[robtheslob]

Hello CFD-online forum,

I performed a quick search of the forum for "surface source" only to find a very limited selection of topics. Nothing seemed to address my issue. I feel pretty certain that someone will be able to answer my question!

I am using SolidWorks Flow Simulation 2014.

Is it possible to constrain a surface heat source to a specified temperature? Why is the temperature specification missing from the Surface Source feature?

This appears to make (physical) sense in my head, although perhaps I'm overlooking something quite simple...

Say I have an metal cube involved in a CHT problem. I'm interested in determining the temperature distribution in the cube if five of the sides are subject to forced convection. To the sixth side is affixed a [insert a heat source here: a combustion chamber, TEG, heat exchanger, extended surface geometry subject to some other flow, etc.] such that I can safely assume that the heated surface of the cube takes on the temperature of the provider of that heat. And, as you may have guessed, I am not interested in modelling the intricacies of that heat source. How would you go about modelling such a scenario in SWFS?

For now, my solution would be to create a very thin solid body in perfect thermal contact with the cube and apply a Volume Source feature with a specified constant temperature to that thin body. Is this the best approach? Are there any physical concerns (i.e. concerns with this model accurately representing the real-life scenario) when approaching a problem in this way?

Thanks for the help!

[Boris_M]

Hi Rob,

Yes, but you have to specify it in the "Boundary Condition" rather than under "Surface Source". So just like specifying an inlet or outlet you can specify a wall type of that condition in which you can define conditions such as roughness different from the one set in the general settings to selected surfaces as well as heat transfer coefficient and a temperature or just a wall temperature.
Maybe a little bit confusing.

I hope this ends your search,
Boris

[robtheslob]

Boris,

Thank you for the reply. You are absolutely correct; imposing a constant-temperature boundary condition for a wall that bounds a fluid subdomain is definitely possible.

However, what if that wall lies elsewhere? In conjugate heat transfer problems, it is often the case that a heat source is acting on a fluid subdomain "at a distance" if that wall is separated from the subdomain by virtue of some material.

If you try imposing a boundary condition on such a wall in Flow Sim, you will receive an error, as the wall does not bound the fluid subdomain. Specifically, it will appear as a rebuild error, and the message will read "[nameOfFace] is not laying on the boundary between solid and fluid region."

I probably didn't make it clear in my first post that such a case was the one I was interested in. Sorry!

[Boris_M]

Oh, I understand.
You have an internal simulation with a body in a distance to the actual considered model under flow conditions such as a hot engine in a distance to a pipe with a flow thought but only the pipe flow should be cosidered. Is that correct?

But even in that case, as long as both bodies are inside the computational domain, the wall condition can be defined as outer wall which basically means it is not in contact with a fluid even if there is no fluid in between the two bodies the wall has then a defined temperature but you might want to activate radiation as that is then the only way to transfer the heat from the surface to the other component.

Consider the tutorial example "Radiative Heat Transfer". Set it to internal and deactivate the "heat conduction in solids only" setting in the general settings. You need to move the one part of the sphere to have a surface contact with the other part so you have an internal volume. You can delete or deactivate the heat source in the sphere so now you have fluid in the sphere but none around it. You can then apply a wall heat source as outer wall on the large disc and it works. If you have radiation activated it will radiate onto the sphere, if not then there is no heat transfer between the two bodies.

Does that help?
Boris

[robtheslob]

Boris,

Thanks again for the assistance.

I think I may have failed to make the situation clear; it's actually simpler than the situation you're describing!

Let's say we have a solid block of material with a hollow "tunnel" within the block. The tunnel has two exposed openings.



Let's call one opening the inlet and the other, the outlet. Within this cavity will flow a fluid of interest. The fluid subdomain will encompass the cavity that snakes within the block. Our fluid subdomain is totally encompassed by walls; thus, we will run an internal flow analysis.

If I would like to apply a heat source to the opposite side of this block, I must insert a Source feature in Flow Sim. I cannot impose a boundary condition as the face of this block lies outside of the fluid subdomain. Any heat transferred to the fluid is by virtue of conduction through the solid.

No Flow Sim problems so far. Applying a boundary condition to the heat source wall results in an error - expected, as it lies outside of the fluid subdomain. Applying a surface source feature to the wall does indeed result in a CHT system and the solid (and thus the fluid) exhibits a thermal gradient.

