Source overrides
 

Hello colleagues,

I have a question regarding energy sources. I read through the CFX documentation for this answer and could not find anything explicit to this topic.

I have a box generating 450W which I have created a subdomain to assign this value to a volume.

An older engineer said he uses a rule of thumb that 60% of heat will dissipate through a baseplate which for this case would be 270W. I created a boundary for the bottom of the box and created a total source of 270W to account for this.

My question is this: how do these sources work together? I originally thought that the boundary would override the volume source, but when I have them together the baseplate is heated up a lot. When I only have the boundary the temperatures are a lot more feasible, but it doesn't make the analysis a full model. Is this possible?

Thanks for your time!

Both sources are applied. Why would one cancel the other?
You are adding 270 Watts. You need to put in a negative value to remove heat.
I myself would never use a "rule of thumb" in a CFD analysis, I would calculate (model) that amount of heat lost if this is something important.

The processor has a baseplate temperature limit, so I'm trying to keep it below that metric.

When I apply 450W to the subdomain volume that is distributed evenly, right? If I wanted to model that only 270W was coming through the bottom, what is the best way to accomplish that? As you say, would it be assigning -180W to that surface?

We are not the manufacturer of this processor, so that's where the rule of thumb came from. Trying to do our best with very limited information.

Thank you for your quick reply by the way!

I don't fully understand what you are trying to model.
If you assign total source to a volume, yes, it will be evenly distributed, as will a surface source. What other option would there be? Random distribution?
270 Watts coming through the bottom? You mean heat energy leaving the bottom? If so, you would apply -270W to the bottom surface (cooling at that surface) The remaining 180W would have to be removed via other surfaces.

I have this processor on top of a heat sink. I originally called out separate boundaries on the processor bottom and top of sink on the shared surface because I was not getting any sort of heat transfer between the two without them.

If I have the internal 450W on the processor volume only, the two boundaries are solid temperatures in post. It was only when I put 270W on the bottom of the processor and a flux in value on the top of the sink that something started to happen.

Does this make sense? All heat transfer is enabled, but it doesn't actually show anything.

Something doesn't sound set up correctly. Did you set up your interfaces correctly and enable heat transfer at those interfaces? Any pictures of your setup would really help.

Here is a picture of the setup.

Here is the output file.

You have defined a total source as a constant value, but you have defined a total source coefficient as well. As the derivative of your total source term relative to temperature is zero you should have a zero total source term coefficient. Why have you defined a value of 167?

I can tell by the blockyness of your image that you have a very, very coarse mesh. Meshes this coarse are always going to give unreliable results and you should not read too much into it. You need to do a mesh refinement study to determine how fine a mesh you need before your results are reliable.

You have defined a boundary called "Sink Default" which you have defined a heat transfer coefficient of 167 [W m^-2 K^-1]. Is this what you think is a 167W heat sink? If so this is a mistake - you have defined a heat transfer coefficient boundary, commonly used for natural convection, with a heat transfer coefficient of 167 [W/m2K].

It is unlikely your simulation is converged. Your residuals are loose. Also CHT simulations like this really should have imbalances as a convergence criteria as well.

More fundamentally, why do you think you need to explicitly define the heat going into the base anyway? Why don't you directly model the base (you are modelling the base, aren't you?) and then just let the simulation work out how much heat goes into the base and you can ignore rules of thumb. This is how you show the limitations of rules of thumb - they are usually not very accurate when you look at the details of what is going on.

Just to clarify, I followed your advice and got rid of the 270W emitting from the bottom and just had the volume source of 450W all within a 35C environment with some flow through the channels.

I believe this is outputting accurately now.

Based on what you mentioned, it seems like the rule of thumb is inaccurate and should not be attempted. The only thing closest to that is having a boundary that has 270W as a source and no volume source because those two would overlap and emit more than I want.

Correct?

There was a lot more to my advice than just removing the 270W. I doubt your simulation is accurate yet because of all the other issues I identified.

Hi ghorrocks,

I did not see your posting when I replied last.

-The total source coefficient was unclear to me. I thought I needed it to define the material again. So if I did not have a total source then I would need it?

-The sink default is actually a part of the shroud which I have declared as an inlet under Air. I'm not quite sure how to move it to the Air domain or get rid of it here, so I kept it as it was defined the material again. Where does this area truly belong in the tree?

-My heat transfer residuals are the only ones that are not converged right? How to I define imbalances? This is a new topic for me.

