edge to trailing edge). The plot can for example show the pressure coefficient around the blade at span 0.5, which will be described how to visualize in this section of the blog post.
We will use the same approach as in the previous section, creating an isosurface to plot values on, but this time we will use the blade surface instead of the region as input part. The value specified at the isosurface will correspond to the spanwise coordinate you want to look at. You will now obtain an isosurface that is a line on the blade at your span.
We will need reports that extract coordinate values in U-direction in the block-mapped coordinate system. To do this, set up minimum and maximum reports for the block-mapped coordinate in U-direction (from inlet to outlet, since we want to look at results from the leading edge to the trailing edge). Use the isosurface line as input part.
Create an XY-plot for the isosurface line. Both the X and Y type should be scalar, the default X type is direction so that needs to be changed. The X type scalar function should be your normalized length that goes from 0 to 1 (later named as the field function Normalized_plot_dimension_length in this example). The scalar function for Y types will be pressure coefficient in this example, since you are usually looking at a pressure value on the blade for these kinds of plots.
Four field functions are needed when using this approach. So, first you have to set up one field function that extracts the value (position) from the maximum report of the blade in the block-mapped coordinate system, see picture below for definition.
The next field function returns the minimum value of the coordinate of the blade in the block-mapped coordinate system, see picture below for definition.
The next field function calculates the length of the blade section in the block-mapped coordinate system, based on the two first field functions.
The fourth field function gives you the normalized coordinate in U-direction in the block-mapped coordinate system.
Now you are ready to view your plot and analyze your blade profile, see picture below for an example of what the resulting plot can look like.
Note that it is the technique (one of many) of how to create this plot that is important in this example, not the values that are presented in the graph.
We at Volupe hope that this blog post has been interesting, and that you will get a lot of use of the structured meshing and the tips presented in this blog post. If you have any questions or comments, you are always welcome to contact us at email@example.com.
Christoffer Johansson, M.Sc.