multiple runs for lift and drag at various AOA
 

I am currently modelling a wing (to validate my technique) and want to find the performance characteristics for the wing at several angles of attack. Basically I want to be able to hit run once and for it to keep running until all the AOA's I specified have been simulated and the data exported i.e.

1. Run simulation
2. Converge
3. Export results (ie. User points such as cL,cD and cM to exel spread sheet (or similar))
4. Change AOA and repeat process, writing each new set of data onto a new line of the same excel spreadsheet.
5. Repeat until reaching an AOA of 15 degrees.

that way I will end up with discrete lift and drag for aoa's of 2,4,6,8,10 degrees etc

I am under the impression that setting up my domain and changing the components of the fluid velocity is the way to go about it, but I havent been able to find any tutorials that step through the process.

I assume there is a way, so if anyone could give me some advice or point me towards a useful tutorial that would be awesome.

Thanks in advance. :)

Look at the parametric design and possibly the optimisation tutorials for ANSYS Workbench. So you will need the Workbench tutorials for this, not the CFX ones.

You could also probably write a script to do this. Just have CCL files prepared for each flow angle (assuming this is just a change in your boundary conditions) and call cfx5solve with the additional argument "-ccl whatever.ccl". As for writing to excel you could generate a csv file by reading the out file with your script. Not sure if this is easier or harder than using Workbench.

Sorry about the delayed response.

I figured out how to do it in workbench. I've given a brief summary below how I did it, im new on this forum so im not sure about the etiquette but is it good form to make a bit of a tutorial to help anyone else with similar problems? I dont mind doing it, shouldnt take too long, but there is no point doing it if it isn't going to help anyone.

Anyway, what I did was (for anyone wondering) Import the wing into design modeler then create my domain around it in there. Then I performed a body operation (rotate) to allow the wing to rotate around an axis. Then I made this a parameter (check the box next to the angle you are inputting for the amount of rotation) and called it "aoa".

I then followed normal procedure all the way to the solve phase. After the first solve had been performed, I went into Result. Then I went to the expressions tab and right clicked on my cD,cL and cM and made them all output parameters.

Then your workbench should look like the photo I have attached .

After clicking the parameters box it looks like the second pic attached. Then I just added my parameters (in this case -5,0,2.5,5,7.5,10 for my angle of attacks) and make sure you check the "Exported" tab so you get a new design point for each parameter, so it should look like the 3rd picture. then just hit "update all design points" and away you go.

For anyone that finds this while looking for a way to do this themselves, If I get a chance and anyone would like a little document made up as a bit of a tutorial I will try to do that. Or just pm me if you would like some clarification.

I did whip a quick tutorial, im not sure how technically correct it is (there is probably better ways to do it) but it worked for me.


Sorry its pretty rough, if I get a chance I will try and tidy it up when I get some spare time but its nearly impossible to get any decent amount of information into a file 97.7KB .doc file. grr, stupid attachment limit.

For the mean time, I hope this helps someone.

Cool, I'm sure this will help people.

It Works
 

Helped me out! Thanks for that info. It works with Fluent as well with the same procedure in case anyone is curious.

workbench parametric design
 

hi guys
i already meshed my model in ANSA. i have meshed file so how to proceed for this situation.

dude i am not getting the cl cd cm what should i do