[himanshu28]

Hi,



I am trying to simulate "Modeling Internal flow and Heat transfer through a wavy pipe" (attached a .jpeg).i have splited my surfaces into 3 surfaces as inlet, outlet and wall.In the problem i have considered that the wall is at the constant temperature (1000 C) and the fluid at the inlet has velocity and intial temperature as 200 C in the physics continua i have specified outlet as the pressure oulet now in the outlet continua there is a static temperature option which by default is taken as 300K ,but since i am intrested in finding the temperature at the oulet of the fluid then why do i need to specify it ? another thin which is coming in my mind is am I modeling the problem correctly, that is because since pipe surface is a solid so do i need to create another surface across the fluid continua and then create and interface between the two.I am totally confused i have run the solver by the above expalined setup and obtained no change in the outlet the fluid temperature.I have seen the heat tansfer problem given in the tutorial file but couldn't find any explaination to my problem.Untitled.jpg

[triple_r]

The temperature needed for the outlet is for backflow. So, if you have an eddy, for example, near the outlet, and the solution domain is too short that cuts through the eddy, you will have some backflow. As there is some fluid going into the solution domain, the software has to know what value it should use for temperature. If you have selected the solution domain so that you will not have a backflow, then do not worry about the value that you provide.

Don't give a way off value though, as during the convergence you might see some back flow, and if the outlet temperature is way off, you might end up with an unstable situation. In your case as you have a constant wall temperature, you can't go wrong with having a temperature in between the inlet temperature ans wall temperature (depending on the pipe length, you can decide approximately where in that range the value you provide should be)

Regarding the other question, it depends on the physical situation that you want to model, how much information you have when it comes to boundary conditions, and how detailed you want to model the problem.

If the pipe wall is thick and you only have information about the outside of the pipe, then you are better off having the wall as a solid domain and define an interface for heat transfer between the two domain. This will add a bit of complexity, and run time, but is not that bad.

On the other hand, if you know that the wall is very thin, so there will be almost no heat transfer in the axial direction, then you can use a onedimensional model for the heat transfer in the wall to adjust the heat transfer coefficient outside, or in your case, just to specify the outside wall temperature as the boundary condition for the fluid flow.

[himanshu28]

thank you....!!!!!!

Originally Posted by triple_r

The temperature needed for the outlet is for backflow. So, if you have an eddy, for example, near the outlet, and the solution domain is too short that cuts through the eddy, you will have some backflow. As there is some fluid going into the solution domain, the software has to know what value it should use for temperature. If you have selected the solution domain so that you will not have a backflow, then do not worry about the value that you provide.

Don't give a way off value though, as during the convergence you might see some back flow, and if the outlet temperature is way off, you might end up with an unstable situation. In your case as you have a constant wall temperature, you can't go wrong with having a temperature in between the inlet temperature ans wall temperature (depending on the pipe length, you can decide approximately where in that range the value you provide should be)

Regarding the other question, it depends on the physical situation that you want to model, how much information you have when it comes to boundary conditions, and how detailed you want to model the problem.

If the pipe wall is thick and you only have information about the outside of the pipe, then you are better off having the wall as a solid domain and define an interface for heat transfer between the two domain. This will add a bit of complexity, and run time, but is not that bad.

On the other hand, if you know that the wall is very thin, so there will be almost no heat transfer in the axial direction, then you can use a onedimensional model for the heat transfer in the wall to adjust the heat transfer coefficient outside, or in your case, just to specify the outside wall temperature as the boundary condition for the fluid flow.

[himanshu28]

hi Reza,
if i want to know how much heat from the wall is been transfferd by the pipe wall to the fluid region then i should have two regions on solid and another liquid.? and then i should create an interface between the two...presently i have not generated any solid wall across the fluid(water) continua and i have given wall temp 1000K of fluid continua but i am unable to see change any change in the monitor of heat transfer coeffi. and in X Y plot of the Nusselt number and distance so. please suggest should i make an interface so that i can select two regions of my intrest on solid and on fluid and then see change in properties of fluid.

thanks in advance

regards
Himanshu sharma

[triple_r]

Sorry for my late reply. I don't check this forum that much, which I should.

Going back to your question, there are two ways to find the total heat transfer from pipe wall to fluid:

1) This is the easy way! You can integrate the heat flux on the wall. I don't know how to write equations here, so I'll try a text version of it:

total heat flow = integral of (heat flux) dA over the region you have called the wall

In starccm+ you can use a report: right-click on the reports > New report > Surface integral, then select heat flux as the function to be integrated, and select the wall boundary as the part.

2) This is the hard way, and assumes the solution has converged and is steady, but will show you if the solution is correct. You can use the first law of thermodynamics:

total heat transfer into the fluid = energy flow out of the solution domain - energy flow into the solution domain.

If we can assume the properties are constant to make life easier:

total heat transfer = specific heat * mass flow rate * (outlet bulk temperature - inlet bulk temperature)

to get bulk temperatures, use reports again:

right-click on reports > new reports > Mass flow averaged

then select temperature as the function, and outlet or inlet as the part. You'll need two reports, one for outlet, and one for inlet. Then run the reports and subtract the values, and multiply by specific heat and mass flow rate (to get mass flow rate, create another report for Mass flow)

The value that you get from the two reports should be almost equal, and by almost I mean within the accuracy of the solution, or in the order of residuals.

I hope this helps.

[Goutam]

Hi,

Could you tell me, how to draw a wavy circular pipe?

Originally Posted by himanshu28

Hi,



I am trying to simulate "Modeling Internal flow and Heat transfer through a wavy pipe" (attached a .jpeg).i have splited my surfaces into 3 surfaces as inlet, outlet and wall.In the problem i have considered that the wall is at the constant temperature (1000 C) and the fluid at the inlet has velocity and intial temperature as 200 C in the physics continua i have specified outlet as the pressure oulet now in the outlet continua there is a static temperature option which by default is taken as 300K ,but since i am intrested in finding the temperature at the oulet of the fluid then why do i need to specify it ? another thin which is coming in my mind is am I modeling the problem correctly, that is because since pipe surface is a solid so do i need to create another surface across the fluid continua and then create and interface between the two.I am totally confused i have run the solver by the above expalined setup and obtained no change in the outlet the fluid temperature.I have seen the heat tansfer problem given in the tutorial file but couldn't find any explaination to my problem.Attachment 16555

[himanshu28]

Originally Posted by Goutam

Hi,

Could you tell me, how to draw a wavy circular pipe?

Hi,

I have drawn the Pipe in Autodesk Inventor 2013 it gives you an option of generating a the curve by equation.So i used the equation to generate the curve and then revolved the curve 360 deg around the an axis to generate the corrugations.
U can try the same with splines as well

Cheers