[jgross]

Hi everyone,

I would like to use BladeGen for a design optimisation study of centrifugal pumps. Using the GUI initially, I can export a BGI file, define variables, and use the batch command to create new geometries from the BGI file.

However, there is a problem when defining the control points of the LE. Namely, in the GUI, the end control points are such that they always lie on the hub and shroud curves. You can even define a length fraction that specifies how far along the streamwise direction of the hub and shroud curves the LE control points are.



However, in the BGI file, the control points of the LE are not constrained such that the end points lie on the hub and shroud surfaces. Instead, these points are strictly defined by their Z-R values.

    Begin LeadingEdgeCurve
        New Segment
            CurveType=Bezier
            UpstreamControl=Free
            Begin Data
                ( -7.669881059,23.35438893 )
                ( -15.79710000,30.48810000 )
                ( -25.22529274,37.83793911 )
                ( -32.58647974,44.66386003 )
            End Data
            DownstreamControl=Free
        End Segment
    End LeadingEdgeCurve

This leads to difficulties when I change the location of the control points for the hub and shroud or the LE curve, as these end points no longer lie on the hub and shroud surfaces, which leads to issues when exporting curve profiles to TurboGrid. Is there any way to ensure these end points are strictly constrained to lie on the hub and shroud surfaces in the BGI file?

Thanks for any help or advice you can give!

James

[jgross]

No one?

I've managed to come up with a workaround by creating a simple Python script. The function takes in the hub or shroud Bezier curve control points and a length fraction and creates a Bezier curve. This Bezier curve is then discretised into a user-defined number of points. The function then outputs these points (as well as the LE point) to be used for a spline representation of the hub or shroud.

The workaround is very imperfect, but it gets the job done (particularly if the number of discretised points is large). However, I would still be very interested if anyone else has any advice or tips.

James

[mertal1905]

Dear James,

I need to change .bgi file parameters to create new blade geometries, like youre doing.

But, i dont know how i will use this .bgi file while creating turbogrid mesh?

Can I use WB journal file?

I will be very happy if you can share details about BladeGen scripting. I would be more happy if you can share even simple script to explain a problem.

Best regards,
Mert

[jgross]

Hi Mert,

I'm sure you can use a WB journal if you would like.

However, the way I did it was by using the 'BladeBatch.exe' which is located in the folder

PathToAnsys\aisol\BladeModeler\BladeGen

where PathToAnsys is your local path to Ansys. On Windows it might be something like C:\Program Files\ANSYS Inc\v182

To create the TurboGrid files, just add the '-TG' flag with the directory you would like to place the files into.

For example, the whole command may look like

PathToAnsys\aisol\BladeModeler\BladeGen\BladeGen.exe yourFile.bgi -TG yourDirectory

Hope this helps

James

[mertal1905]

Dear James,

Thank you so much for your explanation in detail.

Best regards

Originally Posted by jgross

Hi Mert,

I'm sure you can use a WB journal if you would like.

However, the way I did it was by using the 'BladeBatch.exe' which is located in the folder

PathToAnsys\aisol\BladeModeler\BladeGen

where PathToAnsys is your local path to Ansys. On Windows it might be something like C:\Program Files\ANSYS Inc\v182

To create the TurboGrid files, just add the '-TG' flag with the directory you would like to place the files into.

For example, the whole command may look like

PathToAnsys\aisol\BladeModeler\BladeGen\BladeGen.exe yourFile.bgi -TG yourDirectory

Hope this helps

James

[ssmacae]

Dear James and Met,

I´ve been trying to work on a similar project performing turbomachinery optimization, but I´m very new to this windows batch mode, do you have any resources where I can learn about it?

Basically, I want to create an automated procedure to achieve a specific performance from turbomachinery. It's a type of pump, where I perform the CFD simulation using CFX, then I get a result. Then I change the pump diameter for example and get another result, so I want to do it iteratively until a reach the required result.

The iterative process would be:
Bladegen -> Turbogrid -> CFX -> meet the criteria? if not do it again.

[jgross]

Hi Joao,

Unfortunately, it seems that the documentation for batch capabilities in ANSYS is a little lacking. However, the main thing to note is that you will need to create template files for each step (i.e. a BGI file for BladeGen, a TSE file file for TurboGrid, a PRE file and a CCL for CFX Pre.

You can then call all of these processes in batch mode using the ANSYS batch commands from your favourite programming language (I have used Python, but you can use anything you want).

For BladeGen, the batch command is as above.

For TurboGrid, it looks something like:

PathToAnsys\TurboGrid\bin\cfxtg.exe -batch yourFile.tse

For CFX Pre, it looks something like:

PathToAnsys\CFX\bin\cfx5pre.exe -batch yourFile.pre

For CFX Solver, it looks something like:

PathToAnsys\CFX\bin\cfx5solve.exe -batch yourFile.def

For further information about these commands, you can read the output of the help from each of these commands.

The following link shows how the CFX portion of this process can be done in Perl:
https://www.google.com/url?sa=t&rct=...yTmeloY1MXvEQI

Hope this helps!
James

[ssmacae]

Thanks a lot, James!!

I´ll go through it!