[Maulana Akbar R]

Hello everyone,
Currently i have a project to analyze the effects of vortex generator on lift and drag coefficient of NACA0021 airfoil. I use Ansys CFX as the cfd module. The analysis was done in 3D. I used multiblock model, structured outer domain, unstructured near the foil as can be seen in the picture below. The problem is it seems that the vortex generator did not prevent flow separation at higher angle of attack when the foil stalled. The lift and drag coefficient did not differ significantly from the model without the vg. Maybe somebody know what the problem is? Thank you

here's the link to the image i've got:
https://drive.google.com/drive/folde...usp=share_link

[ghorrocks]

Please attach images directly onto the forum in future. To not use third party download sites.

Your airfoil appears to be running at a massive angle of attack, and the flow is grossly separated. Vortex generators work by adding turbulence to the flow to allow an airfoil which is just separating to keep the flow attached.

In other words you need to be looking at a flow just beyond the separation angle, not grossly beyond it like you have done.

[Maulana Akbar R]

Originally Posted by ghorrocks

Please attach images directly onto the forum in future. To not use third party download sites.

Your airfoil appears to be running at a massive angle of attack, and the flow is grossly separated. Vortex generators work by adding turbulence to the flow to allow an airfoil which is just separating to keep the flow attached.

In other words you need to be looking at a flow just beyond the separation angle, not grossly beyond it like you have done.

Sorry for the inconvenience Glenn, this is the first time i posted in this forum. I will attach images directly in the future.
Thank you for your quick reply. However, my supervisor intended to analyze the effects of vg in AOA range of 0-180 degrees as it will be used in a vertical axis turbine.
The image before is from AOA of 30 degrees, i will simulate the case again at a lower AOA as you suggest. I will provide further improvements/problems here. Thanks again for your insight.

[ghorrocks]

And additionally: The vortex generators work by tripping a laminar boundary layer to turbulence earlier than would otherwise happen, and that is beneficial because turbulent boundary layers stay attached better than laminar boundary layers.

This is a very tricky thing to model. I have tried to model this effect on airfoils before and failed, it is not simple. You are going to need a turbulence transition model, the SST turbulence model and a very fine mesh. It might also need an LES approach to get working (not sure on that). But it is definitely a very challenging simulation to attempt and will require considerable development and validation before it is working.

Good luck!

[Maulana Akbar R]

Hello Glenn, after doing two other simulation at a more appropiate angle of attacks, the vortex generator still did not affect the airfoil performance. I wonder if there is a minimum thickness required to model a wall in Ansys CFX? I've read that this solver could do only 3d simulation. Currently i have my vg thickness at 0.5 mm, do you think it might be the problem?

[ghorrocks]

I will repeat my previous post:

This is a very tricky thing to model. I have tried to model this effect on airfoils before and failed, it is not simple. You are going to need a turbulence transition model, the SST turbulence model and a very fine mesh. It might also need an LES approach to get working (not sure on that). But it is definitely a very challenging simulation to attempt and will require considerable development and validation before it is working.

And to answer your comment, yes, the vortex generator will need to be correctly designed as well. Too small and it will do nothing, too big and it will just generate a big separation which does not reattach (and increase drag, if that is relevant). So if you have guessed your vortex generator geometry then you almost certainly have it wrong. You will need to do a literature review to work out what design of vortex generator you need.

[Maulana Akbar R]

Originally Posted by ghorrocks

I will repeat my previous post:


And to answer your comment, yes, the vortex generator will need to be correctly designed as well. Too small and it will do nothing, too big and it will just generate a big separation which does not reattach (and increase drag, if that is relevant). So if you have guessed your vortex generator geometry then you almost certainly have it wrong. You will need to do a literature review to work out what design of vortex generator you need.

Thank you again for your reply. After improving the mesh quality and quantity, it seems that the vg is disturbing the fluid flow around it in CFD-post. Although the cl and cd is still the same as the model without vg. I think i still need to simulate more AOA around the stall region. I have another question, can you plot pressure coefficient (cp) from cfx solver? I know how to do it using ansys fluent, but not cfx.

[ghorrocks]

Yes, you can plot pressure coefficient, but you have to define it as an expression and deal with it as any other variable. It is not available as a built in option.

[Maulana Akbar R]

I want to give an update regarding this problem, in case someone struggle with this problem in the future. This problem was solved, i did what Glenn suggested. It seems that the vortex generator affect the CL and CD in a range between 10 - 20 degrees angle of attack, before the flow completely separates from the foil's leading edge. Also, make sure to increase the quality and quantity of the mesh around the vortex generator to fully capture its effect on foil performance. I make a separate domain that enclose the vortex generator, as it will take a massive amount of nodes when using a single fluid domain.

[nzerimo]

Originally Posted by Maulana Akbar R

I want to give an update regarding this problem, in case someone struggle with this problem in the future. This problem was solved, i did what Glenn suggested. It seems that the vortex generator affect the CL and CD in a range between 10 - 20 degrees angle of attack, before the flow completely separates from the foil's leading edge. Also, make sure to increase the quality and quantity of the mesh around the vortex generator to fully capture its effect on foil performance. I make a separate domain that enclose the vortex generator, as it will take a massive amount of nodes when using a single fluid domain.

Hello, please were you able to sort this out, I happen to be working on similar project currently