Discussion Groups

Simulation CFD

Reply
Active Contributor
DenPopov
Posts: 31
Registered: ‎08-22-2013
Accepted Solution

Heating of the current water

220 Views, 5 Replies
11-26-2013 09:23 AM

Hello. Tell please, whether I made everything correctly?

 

There is a pipe on which water flows. The pipe has the heater intended for heating of water. I want to learn what water temperature will be at the exit.

 

My steps:

 

1) I appointed to all objects materials.

01.png

 

2)  I appointed boundary conditions.

02.png

03.png

 

3) I started calculation.

04.png

 

Whether I made everything correctly?

Please use plain text.
Product Support
wildej
Posts: 934
Registered: ‎08-25-2011

Re: Heating of the current water

11-27-2013 08:28 AM in reply to: DenPopov

Hi DenPopov,

 

This will not work as it is. What are you expecting to happen in the surrounding air? Is there a forced convection here or is it naturally convected?

The P=0 and Temps on the air are the issue.

 

I think it would be best to point to towards these guidelines but also remind you that all surface Boundary Conditions must remain external.

 

Kind regards,

Jon



Jon Wilde
Please use plain text.
Active Contributor
DenPopov
Posts: 31
Registered: ‎08-22-2013

Re: Heating of the current water

11-27-2013 02:22 PM in reply to: wildej

Pipe receives heat from the heater, thus flowing water also receives heat. This device (pipe with heater) is in the room with the air temperature 22 C. The part of heat is allocated in environment (air), therefore the pipe and the heater are cooled.

 

In the model, I put the device in the air, ie created a part (solid part) that covers the device. In the room is no fan, so I appropriated all facets of air P = 0. Indoor air is 22 C, so I appropriated all facets of air T = 22 C. What is wrong? How to do it right?

 

In the model, all surface Boundary Conditions are external or where I do not understand?

Please use plain text.
Product Support
wildej
Posts: 934
Registered: ‎08-25-2011

Re: Heating of the current water

11-28-2013 07:48 AM in reply to: DenPopov

Hi DenPopov,

 

Please take a look at the natural convection guide I posted, you need to base this analysis on it.

 

You will need to model the water and solid part within a large air domain using the 'chimney' approach. P=0 top and bottom and ambient temp at the bottom also.

Making air 'variable' and enabling gravity also.

 

You will then need to add suppressed solids at either end of the water so that you do not have internal BC's.

 

This should work OK, although please understand that really you need a fully developed flow in the pipe and an excellent mesh to be able to calculate an accurate heat transfer - it might even be better to run the pipe out the sides of the large air domain but have a suppressed solid around most of it internally, so only the central section that you have here is meshed and under test, does that make sense?

 

Kind regards,

Jon



Jon Wilde
Please use plain text.
Active Contributor
DenPopov
Posts: 31
Registered: ‎08-22-2013

Re: Heating of the current water

11-30-2013 05:16 PM in reply to: wildej

I seem understood you.

 

1) I created two aluminum "stoppers" (rectangular object having thickness of 1 mm) in order that water didn't concern air.

01.png

 

2) I created a detail "air". On the Material Environment dialog, I select Variable. The top and bottom surface of a detail (air) have P = 0 (2 surfaces). Lateral surfaces of a detail (air) have T = 22 C (4 surfaces).

02.png

03.png

 

3) On the Solve dialog, enable Flow and Heat Transfer and specify a Gravity vector.

04.png

 

4) I carried out calculation. The results look convincing - warm air rises.

05.png

 

That's right?

 

- Whether it is necessary to exclude from the analysis of stoppers?

- Whether it is necessary for water on the Material Environment dialog, select Variable?

Please use plain text.
Product Support
wildej
Posts: 934
Registered: ‎08-25-2011

Re: Heating of the current water

12-02-2013 01:04 AM in reply to: DenPopov

Hi,

 

This is nearly there, a few more points:

 

  1. Yes, suppress those caps, the BC's must not be internal and they must be attached to a suppressed part
  2. Please refer to the guide I sent regarding the dimensions of the domain - ideally it should be taller, we need to capture the plume
  3. Remove the temps on the sides, you only need one on the base with the P=0

That should be about it - be sure that you have a good mesh. Try cloning the scenario and refining the mesh to see if the results change, if they do they are likey tending towards a more accurate result.



Jon Wilde
Please use plain text.