Learning Forum

[Laure]

Hi,

I am creating a simple 2D model (transient thermal) to run it in Fluent. The model has two faces representing a free water zone and a porous zone (as indicated in the image attached). I would like to include three line-heat sources at different depths, which will represent heating tapes that deliver heat at contant rate (~20W/m). Could you please guide me on how to include these heat sources? Thanks in advance.

 

 

 

 

 

 

 

 

[Nikhil Narale]

Hello, 

 

One possible solution that comes to mind is to increase the thickness (little bit) of the Line heat source as shown in the image. Then, you can assign a named selection to it and apply a heat flux boundary condition.

If anyone is having any other suggestions, feel free to share them.

[NickFL]

 

Could we not do it with a radiator source? (1) Imprint the faces in DesignModeler (2) Create a Named Selection for these imprinted lines in ANSYS Meshing. (3) Find these lines in the Boundary Conditions -> Internal. (4) Select the lines and convert to Radiator type.

Laureano, is it acceptable to have the heat go on both directions or is it only on one side of the interface? Do you know the heat flux or the heat transfer coefficient? Look closer at the documentation.

Edit: Sorry I missed you said that it is 20 [W/m²]. Yes that can be done as above. Is there potentially water flowing thru this line? Or does it act like a wall? If you switch these interior to a wall then it will create it and a shadow. Then you can specify the heat transfer just in one direction, but then it restricts flow through the line.

[Laure]

Thank you NickFL / Nikhil,

I need the heat to go on both directions. At the moment, I am not considering water flowing across the line heater, but later I may want to compare with the case where there is convection due to hotter water bouyancy in porous media.

I did a test by creating a line in DisgnModeler (representing one line heater):  1) added a New Sketch,  2) selected Line in Sketching tap and c) drew a line (see snapshot attached)

Then, I generated a Line from Sketches: Concept / Lines from Sketches

Next, I tried to imprint the line on a face/body by: Create / Body Operation. I selected "Imprint Faces" on Type, and tried to select the face and line, but it did not work. I got a error message saying:

Warning: Some selected bodies are invalid,

Line bodies are not permitted for boolean type operations. Context: Body Operation Feature BodyOp1

I did another test in which I created 3 Name Selection in Ansys Mesing using selected nodes (image below). However, these names do not appear in Boundary Conditions (Fluent).

Could you please guide me on how to imprint these 3 lines in DesignModeler? or can provide any other workaround to represent these three line heat sources in Fluent. Thanks in advance.

 

[NickFL]

In DesignModeler, the imprint is done with the projection of these lines onto the Surface. Projection is found under the Tools pull-down menu (it looks like you are using the English version). This will slice the face (just over the region of the line) and then you can add a Named Selection to them in DesignModeler or in ANSYS Meshing.

Line bodies aren’t going to help you in Fluent.

 

[Laure]

Hi NickFL,

Thanks so much. After a couple of attempts witht Projection it looks like is working. I will compare this approach with the one suggested by Nihil.

 

[Rob]

To add, in Fluent if the lines are set as thin walls there's an option to give them a thickness and add a "volume" heat source. That may be more suitable than the radiator boundary type. 

[Laure]

Thank you Rob.

[Laure]

Hi Rob,
The heating cable that I used in the physical experiment, which I am trying to model with Fluent, delivers heat at 20W per meter of cable (20 W/m). I am wondering if there is a way to convert this quantity to the units required in Fluent (W/m2)? Thanks in advance.  

[NickFL]

You are simulating a 2D model. In theory it goes infinitely into/out of the screen. But in your real case we have a fixed depth. How can we take a slice of this and compare it to the slice of the infinitely deep 2D model?

Hint: How wide is the tape?

[Laure]

Thank you Rob / NickFL,

The tape's cross-sectional dimensions are 1.3 x 0.85 cm.