My question is this: why isn't the constant-temperature specification available for the Surface Source feature? It's available for the Volume Source feature, and it seems odd to me that it's missing from Surface Source.

[Boris_M]

Ok, a sketch makes it all much clearer :-)
The reason why it is not in surface source is simple because the developers didn't do it that way. I know it might be confusing in this case of a surface temperature while a volume temperature is under volume source.
I cannot speak for the developer who initially did it this way or why it was done like this as it is like this for many years.
However, you need to specify a "Boundary Condition" with the type of "wall" and the wall type "outer wall". Here you can specify the temperature of the wall as well as a different wall roughness and a heat transfer coefficient.

Maybe they did it because it is a wall boundary condition and not a source in that way and wanted to include it in the boundary condition feature and maybe later in the early development years they saw the need for a surface source but the wall temperature was already in the other feature so they left it. However, you will need the boundary condition feature as described above and If you use an internal simulation with heat conduction and the whole model is inside the computational domain (make sure the reset the computational domain to be sure) then it should be possible to define such an "outer wall" type wall with a specified temperature.

I'll try to do a screenshot of an example.

Boris

[Boris_M]

This image shows the outer wall setting and the outer wall, as the name suggests, does not need a fluid domain contact such as the regular wall type.

Boris

[robtheslob]

Boris,

Wow. How simple. How did I overlook that third option each and every time?! You literally gave me the answer in an earlier post and I failed to realize it.

Now it's clear why your mind starting going in the direction of complex radiation models: you must have assumed the answer you were providing was too simple! I'm off to a good start on this forum...

Thank you so much for the information. That was very helpful!

As an aside: is there a SW Flow Sim user manual? I have three documents (and I had to dig for all of them in my file system) for use as Flow Sim references: a Tutorial manual (full of helpful tutorials), a Technical Reference (Information on underlying software mechanics and physics, and their corroboration) and a Solving Engineering Problems document (an interesting read with advanced topics and advice). However, I wouldn't call any of these documents a "user manual," outlining the function of each feature and tool in Flow Sim, one by one.

If I have a question about a feature in ANSYS, for example, I open up the (Fluent) user manual, hit Ctrl + f and search for the function name / a keyword. The document contains every single tool, menu, GUI and CLI function, etc., so if it's not in there, it's probably not in the software.

Is there such a manual for Flow Sim? That way, I don't have to resort to wasting other users' time with silly questions.

[Boris_M]

Hi Rob,
I'm glad, I thought I am missing something in your case.

Yes, of course. In every feature such as boundary condition or window that you open like for the engineering database or the solver run, you have a question mark somewhere in the window like the one in my screenshot right next to the header name "Boundary Condition". Simply click on it and you are already in the help related to that specific feature in which all the settings are explained on what they mean. If you want to know more about a certain parameter or option you can also search in that help by going to the search or index part of the help and type in anything you are looking for and it should find some related topics in which it is mentioned.

However, if you have any question that might not be clear to you from that help, feel free to come back to the forum ;-)

Boris

[robtheslob]

Boris,

Yet another simple answer to a simple question. Thank you for being awesome.

Perhaps it's because I couldn't access the tutorials via the SW menus (as you would access them for other SW software modules; that is, via Help > SolidWorks Tutorials) that I just assumed that the only way to access reading material for Flow Sim was by digging around in the file system. I've literally never once clicked on one of those little question marks. How funny.

Thanks again for everything!

[Grandup]

hello ,
i appreciate your efforts to solve problems .
i have exactly the same case now in the picture description but i'm working on FLUENT .
so i will be grateful if you help me to define this boudary in conjugate heat transfer . ( i tried a very thin volume source at the surface also ..) but the solution is diverged .
thank you very much

[robtheslob]

Grandup,

I would recommend starting a new thread for this problem. People reading this thread from the top down (to get an idea of what we're talking about) may assume that the issue is constrained to SW Flow Sim, and Fluent experts may stop reading before they get to your question.

Good luck.