-I suppose I was focused on the rule of thumb so much because of someone with more experience (not FEA/CFD experience) told me. Being younger, I tend to follow their guidance thinking it is true. Ignorance breeds ignorance I suppose. Learning from everyone here allows me to correct that incorrect thinking. I am very thankful for the guidance. Now I know to model it fully and see what happens for myself. Is there a way to get a specific calculated output beyond looking at the contour map of that boundary?

Read the documentation about source terms - you should not be using options you do not understand! In short, the source term coefficient should be set to the derivative of the source term WRT the equation variable.

Sink Default - I have no idea what you are saying. You have defined this boundary to be a heat transfer coefficient boundary. If you don't want a HTC boundary then delete it.

You should do a convergence sensitivity check to see how tight you need to converge for the accuracy you want. There is no general answer to your question.

The solver and CFD-Post allows many quantitative values to be calculated. If you explain what you want to do we might be able to suggest how to do it.

-I removed the total source coefficient. Reading the documentation, I now know it is intended to improve convergence for nonlinear solution. Since I have a simple power source, it's not needed here.

-I attempted several times to get rid of the sink default. It will not allow me to delete it. Even after toggling the automated generation settings, it still creates it. Since it will be regarded as a wall and it's an area that I'm not really observing results-wise, I am cutting my losses. It's a problem I've seen others have based on research, but I could not find a definitive solution.

-Because you mentioned that my results look like I have a very course mesh, I ran a mesh refinement study (1.5x delta) with parametrics. I was a bit perplexed because my area of interest (the baseplate) never really changed temperatures. At first I was altering the mesh size of the baseplate to save time. Then without a change in temperature I did the overall mesh of the system and it yielded the same result. I felt that there was enough range to permit some changes in result. Maybe it is my laptop, but these studies took most of the day. You can see my charts in the attached. Did I commit an error? It's my first time using parametrics in Ansys.

-I included an imbalance monitor based on your suggestion for CHT and they all converged around zero. See attached. Based on my research, that is what should be expected. The overall convergence and heat transfer especially is still not there so a problem is very much present.

Thank you

I still have no idea what you are talking about with "Sink Default". The only thing I can think of is that it is the default boundary condition, and that means when you delete it, it is regenerated. You need to think about what you are doing (or explain it to us so we can help you) - in CFD you to define a boundary condition on all boundary faces. So CFX has a default boundary condition (a wall), which you can change to some other boundary if you like. But you have to define SOME boundary condition on it, you cannot have no boundary condition.

Good to see you tried a mesh sensitivity analysis. But you appear to have only changed the mesh parameters on one face or mesh feature. It is often better to do you mesh sensitivity on the entire mesh, meaning that you change all mesh element edge lengths simultaneously.

Getting the imbalances under 1% is good enough for most cases.

-Right I understand that it's an automatic boundary condition for the domain. I suppose my confusion lies in the fact that the domain already has two boundary conditions in fluid fluid and fluid solid interfaces. All parts of that domain should be accounted for in those interfaces and I believed that the default should disappear because of that. Regardless, I do have it as a wall and assigned a boundary condition as a heat transfer coefficient. This should not cause an error at this point.

-I'm glad you liked the study. I'm really trying to listen and build from your advice. The top chart is where I varied the face and received no temperature difference. The second chart under that is where I modified the default size for the whole system mesh. I think this is what you last suggested. It varies in the hundredth place. Was the default parameter not the correct stat to change? I'm reaching the point where if I go much smaller in size, my node student limitation will be reached. I'm hoping I'm not artificially stuck with a bad model here because of that.

-Currently, I made the enclosure fluid as small as possible and am running it again. I've notice that since I put the imbalance requirement in the runs have increased a lot in time.

Automatic boundary condition - if that face was intended to be an interface then you should make it an interface, and if it does not let you make it an interface have a look why not. It will probably be because the matching face in the other block does not actually intersect it.

The easiest place to start with mesh refinement studies is to halve the element edge length on everything at the same time. That is, half the coarse mesh and the refined areas all at once. The reason for this is because this allows easy calculation of grid convergence indexes and Richardson Extrapolation. But it also means that if you refine a part of the mesh which is not important you don't get fooled into thinking your mesh is OK because you missed the important bit.

You will probably find you hit the node limit of your student version pretty quickly. This is not "artificial", this is real - it means you don't have enough resources to complete the task, so you should not even start the task because you will be wasting your time. If you proceed you know your results will be inaccurate.

In CHT simulations it is normal for the solid time scales to be much, much slower than the fluid time scales. For steady state runs you can speed this up with solid time scale factors. For transient simulations you have to live with it - but you should consider separation of variables (look it up).