Yesterday, I came up with a possible solution. From a prevoius experiment where I coiled the heating tape on a PVC pipe, I have the cylindrical area covered with 5 m of the heating tape. I can now associate this quatity (heat delivered per m2) with the heating tape linear length I have in the new experiment (20 m). I'll test this I let you know the outcomes.

[Rob]

And in 2d the default thickness is 1m. It's possible to change this in the reference values but I REALLY suggest that you don't. 

[Laure]

Hello,

I am reaching out again because I couldn't find a way to convert from W/m to W/m2. Any other idea?

The heating tape (line source) delivers heat at 20 W/m. 

Thanks in advance.

 

[Rob]

OK. The thin wall has a thickness which you defined in the wall bc panel. In 2d the domain is 1m thick unless you changed a reference value. If you changed a reference value, change it back. So, your 20W total is applied as W/m3 with the wall volume being length (from geometry) * thickness (BC panel) * 1m.  

[Laure]

Thank you Rob.

This means that if my heated cable is 20 m long, the heat flux I should input is 400 W/m2 (assuming 1m thickness)?? 

 

[Rob]

If you have 20m of cable at 20W/m you need to add 400W.  You are NOT adding W/m2 you are adding W/m3.   

In the CFD model you have the lines. It's 20m long, and 1m deep with a thickness (wall bc Thermal tab) which gives you the volume. Divide the total heat input by that volume, to get W/m3 and put that value into the panel. 

[Laure]

Thank you. 

Sorry to bother you again. I am still stuck with the power setting for my 2D case. 

This is the point: If I am assuming a line heat source, the cable thickness should negligible, so why I need to add a thickness and input heat per volume?

 

[NickFL]

We need a "volume" for the Fluent to be able to use the heat generation which is in [W/m³]. Your length, the one meter into the screen and then the last dimension for the volume is the thickness. The effects of this thickness on the flow field is not really considered as we are not resolving the thickness of the wall in the mesh.

One thing to keep in mind as you are comparing this to experiment, is that we are apply this in a planar model. If your experiment is on a circular pipe where there is water on either side of the pipe (into and out of the screen), then would we expect our model to be a little to hot or too cold?

[Rob]

This thickness

[Laure]

Thanks Nick / Rob for your reply.

I ran three cases in a simplified 2D model. The tank in 6 m long and 2 m deep. The top 0.2 m contain water (fluid) and the rest is sediment (solid). The line heat source in 2 m and is located 0.5 from the top, heating the sediment (solid) for 4 hr. In these cases, I am only considering conduction in sediment.

In case 1, I assigned the thermal conditions of the line source as Heat Flux and input power rate per m2

In case 2, I assigned the thermal conditions of the line source as Heat Flux and input power rate per m3 (assumed cable thickness = 0.01 m)

In case 3, I assigned the thermal conditions of the line source as Coupled and input power rate per m3 (assumed cable thickness = 0.01 m)

Cases 1 & 2 produced the same results. However, Case 3 developed a much lower temperature profile (please refer to image below).

All cases reached a lower maximum temperature compared with the observed maximum value (34 C).

Questions:

1)      What is the correct approach to define heat rate for the line heat source of this problem?

2)      Do you have any idea of the differences between Case 1 (or Case 2) and Case 3?

3)      Why do you think simulated maximum temperature is lower than the observed maximum temperature? Note: I did a sensitivity analysis of solid thermal conductivity, specific heat, and density (using appropriate ranges). In all cases, simulated maximum temperature was lower than observed maximum temperature. 

Thanks in advance.

[NickFL]

Good Morning,

So here are my thoughts based on those images:

• First look under Reports -> Fluxes -> Total heat transfer rate and then select the surfaces. Compare these between the cases.
• For each of the walls you have section2 and section2.shadow correct? When you have it set up for coupled, then any changes that occur on one side of the wall will automatically be applied to the other side. This means these two sides are coupled together. On the other hand, when you have the heat flux, then you can set different values for either side. This means that for cases 1 & 2 you effectively have double the loading of the case 3. I hope the results from the flux report demonstrate this.