[CFDfan]

Originally Posted by Boris_M

Hi Rob,

Yes, but you have to specify it in the "Boundary Condition" rather than under "Surface Source". So just like specifying an inlet or outlet you can specify a wall type of that condition in which you can define conditions such as roughness different from the one set in the general settings to selected surfaces as well as heat transfer coefficient and a temperature or just a wall temperature.
Maybe a little bit confusing.

I hope this ends your search,
Boris

Boris when you specify the roughness of the wall and that wall is not radiating but a part of the conduction heat transfer assembly (for instance the wall of a heatsink with semiconductor device attached to it). So the questions are:

1.Does Floworks account (i.e. calculates) for the increased contact thermal resistance between the devices and the heatsink when the roughness of the heatsink wall increases?

2. Does it account for the improved heat transfer (film) coefficient of the heatsink with higher roughness?

3. If the answers of 1 or 2 are "YES" could you please point me to a reference(s) with equations of how the thermal contact resistance varies with the roughness and how the film coefficient varies with the roughness

P.S. Boris hasn't answered and in the meantime and run a model with varied roughness of the walls. It didn't change the results, so it looks like the roughness doesn't affect the contact thermal resistance nor the film coefficient. In that case what would one need it for?

[Boris_M]

Hi CFDfan,

No, the wall roughness is only for the solid-fluid interface, so when the flow is in contact with the wall. The software has ideal contact where geometries are in direct contact. Reason is, that it would depend how the roughness is pressed onto each other or to exaggerate, if you have a saw tooth structure on both contacting surfaces, the structure of the two could be only in contact with the tips or with 20% of the flanks of the saw tooth or fully matched into each others hills and valleys. How would you want to define that then ;-)

You would need to specify a thermal contact resistance in such a case via the corresponding boundary condition.

The roughness will influence the flow and pressure loss for example in a very narrow channel due to increased turbulence.

So if you use a roughness in a very close finned heat sink, it would influence the flow and increase the heat transfer through turbulence.

Boris

[mikek]

I have a very similar problem to solve as ROBTHESLOB has posted above, however, I want to set up his heat source as a constant temperature AND heat rate.

With SolidWorks flow 2016, I can specify a volume heat source with parameters such as heat rate (watts) OR constant temperature. Can I do both? Possibly with a temp sensor? I know I can do this in a thermal study but not flow study. I am setting this up as external flow because in addition to Rob's internal fluid flow and heater, I have a cooling fan blowing on an external heatsink (mounting point) on the model as well.

The reason I want both: My system has a heater as well as a temperature sensor; controlled by PID. As soon as the internal fluid flows through the subdomain, the heat of the system (block) will begin to drop, then recover. In my opinion, the higher the heat rate or wattage, the faster the system recovers, thus affecting the fluid output temp. Is that correct? Can someone help me set up a heat source for this flow problem?

Thanks.
Mike

[Boris_M]

Hi mikek,

Can you explain what exactly the model should do?
Even in real live such a condition is not possible so there must be some reason for it that you think you need a constant temperature and a heat source.
Do you want to control the temperature of a component to a certain value with a temperature sensor and a heat source or why do you need a constant temperature.

Usually, it is very easy to think "real life". What or how is it happening in reality, which is usually what you want to reproduce in the simulation.

Regards,
Boris

[mikek]

Boris thank you for replying.

The system is meant to heat the fluid flowing through it to a temperature of 200C. The temperature does not need to be precise and I am not trying to control the temperature. I simply want to measure, through simulation, how much the temperature fluctuates during initial flow conditions.

The system explained step by step:

1. From room temperature, the system is heated to 200C with a 20 watt power source.

(Note: remnant internal fluid is within the system during warm up).

2. Once system reaches steady state 200C (controlled by a thermocouple located at a specific point on the system), internal flow begins.

(Note: incoming fluid is at room temperature)

Once the fluid flow begins, the temperature of the system will drop due to the incoming fluid being at room temperature. I want to be able to measure the drop in temperature once fluid flow begins. Specifically, I want to measure or probe the exit temperature of the fluid during the entire simulation.

Is it possible to setup a flow or conjugate simulation with a heat source of 20W, a set temperature of 200C (possibly adding a temperature sensor as well) and internal fluid flow on a time step function?

Let me know if I can explain this better or if you need any other information.

Thank you,
Mike

[Boris_M]

Hi mikek,

this is an excellent description of the case you want to simulate. This helps a lot to give you the right advice.

