Total-Pressure loses

pioneersteffen · September 15, 2009, 10:08

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?

Thanks for your help.

Kind regards

Steffen

olesen · September 16, 2009, 02:28

Quote:

Originally Posted by pioneersteffen

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,

thanks for your answer.

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.

Thanks for your help.

Kind regards

Steffen

olesen · September 16, 2009, 09:15

Quote:

Originally Posted by pioneersteffen

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

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..

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.

I hope I can help you.

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,

thanks for your answer.

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 907mm². Or do I have the wrong train of thoughts?

Thanks for your help.

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.

I hope I can help you.

Regards
Steffen

anil1886 · October 7, 2009, 16:53

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.

Maddin · October 9, 2009, 05:05

Normally you do this in a 1D simulation with GT-Power or something else.
In 3D you often only make a virtual flow bench run, 50mbar pressure on inlet or -50mbar on outleut (N/A or turbo engine) and then you can work on the design.
Next step would be a coupling of GT-Power with StarCD or CCM+ (in the next version).

September 15, 2009, 10:08	Total-Pressure loses	#1
pioneersteffen New Member Steffen Gruner Join Date: Sep 2009 Posts: 5 Rep Power: 16	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? Thanks for your help. Kind regards Steffen

September 16, 2009, 16:04	help regarding my simulation..	#5
anil1886 New Member anil Join Date: Aug 2009 Posts: 5 Rep Power: 16	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..

October 7, 2009, 16:53	sample value of pressure	#10
anil1886 New Member anil Join Date: Aug 2009 Posts: 5 Rep Power: 16	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.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
"Pressure Inlet" Boundary Setup	Wijaya	FLUENT	15	May 18, 2016 10:08
Static Pressure, Total Pressure	ufechner	FloEFD, FloWorks & FloTHERM	5	March 2, 2015 07:56
Pressure BC for combustion chamber	Giuki	FLUENT	1	July 19, 2011 11:35
total pressure in CFX	Atit Koonsrisuk	CFX	0	January 1, 2005 05:46
Total pressure to static pressure ratio	roadracer	Siemens	1	April 17, 2003 05:31

September 16, 2009, 09:04		#3
pioneersteffen New Member Steffen Gruner Join Date: Sep 2009 Posts: 5 Rep Power: 16	Dear Mark, thanks for your answer. 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. Thanks for your help. Kind regards Steffen

September 18, 2009, 03:39		#6
pioneersteffen New Member Steffen Gruner Join Date: Sep 2009 Posts: 5 Rep Power: 16	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. I hope I can help you. Kind Regards Steffen

September 18, 2009, 04:14		#7
anil1886 New Member anil Join Date: Aug 2009 Posts: 5 Rep Power: 16	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.

September 18, 2009, 04:55		#8
pioneersteffen New Member Steffen Gruner Join Date: Sep 2009 Posts: 5 Rep Power: 16	Dear Mr. Olesen, thanks for your answer. 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 907mm². Or do I have the wrong train of thoughts? Thanks for your help. Kind Regards. Steffen

September 18, 2009, 08:57		#9
pioneersteffen New Member Steffen Gruner Join Date: Sep 2009 Posts: 5 Rep Power: 16	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. I hope I can help you. Regards Steffen

October 9, 2009, 05:05		#11
Maddin Senior Member Join Date: Mar 2009 Posts: 260 Rep Power: 18	Normally you do this in a 1D simulation with GT-Power or something else. In 3D you often only make a virtual flow bench run, 50mbar pressure on inlet or -50mbar on outleut (N/A or turbo engine) and then you can work on the design. Next step would be a coupling of GT-Power with StarCD or CCM+ (in the next version).