Setting the computation

To set the computation you must define operating conditions in the Star GUIde window.

Then you must define the numerical parameters:

  1. check id you are in steady time or transient. in Select analysis features.
  2. in Analysis preparation/running > Set run time controls you can chose the time step and the number of iterations.
  3. in Analysis control > Analysis output you can select the frequency for writing data into a file.  In the transient tab you can chose the variables to be saved by checking the Post button. Warning you should verify that the setting is correct just before saving the files.
  4. Save all files and quit. Warning after saving the problem and geometry file check the result in the command window. Don't forget to connect the events before saving.
Running the computation

To run the computation you should:

  1. Launch pmovlink that will create the events.
  2. starlink will build the star executable according to the parameters set in the prosize
  3. star will compute the results.
    Loading data

To load data use the Star GUIde Post processing > Load data.

  1. Select transient to be able to load all time steps (case.pstt file). If the file doesn't exist the Analysis output is probably not set right.
  2. Select a position in the list and set moving mesh on if necessary.
  3. Only then Add file to list and Open transient post file.
  4. Choose a time from the list and store it.
  5. Click on the Data tab select the variables to be stored (you can put the smooth option on) and click on Get data
Displaying data: vector, contour, particles
Vectors and contours

To display the data concerning the time you have loaded go to the Create plots menu.

In the option select if you want to display contours or vectors and click on Plot to screen.

Particle track

To display particles tracks go to the particle tracks menu.

  1. Click on Add location to list. In the graphical window click on vertexes that will be the starting point of your particles. When you are finished go back to the Star GUIde and click on Done
  2. Click on Recall list
  3. Click on the Plot particle tracks tab and Plot tracks
Saving pictures
To save pictures use the Utility>Save screen as menu of the graphical window.

If you want you can use the scdu command:
scdu gif 1000 save an image named casename1000.gif and increments the name each time you use replot.
scdu off is used to stop the saving process for each replot

These commands are useful when saving more pictures using loops like the following one:
This loop loads the first time step and then saves 40 images of the velocity magnitude for each new time.

store, first
scdu gif 1000
*defi noexe
getc none,vmag
sdcu gif 1000
*loop 1,40
scdu off


Go to Thermophysical Models and Properties > Turbulence Models
Turn turbulence On
Select K-E/High Reynolds Number
Go to Monitoring and Reference Data
type 5 in the Monitoring cell number


Go to Analysis features
Select Transient

Go to Analysis controls > Solution controls > Equations behavior > Primary variables > Equation status tab
Exclude the WMom from being solved.

Go to Analysis Preparation/Running > Set Run time controls
Type 600 in Number of time steps
Type 0.001 in Time step size

Go to Analysis Controls > Output controls > Transient tab
Type 5 in Post frequency
Select U,V,P,KE in the Post button.

Save the Geometry file
Save the Problem file
Quit and save


In the terminal

type the case name


type the casename


open prostar
Go to Post Processing > Load data
Select Transient in the analysis menu
Select Yes in the moving mesh menu
Select the first position in the list and click Add file to List
Click Open transient post data file

Select a time step
Click on Store/iter time

Click on the Data tab
Click on Get Data
Click Go to create plots
Select the Vector option
Click on Plot to screen.

That's it!