CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   STAR-CCM+ (https://www.cfd-online.com/Forums/star-ccm/)
-   -   How to calculate lift, drag and lift distribution in Star CCM+? (https://www.cfd-online.com/Forums/star-ccm/161272-how-calculate-lift-drag-lift-distribution-star-ccm.html)

 israelcasillas94 October 21, 2015 04:01

How to calculate lift, drag and lift distribution in Star CCM+?

Howdy,

I'm currently trying to import a parasolid model of an RC aircraft into star ccm+ to determine the lift, drag and lift distribution over the wings, but I'm having some trouble setting up meshes and running the simulation properly, can someone tell me if my steps are correct?

First open a file and import the parasolid model.

Then check the model for any surface error.

Create a wind tunnel, by making a block large enough to fit the entire aircraft.

Set the region of the wind tunnel walls and aircraft body as a region with each part surface having their own boundary.

Set the inlet, outlet, plane of symmatry, and walls for the wind tunnel.

Create a surface repair operation, and set the appropriate settings, in my case lowering the target cell area to be .02 m, curvature points to be 100, and selecting both my wind tunnel and aircraft as the parts for the surface repair.

Execute the surface repair operation. After this point there should be no errors on my plane.

SAVE

Define my physics continium, setting steady, turbulent, 3 dimentional flow settings. Set the velocity of my inlet to be 35 mph in the x direction.

Establish my reports for the force in the y direction for lift, x for drag. How do I do lift distribution?

SAVE

Refine my leading and trailing edges by placing blocks and cylinders over the wings with more specific parameters to refine those areas.

Set up a volume mesh for my surface mesh and my new blocks, and cylinders. setting up the cell dimensions to be the same as the surface repair dimensions.

Then SAVE

Reopen using parallel, and run my simulation.

Those are all the steps I attempt to go through when conducting my simulations is this correct? I am messing up in one area, since my lift values are incredibly low and do not make sense. Where could my error be? in my volume mesh most likely? Also how do you set up the lift distribution over the wing? Is it even possible?

If someone can recommend a good tutorial on this matter that would greatly help!

Thank you for the help!

 fluid23 October 21, 2015 15:41

Second, there is a Star-CCM+ forum for software specific questions. Your thread will probably get moved there.

Third, your low total lift is almost certainly a mesh issue. Did you do a mesh dependency study? Are you resolving your wake and tip vorticies?

Fourth, here is the workflow I use for parts based meshing.

Fifth, you shouldn't really need to refine leading/trailing edges using volume shapes (blocks, cylinders). If your surface mesh is properly refined and your volume mesh settings appropriate, you will get a good mesh. However, you may need to use volume shapes to refine the wake depending on your mesh selection. For external aero you should probably use the trimmed mesher which has an option for automatic wake refinement. (Work the tutorials/check Steve Portal if you are unfamiliar).

Sixth, there are a number of ways to approach extraction of spanwise lift distribution. Probably the easiest is to:

1. Go into your CAD file and cut the wing surface into a series of spanwise panels.
-Use an elliptic distribution to cluster sections more at the wing tip than at the root.

2. If you don't have a constant chord wing, keep the spanwise sections small enough that your change in chord from inboard edge to outboard edge of each panel is small.

3. Assign each spanwise section of your wing to a different region boundary. All will still be walls, but you want to have separate sections that you can setup reports on.

4. Setup force reports to give you lift of each spanwise section. Couple this with your knoweldge of how the span is divided, the average chord of each section, etc... to get your spanwise lift distribution. You should be able to do this and generate a plot without ever leaving star-ccm.

 israelcasillas94 October 22, 2015 18:52

Quote:
Thank you for the response. Sorry about the title I just realized how different it is to what I am asking. I attempted to look for a Star CCM+ forum, but I must have missed it. I'll improve next time.

As far as doing a mesh dependency study, I did not. What exactly would mesh dependency study do? ensure that my solution is not dependent on the size of my volume mesh over the aircraft? I believe I am, but I could be wrong, where should I look to ensure that I am properly resolving the wake and tip vorticies?

This flow chart looks great! Thank you for sharing it. I'll look to follow this on my next simulation.

Thank you for all the help! I'll attempt to do the lift distribution using that method.

 me3840 October 22, 2015 19:20

You can also create an accumulated force table to display the lift build up or you can create your own field function of the lift force and plot that through an XYZ internal table. Those are a lot easier than chopping your boundaries up.

 HarshiBavishi November 6, 2020 09:35

Quote:
 Originally Posted by me3840 (Post 569726) You can also create an accumulated force table to display the lift build up or you can create your own field function of the lift force and plot that through an XYZ internal table. Those are a lot easier than chopping your boundaries up.
Can you please elaborate on this process? Im new to star ccm+. If possible please explain the entire procedure in points. Thank you very much

 All times are GMT -4. The time now is 06:15.