As for the comparison of the model to the experiment

• You are running these as transient, correct? What are you using to judge convergence per timestep? It is very likely that the energy RMS values will be converged below 1e-6 before the temperature on each heater is converged. Set-up a monitor point on each of these heated sections and see if it is converged before moving on to the next time step. It could be the error associated with this is causing the under-prediction.
• In my last post I asked if the sections planes or pipes in the experiment. How we compare the results with the experiment will be a little different between the two. If it is the former the results should match up pretty well. If it is the latter, we can discuss further.

[Laure]

Thanks Nick,

I'll have a look to the flux report and heater convergence. 

Yes, for wall section2 (line source) I have a shadow wall. In all cases, I always made sure both walls have the same heat rate (either in W/m2 or W/m3).

The experiment can be considered a horizontal sediment layer & a water layer (not a pipe) since the pond channel is approximately 2 m wide and the maximum heating time is only 4 hr. The cable was burried in the middle of the channel. So, the tank that I have in my 2D model represents a logitudinal section of the channel and line heat source. 

Please let me know if you need any other info. Thanks in advance.

[Laure]

Hello everyone,
I ran the same model in Mechanical and got similar results than in Fluent (i.e., conduction is the main heat transfer mechanism).
Now, I added another geometry (circle) to deliver heat to the sediment body. I compared the temperature profiles in the two heat sources and observed that they differed significantly (image below). The circle-shape source in the 2D represents heat injection/propagation perpendicular to the line heat source (heating tape), whereas the thin bar represents heat injection/propagation longitudinal to the heating tape.
Wonder why the shape of temperature profiles are so different??
Note: in my experiments, the heating and cooling profiles (observed data) resembles those resulted from the circle heating source in the 2D model.

[NickFL]

My thinking is that this goes back to my comment about the 2D plane and the pipe. There is a difference between them, but we would model them in the same way.

Think of it like this: If we had a pipe, how much surface area is in contact with the outside? In comparison, if we took a slice on the plane (to make it look like the point source), we will only have the top and bottom surfaces to radiate. The neighboring slices would also have only the top and bottom and cannot go "radially/axially".

I am more surprised in how SIMILAR they are than the differences. Although it looks like the circle is already approaching a limit and the bar still has a ways to go.

[Laure]

Hi Nick,
Thank you. Correct, unlike the circular heat source, the line source hasn’t reached a pseudo steady state.
So, the best option to represent my experiment is to create a 3D tank model with a thin cylinder as the 20-m heat source (heating tape). Is this correct?? Appreciate your comments.

 

[NickFL]

Good morning Laureano,

It really depends on the goal of your model. Is it meant to compare against some standard, or are you trying to match experiment?

1. For matching to experiment, yes, a 3D model would work well, but there is definitely cost associated with this. Running a transient 3D will take a lot more computational time than your simple 2D model. Is it worth it? This is an engineering judgement you have to make.

2. If you are trying to show that this configuration meets some standard, then your 2D model will be useful. Why? Because it is conservative. This means if your 2D model meets the criteria then the real 3D case will too.

3. Depending on exactly the goals of the model, there may be a way to re-scale the input heat flux. I don't have a scaling factor in my head, nor do I have my copy of Incropera & DeWitt handy. But there may be something in there that could be useful.

Good work so far!

[NickFL]

 

Also, going back to your results on May 12th, why is the temperature cooler in the middle of the free water zone? In the middle it is the dark blue 23.4° contour and on all four sides it is at the 24.27°C contour. Do you have an explanation for this?

 

[Laure]

Thank you for this quesion. 

For these tests, I am assuming the same temperature no vertical temperature variation in water (20 cm water column). I am using water temperature time series as input data. Water transfers heat to sediment at the interface. Also, heat pulses through the heating tape transfer heat to the sediment. 

The objective of the modelling is to match observed temperatures recorded using fibre optic sensors attached along the heating tape.