Problem with FlowPath and ExportPoints
 

Hi.

I am trying to define the flow path for a radial turbine blade, but without success. I am not sure how this feature works, it seems like it is axis dependant. I define the hub, shroud, inlet and outlet of the blades as lines, but I get an error message when I try to generate the FlowPath ("Error: Failed to generate because of invalid property/properties. Context: ansFClientBMBladeDesign: :Execute FlowPath4").

I have managed in some cases to create a FlowPath, but when I try to export the points I have problems generating the feature as well. The points can be exported when I turn off all the layers created in the flow path, but then I think don't have enough data to continue to turbogrid (get error message in turbogrid: Blade number is out of range)

I have tried to use tutorials online, but it doesn't work if I try to do the same or similar. Can anyone please explain to me how these features work, and what might be the cause of these problems I am having? After exporting the points, the plan is to make the mesh in turbogrid.

Thanks in advance.

stay positive
 

When using BladeModeler in DM, to define the FlowPath feature, the turbine axis must be the Z axis.

Arrange your geometry so that the outlet of the turbine points towards the -Z axis. Now change your view orientation to look at the +Z axis.

If a blade passes through the XZ plane (on the +X side), remove the blade from the geometry by deleting the faces associated with them. If not, continue to the next step.

Slice the turbine with the XZ plane and hide the lower body, leaving only the top half of the wheel. Create a new plane on the XZ plane.

With the new plane selected, insert a sketch projection of the flow path area (the cross section face you just created by slicing the wheel in half) to define the absolute edges of the hub, shroud, inlet and outlet.

Create a new sketch (for the hub profile) on the new plane, and duplicate the line segments that make up your hub profile from the previous sketch projection.

Repeat this for the shroud, inlet, and outlet.

Create the FlowPath feature using the new four sketches that define the flowpath.

Create the ExportPoints feature by using the FlowPath feature and selecting the blade surfaces closest to the +X axis (making sure that they don't intersect the XZ plane!).

Linking the Geometry cell to the TurboGrid cell in Workbench will then begin your process of creating a structured mesh between the blade passages.

Hope this helps. If you need further clarification, don't hesitate to ask.

Thank you for a good reply. I am not sure I understand one step correctly, can you please explain this a little further:

In the figure attached you can see that the blade passes through the XZ plane, but I am not sure what you mean by removing the blade from the geometry.

It looks like you are using the solid geometry of the blade...

I have only had success using the FlowPath feature when using the water volume geometry (the negative volume solid of the turbine solid model).

Can you confirm what you are using as the geometry?

yes, I am using a solid model. What is the best way to make a negative volume of the blades?

If you have a solid model of the turbine, create a solid model of the flowpath volume (sketch inlet, shroud, inlet, outlet, then revolve to create 3D geometry), then remove the turbine geometry from the flowpath volume geometry - I usually do this in my native CAD (SW) program before bringing into DM.

Maybe if I describe better what I am doing it will be easier for you to help me, since I am not sure how to use negative volume in this case.

I have data that includes xyz coordinates for points on 10 different surfaces. These points are imported into designmodeler and 3D curve used to spline each section of the blade.
From there I use skin to generate the blade sides and surfaces from edges to close the hub and shroud.
Then I create a solid part with body operation.

I used to generate the flow path from here, by projecting the blade on the XZ plane and defined the inlet, outlet, hub and shroud in that plane with sketches. The inlet and outlet ducts are very simplified and only temporary.

The flow path operation seems to work with this method but I get an error when I try to export the points.

Since I am trying to avoid drawing up the whole geometry (don't have access to any good CAD software) and only simulate one blade passage, is there any easier way to do this?

Do you think it is possible to do this in a similar to what I have been doing?

If CAD modelling is the easiest way, can you maybe describe it a bit better? Do you import the whole turbine to DM, just one passage or do you only import the fluid volume (negative volume?)?

I understand what you are trying to do, but I have not tried this approach before.

My suggestion would be, while in DM, pattern your blades based on the number of blades in the turbine. Create another body (I will refer to it as the "fluid body") by revolving a defined sketch containing the hub, shroud, inlet and outlet profiles around the correct axis.

(At this point, you should have a solid body for all the blades, and a solid body of the fluid space)

I am not incredibly familiar with all of the features of DM but it uses the same modelling kernal as SolidWorks, so there should exist a feature that you can remove one body from another. Refer to DM Help & Tutorials on how to do this.

Remove all of the blade bodies from the fluid body to create the "negative" or fluid space of the turbine, and then follow my earlier instructions.

[Q] "Since I am trying to avoid drawing up the whole geometry (don't have access to any good CAD software) and only simulate one blade passage, is there any easier way to do this?"

[A] The FlowPath & ExportPoints feature will create a single blade passage (fluid space around one blade) and be available as an export to TurboGrid, where it can be meshed with high quality.

Hope this helps!

I think I have followed what you suggested, but I am still having problem with exporting the points (Error message: failed to generate the export data). Is it correct to select the surfaces of the blade closest to X+ axis that does not intersect the XZ plane? I use the freeze feature to be able to select the blade surface, and select the whole blade: hub, shroud and the sides of the blade. A figure is attached, showing the blade and geometry I am using. Decided to try it on the guide vanes as the geometry is simpler.

Appreciate your time and patience!

Make sure you are always working with the positive axes. From your image, it looks right, but you should be selecting the blade between the +X and +Y axis, not the +X and -Y. Hopefully that makes the difference.

I'm not sure why you need to use the Freeze feature, you should be able to select the blade surfaces, as the edges of the blades should extend to the hub and shroud. If your blade doesn't intersect the hub or shroud, that could also be why it isn't working. You can adjust the hub/shroud offset to a higher value, which may help in that case.

Progress?
 

I think I have made some progress, I don't get an error for the flowpath nor export points (errors on flowpath before probably due to some open curves, not sure what caused errors in export points, but the distance of the inlet/outlet from leading/trailing edge seems to be important as well as hub/shroud offset), but the geometry of the blades is not correct when imported to turbogrid, see the attached figures. Any idea what is going on here?

I was watching once again a video from "turboengineer" on youtube (https://www.youtube.com/watch?v=0Qmm9sKQaFc#t=406), and noticed for the exportpoints feature that the option "hub and shroud from" is not available in my case, even though it seems like I am using the same version of Ansys. Any idea why this is not identical?

How many layers do you use in your FlowPath feature? It is hard to say what the issue is without having the geometry.

I have tried a wide range of layers, from the two default for the hub and shroud up to 8 additional layers.

It looks like the blade gets distorted when the flowpath is too close to the shroud, as seen in the figures attached. Any idea how to fix this? The problem seems to start at the trailing edge and the geometry of the blade becomes far from what it should be..

I have the 5 solid blades on solid works...How can I generate the flow path on solid works? please

Try to help me to make this in solidworks..I am stuck.. please