CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   CFX (https://www.cfd-online.com/Forums/cfx/)
-   -   How should I plot dv/dt in CFX? (https://www.cfd-online.com/Forums/cfx/95720-how-should-i-plot-dv-dt-cfx.html)

 ali8500 December 30, 2011 01:31

How should I plot dv/dt in CFX?

Hi Guys,
Does anyone know How I can plot dv/dt in CFX where v is velocity and t is time?? I want to see the change of this term at specific time for my 2d simulation. I like to have a contour showing the changes of dv/dt.

Thanks,
Ali

 alemarins December 30, 2011 04:35

Time derivatives are partially supported in CEL.
Velocity time derivatives can be accessed with the ".Time Derivative" operator by setting up an additional variable as follows:

Option = Vector Algebraic Equation
Vector xValue = u.Time Derivative
Vector yValue = v.Time Derivative
Vector zValue = w.Time Derivative
END

:)

 ali8500 December 30, 2011 04:41

What is utderiv? do I need to define a new variable named utderiv?
I've started using CFX recentley. could you please explain more about the code?
tnx :)

 alemarins December 30, 2011 09:57

utderiv is the name of the vector variable with du/dt, dv/dt, and dw/dt components.

This way could be simpler for you:
1) from CFX-Pre GUI define a new Additional Variable named "utderiv" (or whatever you like)
2) in the panel select: Variable Type = Unspecified; Units [m s^-2]; Tensor Type = Vector
3) go to Domain->Fluid Models->Additional Variable Models and select "utderiv" in the selection area
4) flag the check-box just below the selection area
5) type "u.Time Derivative" in Vector xValue, and so on.

 Lance December 30, 2011 11:55

huh, I had no idea you could do that.
Reading a bit in cfx_ref.pdf I also found .Magnitude, .Gradient, .Curl, .Laplacian among others. Do they also work like .Time Derivative on AVs?

 ali8500 December 30, 2011 15:47

Thank you so much Alemarins.
I have two more questions. In Vector-xvalue box I have to enter u.Time Derivative or Velocity u.Time Derivative???
My second question: It seems that I have to run my simulation again so as to get the results for my new variable right? since I've already run my simulation is there any way to find du/dt in CFD-post?