CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   STAR-CD (https://www.cfd-online.com/Forums/star-cd/)
-   -   Total-Pressure loses (https://www.cfd-online.com/Forums/star-cd/68325-total-pressure-loses.html)

 pioneersteffen September 15, 2009 10:08

Total-Pressure loses

Dear Star-users,

I currently do a transient simulation of an exhaust manifold and I want to devide the manifold in the postprecessing into different parts to analyse absolute pressure loses. The simulation is allready done and I want to anlalyse the results in Post.

How can I do this in Star-CD-Post?

I think I must implement some "areas" to average the absolut pressure over the area and get a value. But how does in work in Star-CD?

Kind regards

Steffen

 olesen September 16, 2009 02:28

Quote:
 Originally Posted by pioneersteffen (Post 229561) I currently do a transient simulation of an exhaust manifold and I want to devide the manifold in the postprecessing into different parts to analyse absolute pressure loses. The simulation is allready done and I want to anlalyse the results in Post. How can I do this in Star-CD-Post? I think I must implement some "areas" to average the absolut pressure over the area and get a value. But how does in work in Star-CD?
For each time-step

1. get the total pressure. Here's an example with scaling in mbar.
Code:

```! ptotal.MAC ! ! get absolute total pressure in mbar ! use Star-CD definition ! out: reg1-3= Vel, reg4= Ptotal [mbar] getc all PTot,absolute\$oper smult 1e-2 4 4 head\$TOTAL PRESSURE\$ABSOLUTE [mbar]```
2. Set a section cut with 'spoint' and 'snorm'. Note that since this cut extends through the entire model, you have to be careful that you only have the cset that corresponds to your region of interest.

3. Get the average values across the cut.
Eg,
Code:

```! savg.MAC ! ! use current spoint/snormal to calculate avg in slice ofile none *get ATot TAREA *get STot TAS *set Savg STot / ATot ofile screen *list Atot      !-> Area *list Stot      !-> Total Value *list Savg      !-> Avg Value```
These are a straight average; you'll need to do some extra work if you want massflow-weighted values.

 pioneersteffen September 16, 2009 09:04

Dear Mark,

I follow your instruction and I have the problem, you have warned me. When I define a section cut, the entire model is cutted, not only one pipe. How can I do this? Sorry for the stupid question.

I already looking in the uses guide, but I don't find a solution for this problem.

Kind regards

Steffen

 olesen September 16, 2009 09:15

Quote:
 Originally Posted by pioneersteffen (Post 229680) I follow your instruction and I have the problem, you have warned me. When I define a section cut, the entire model is cutted, not only one pipe. How can I do this? Sorry for the stupid question.
As I mentioned, you need to reduce your cell-set to the region-of-interest. Eg, "cset subset zone", or you can also use the pro-STAR button that looks something like [C->] for the same thing.

Since this is command that you'll always be using, I'd suggest making an abbreviation for it (eg, cnz). See the user's manual about defining abbreviations ... I haven't touched mine for quite some time.

This is one of the really nice things about pro-STAR, you can use the menus if you wish, but you can also type the commands too. With a few simple aliases, like that above, you can become quite efficient: type a few letters with your left hand while still holding onto the mouse with your right.

 anil1886 September 16, 2009 16:04

help regarding my simulation..

hi Mr Steffen Gruner,
i'm trying to simulate an exhaust manifold to learn the transient analysis of the model below. i'm done with most of the meshing.
i want to know how to create the boundary conditions for changing the inlets based on the crank angle and firing order.
plz help with this..

http://img17.imageshack.us/img17/2640/14940251.png

 pioneersteffen September 18, 2009 03:39

Hello,

I have convert the Crank-angle into a time. So when you have for example 3500 RPM, you can convert it into a timestep-duration of one crank angle of 60/(3500*360)=4,76e-5s. Then I define a table with the table editor and define the timesteps with the associated pressure and temperature. That table you can import in the boundary condition section.

Kind Regards
Steffen

 anil1886 September 18, 2009 04:14

really thanks for the tip. i got upto that. but how do you change the boundary conditions from one flange to other based on the time step..
like how do you make a port an inlet and a wall based on the time and according firing order..
and if it is ok, i mention, only if it is really ok, can i see how you wrote the time steps in the table editor, because i'm totally new to this and i dont even completely know how to play with the options and boundary conditions. every information you give will be really helpful and i'll be using to solve my problem.
thank you very much for the tip..
thank you,
anil.

 pioneersteffen September 18, 2009 04:55

Dear Mr. Olesen,

I can do only section cut for one pipe yet. I create a new cell set of one pipe and plot only the cell set of the pipe. So it might be secure, that I just use this for section cut and for calculation of the area and therefore the area averaged pressure. Is it right?

The strange thing is, when I use your commands for avagering, and I look at the "Atot" output, the value seems to be very small. The "Atot" is 0.1385e-5, but the diameter of the pipe is 34mm and so we must get 907mm˛. Or do I have the wrong train of thoughts?

Kind Regards.
Steffen

 pioneersteffen September 18, 2009 08:57

Dear Anil,

at first you open the table editor. Then you create a new table and choose "table type selection" as "Boundary Conditions", and select under "options" a boundary type, e.g. "pressure". The next step is to select the "independent variable" as "time" and for "dependent variables" e.g. "PR"(Pressure) and T(Temperatur). Then you type all time steps inside the "independent Variables Table" and "fill the independent Variables to columns". Then you define for every time step, the pressure and temperatur and push "write", so save the table.

In the boundary definition you select "Region Type", "Pressure" and in "User Options" you must choose "Table". Then define the "Table Name" and all is fine.

You can also look at the users-guide and the tutorial guide. I remember, there are some examples.

Regards
Steffen

 anil1886 October 7, 2009 16:53

sample value of pressure

hi Mr Steffen,
I'm working on the simulation now. I'm trying my model in fluent to check how it is working. I dont have more data on the exhaust gas pressure and temperatures.
If u can give any data regarding the pressure, velocity and temperature of exhaust gases of an engine... it would be a great help for me..

my email is anil1886@gmail.com

thanks,
anil.