# Water through pipe

• 829 Views
• Last Post 10 September 2019
• Topic Is Solved
Gate9er posted this 03 February 2019

Hello

I am been struggling to solve the following problem:

I have a 1m plastic pipe with water flowing through (at 1m/s and 7 degrees at inlet). The pipe is submerged in soil with a constant 18 C temperature. What I am trying to find is the water temp at the pipe outlet, as a result of the soil temperature heating (something like a geothermal system).  The model I have built is 3d you can see in the photo attached. There are three bodies, water at the center, surrounded by the pipe, then both surrounded by the soil.

I have created 4 interfaces, then coupled them in two walls. Now the problem is that I can't seem to find the proper boundary conditions in order to achieve water heating from soil, through the pipe and to the water.

Any help would be greatly appreciated.

Thanks

Attached Files

Order By: Standard | Newest | Votes
abenhadj posted this 10 September 2019

Please go through all tutorials.

Best regards,

Amine

Jibzy01 posted this 09 September 2019

Please Kindly explain this. I am running a multiphase flow in horizontal pipe in 2D axisymmetric geometry. Please on what condition(s) do I specify the wall thickness and the gravity please.

Gate9er posted this 04 March 2019

Just wanted to ask, do I need to set a heat generation rate for the wall selection during setup? I have given a temperature of 18 C.

Gate9er posted this 07 February 2019

That's correct, I just realised that I have mistakenly created that line as wall. I should have created a wall at the top of the pipe and not there!

peteroznewman posted this 07 February 2019

Since you are using Shared Topology, there is no need for Contact between the pipe and the water. In Meshing, go into the Connections folder and suppress the Contact that was automatically generated for you.  Maybe this what the contact_region-trg is, the line between the pipe and the water?

Regards, Peter

• Liked by
abenhadj posted this 07 February 2019

Still not clear. Go back to mesh and give named selection for the water and soil surface at first. I do not understand this contact wall. Please give a named selection for the wall between the fluid and solid region. It would make things much easier for you

Best regards,

Amine

Gate9er posted this 07 February 2019

Ok, so I have created an axisymmetric model for the pipe and fluid. I have enabled shared topology between the two surfaces. You can see in the photo below:

Then in Ansys mesh I have created 4 named selections, Inlet, Outlet (left and right of the pipe), then an axis (bottom), and a wall (top of the pipe) which will act as the external domain, soil, with constant temp.

Ansys setup: All available boundaries are shown below.. The model is set to Laminar with energy equation on.

There are three materials assigned, water for fluid domain, HDPE for the pipe, and soil for the wall (at the top of the pipe). The wall (boundary named as contact region target) has been given a constant temp of 18C and  a small thickness of 0.05m. For inlet I have 7C and velocity of 0.1 m/s. The rest are left by default.

Residual criteria have been set to 1*10^-4.

Sections of the flow results are shown below. The water has been assigned with an initial temp of 18C, although I only chose that temp value for the Wall at the top of the pipe.

Hope I have provided with enough information.

Thanks

abenhadj posted this 07 February 2019

Share as screenshots, BC's, models, reports, materials and anything might help to understand the issue. Do not forget the residual plot.

Best regards,

Amine

Gate9er posted this 07 February 2019

Hello, I have run the simulation but I have this issue, it looks the water is cooling the pipe rather than the pipe heating up the water. Any suggestions?

Gate9er posted this 06 February 2019

I will give it a try and come back for anything. Thanks

rwoolhou posted this 04 February 2019

Yes. Assuming the axis is along the y=0 (x) axis. The wall must be given a thickness in Fluent to correctly calculate the conduction through the material.

To add, in 2d axi you could also model a section of the soil too as cell count won't be a problem: if you hit the 512k cell count I'd be very surprised!

Gate9er posted this 04 February 2019

Thank for the input. So to recap, I set a shared topology with a generated conformal mesh. The model is axisymmetric. I then add one inlet, one outlet, one wall (that is the top edge with constant temp of 18 C) and one axis (bottom edge) for axisymmetric. Further heat properties will be subject to added materials.

That should be it yes?

rwoolhou posted this 04 February 2019

Assuming the mesh is conformal Fluent will sort all that out for you. You just need to make sure the mesh is suitable.

• Liked by
Gate9er posted this 04 February 2019

Ok thank you. So no convection scheme needs to be applied between the pipe and fluid?

rwoolhou posted this 04 February 2019

A coupled wall is between two objects in Fluent (pipe & fluid in your case) and you can just leave that as default. On the outside of the pipe set a constant temperature as Peter suggested.  Another simplification is to model the fluid section only and set the outer wall with a constant temperature but also give the "thin" wall a thickness.

Look through the wall boundary condition in the Fluent User's Guide, specifically the heat transfer options.

Gate9er posted this 04 February 2019

Thank you very much.What would be the boundary condition between the two rectangles (the pipe and the fluid) then? Does a coupled wall still needs to be applied or will a convection thermal condition work fine?

peteroznewman posted this 04 February 2019

You have too much detail. It would be better to scale back to a 2D axisymmetric model of just the water and plastic. Let the temperature on the outside of the plastic be a constant 18 C. An axisymmetric 2D model of the pipe and water just needs two rectangular surfaces, 1 m long along the X-axis on the +Y side. If you use shared topology, that will simplify the Fluent model. You need the thermal conductivity of the plastic. In meshing, use Named Selections on the left edge of the water and name that Inlet, while the right edge of the water is named Outlet, and the bottom edge of the water is named Axis.

In Workbench, pick the Geometry cell and set the Analysis Type to 2D before you draw the rectangles. The two rectangles must be drawn on the XY plane along the X axis on the +Y side.  The water rectangle sits on the X-axis and has a height on the Y axis equal to the inner radius of the pipe. The pipe is a rectangle sitting on top of the water rectangle and has a Y height equal to the pipe wall thickness. In SpaceClaim, set Share Topology to Share.

• Liked by