# Surface Source - Fixed Temperature?

 Register Blogs Members List Search Today's Posts Mark Forums Read

 April 24, 2014, 12:19 Surface Source - Fixed Temperature? #1 New Member   Rob Join Date: Apr 2014 Posts: 13 Rep Power: 12 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!

 May 6, 2014, 09:28 #2 Disabled   Join Date: Jul 2009 Posts: 616 Rep Power: 23 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

 May 6, 2014, 10:26 #3 New Member   Rob Join Date: Apr 2014 Posts: 13 Rep Power: 12 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!

 May 6, 2014, 11:15 #4 Disabled   Join Date: Jul 2009 Posts: 616 Rep Power: 23 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

 May 6, 2014, 12:00 #5 New Member   Rob Join Date: Apr 2014 Posts: 13 Rep Power: 12 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.

 May 7, 2014, 06:38 #6 Disabled   Join Date: Jul 2009 Posts: 616 Rep Power: 23 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

May 7, 2014, 07:00
#7
Disabled

Join Date: Jul 2009
Posts: 616
Rep Power: 23
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
Attached Images
 wall2.png (25.5 KB, 135 views)

 May 9, 2014, 02:25 #9 Disabled   Join Date: Jul 2009 Posts: 616 Rep Power: 23 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

 May 9, 2014, 14:14 #10 New Member   Rob Join Date: Apr 2014 Posts: 13 Rep Power: 12 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!

 April 28, 2016, 09:31 #11 New Member   Gabes Join Date: Apr 2016 Posts: 11 Rep Power: 10 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

 April 28, 2016, 17:48 #12 New Member   Rob Join Date: Apr 2014 Posts: 13 Rep Power: 12 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.

June 22, 2016, 19:18
#13
Senior Member

Join Date: Jun 2011
Posts: 202
Rep Power: 15
Quote:
 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?

Last edited by CFDfan; July 4, 2016 at 12:08. Reason: addition

 August 16, 2016, 09:03 #14 Disabled   Join Date: Jul 2009 Posts: 616 Rep Power: 23 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

 April 21, 2017, 23:24 Similar problem but need temp sensor in model #15 New Member   Mike Join Date: Apr 2017 Posts: 3 Rep Power: 9 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

 May 3, 2017, 02:25 #16 Disabled   Join Date: Jul 2009 Posts: 616 Rep Power: 23 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

 May 9, 2017, 20:12 #17 New Member   Mike Join Date: Apr 2017 Posts: 3 Rep Power: 9 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

 May 12, 2017, 02:28 #19 New Member   Mike Join Date: Apr 2017 Posts: 3 Rep Power: 9 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 lee jim likes this.

 Tags cht, solidworks, source, surface, temperature