From your description, I would say it needs to be a transient simulation as you want to probably also know how long it would take to heat up to 200°C.
If the heat up is not necessary in transient then this is also not a problem, but the rest seems to be a transient simulation as soon as the flow starts.

1. Simulation:
You can set up the case with the 20W source and the initial temperatures of fluid and solid as room temperature. Since you use a thermocouple at a specific location, I would suggest using either a point goal of the fluid temperature (as I think the fluid temperature is what you want to measure) or if the thermocouple is larger such as a larger surface, you can also model such a solid geometry and either deactivate it with the component control (for the flow to be able to pass it) or leave it as solid and use a surface or volume (in case of it being deactivated) goal of the fluid temperature. You can then use that goal as stopping criteria in the calculation control options where you can specify the value at which the simulation should be stopped. If you go to the Finishing tab and use the drop-down field for that goal that should be used to stop the simulation, you can select "> Absolute value" and specify that value as 200°C. It is best to uncheck the other goals check boxes to be used in the convergence and make sure that the goal convergence is checked for the finishing criterion and no other criterion as the simulation should only stop when the 200°C are reached and not when the maximum travels or any other criterion is achieved.
This will then stop the transient simulation once the 200°C are reached.

2. Simulation:
Now that you have reached the 200°C, you can use that result from that simulation as an initial condition for the second simulation to include the starting fluid flow.
You can set up the project with the flow rate you want to specify and in the general settings under the initial and ambient condition tab, you can select in the very first row named "Parameter definition" the drop down which currently shows "User Defined" and select "Transferred". Then you can select the FloEFD Project by clicking on Browse. This will map the results from the previous simulation onto the model as initial conditions so as if you simply continue where you left off, but now with the defined flow condition.
To make it all easier, you can do the project setup of the 1. Simulation up to the point where I said to change the calculation control options and then clone the project and name both of them like "Initial phase" and "Starting Flow" or something like that. Makes it easier to tell which order they are :-)
You can then do the changes described in 2. Simulation on that clone. This saves you the full setup of the project again and you only need to do some minor changes like defining the flow rate and the end time for the transient simulation and in the 1. simulation then the calculation control changes. You can also add any goals you like to have for tracking the temperature etc.

Once both projects are defined, you can use the batch run to run them in the corresponding order and the second simulation will then automatically use the results of the first run as initial condition.
The reason for using two simulations is that at the moment it is not possible to define a flow rate boundary condition in dependency of a goal so the 2. Simulation will basically start with flow one the 1. Simulation reached the temperature.
There is also a way to do it in one run but it depends on what type of goal you want to set and could possibly stop the flow. In this case, you would need to use a fan curve for the flow which can be made goal dependent and be switched on once a specific goal is reached. If you are using a pump or fan then you can also model the flow rate more accurate depending on the system pressure loss, but you can also define your own fan with constant volume or mass flow rate overall pressure losses and therefore keep it constant. You then select the "toggle" option not as "Always On" but in the "fx" button as Goal dependendt with the "F(goal) - table" in the fan curve boundary condition. Here you can then select "Switch ON when goal > control value" and set the control value as 200°C and have a large dead band of probably best "100 K". This basically determines that the fan switches off when the temperature drops 100K below the 200°C so once it reaches 100°C. You should choose it high because you don't want the flow to stop due to the lower temperature that is reached at the thermocouple. You could also set it to 200 K and then the flow would need to reach 0°C which is basically impossible if the flow enters at room temperature. You then only have to select the thermocouple temperature goal from the drop down list of goals.

I would maybe advise you to use the transient explorer for the simulation to save detailed results savings but you have to decide which parameters you are interested in your analysis to visualise before the simulation is started as only those will be saved every X iterations and can afterwards be visualised.
You can find more information about the transient explorer when searching in the FloEFD help for it.
There is also video about the new features in V16 in which it is shown and briefly described, it starts at 8:45 in the video: https://www.mentor.com/products/mech...6---what-s-new

I hope this helps,
Boris

[mikek]

Boris,

Thank you for the detailed reply. I am using Solidworks Flow as I do not have FlowEFD, however, I think I can set this up as you described, in Solidworks. I will give it a go and let you know the results or come back with more questions. Again, much appreciated. Thank you.

Mike