In the same general setting window that you set the radiation temerature, pick the "Wall conditions" on the navigator pane then expand the "Thermodynamic Parameters" and set the temperature. You can also expand the "Solid Parameters" and set the initial solid temperature.
Hope this helps.
Thanks for the information, but I'm still trying to figure out the correct way to simulate this scenario, perhaps you could be of further assistance. I have a completely sealed enclosure, no air openings at all. In the center of the enclosure is a liquid cooled cold plate, which I have simulated successfully separately. When I place it inside the enclosure I get drastically unpredictable results, which suggests to me that I am doing something wrong (that is I keep getting that annoying message "Solid is Melting", which was funny at first, now just frustrating). Where I'm getting wrapped around the axial is with the Boundary conditions and initial setup of the simulation. basically this is a three fluid simulation, being a fluid inside the cold plate (water), fluid inside the enclosed box (Air) and the fluid around the exterior of the enclosure (also Air). I’ve take the fluid cold plate out of the equation and settled on trying to figure out the correct approach without it. I Believe my error is within my full understanding of the general settings. Below is how I have the simulation set-up:
- General Settings (in attachment)
- Under wall Conditions I have the default wall radiative surface to Blackbody wall.
- Under Initial and Ambient conditions, I set both the Thermodynamic parameters and sold parameters for temperature to 85.
I created a Fluid subdomain inside the enclosure for the air. There are no boundary conditions set.
The simulation runs, but the enclosure doesn’t exhibit any characteristics of being affected by the heat inside the enclosure, even through my heat source is located on the bottom of the enclosure.
What I am hoping to accomplish is:
- a) Determine the inside temperature of the enclosure
- b) The skin, Outside temperature of the enclosure.
Thanks – keven
General_Settings.pdf 60.3 KB
It might be best for you to spend some time going through some of the tutorials.
In the meantime, turn off radiation and set the default outer wall condition to 'temperature', and then set your temperature.
OuterWall.jpg 59.1 KB
I didn't have much success with your suggestion. With the Analysis type set to External and radiation off, there are no default wall conditions as your BMP suggests. I'm using 2009, is this a new parameter setting in 2010?
All my previous simulations have been successful, it's as soon as I seal the box up that I have been having issues. I couldn't find a tutorial or any examples of simulations that fit what I'm doing.
Do you have any other suggestions?
At this point, please post your SLDPRT or use Pack and Go on the SLDASM.
- General Settings (in attachment)
I've used external simulations with a large enclosure with a high voltage transformer and it solves just fine. (see attached)
If you're not confident in that you could create a dummy wind tunnel - make a box larger than your enclosure - set a very small mass flow at one end with the desired ambient temperature, and define the pressure at the other end to be 1atm. You might also set all 6 inside surfaces of this bounding box as pressures that are all 1 atmosphere (I'm not sure if it will complain about no defined pressure or mass flow though).
Thanks for your suggestion regarding the wind tunnel. Sadly that didn't work for me either. I can't quite figure out where I'm messing this up. I reduced everything down to a simple enclosure with a 100w heater inside and the simulations still reach 1400C. Any idea at all what I'm missing? - Keven
Document2.pdf 25.9 KB
well 100W with no cooling is going to get toasty with no active cooling. I put together a simple sink/source/enclosure model and had it run while I went to lunch and got 600C using 150C as the initial and ambient temperature including radiation and gravity.
Unfortunately the one simulation computer I had available only has a 2007 license so I can't open your model, but I'm attaching my model so you can look at the settings and see if things are the same.
What solids are you using? without a high conductivity 100W is going to be tough to disippate without a large surface area.
enclosure.zip 25.4 MB
I loaded your model, changed it back to external and set the initial (ambient) temp to 85C. I set the initial (ambient) z velocity to 1 ft/sec, which is flowing left to right in the picture.
The results seem okay to me? peak of 750C in the aluminum rods.
The surface of the aluminum will start to melt in the initial stages, until conduction has a chance to dissipate the surface heat source.
box.jpg 282.7 KB
Well that certainly is interesting, simply adding a velocity brought everything in line with expectations, which I suppose in hindsight makes sense, you are never likely going to have completely dead air. What is going to be interesting, which is also why the temperature was set to 25, is that I have an experiment running in the lab duplicating what I have been simulating. I happen to have this enclosure and a couple of 100w resistors. I still am wondering if I'm approaching this simulation from the correct angle. I know (as Chris has pointed out) I'm going to have to employ some active cooling to manage the inside enclosure temperature, so maybe I should just start my simulations with some and work from there - don't know. Thanks for your help. If you have any other suggestions or comments they are always welcome. - Keven
Don't forget to turn 'Gravity' on, or you won't get proper convective cooling, either inside or outside.
At those high temps, the solid will also being shedding heat by radiation, which can be significant so you'll want to enable that.
Although true that objects won't most likely be sitting in an environment that is completely dead air, I don't think applying an arbitrary (even though small) velocity is proper technique. Better questions to ask to match a physical test might be: what was the actual ambient temp and humidity in the testing room; what was the barometric pressure that day; what is the actual efficiency of the heat source components (i.e. is the prescribed heat power accurate).
To answer the best approach to temps inside a sealed enclosure:
You apply a temp, so if you have no sink, then at steady state everything will be at that set temperature. Your sink is the outside. You could simplify the problem doing the calc as an internal flow problem and setting some best guess outside wall condition (maybe a temp, negative heat rate or convective rate and bulk fluid temp) to the outer walls of the enclosure. Your most accurate (but longer) approach would be done as an external flow to solve for the outer wall condition. Extend the computational domain (CD) out far enough so that the resultant boundary temps are about the same as the set ambient. You'll have to include gravity to drive the flow due to bouyancy effects, thus the domain in the direction opposite to gravity will have to be extended more than others. Is the geometry floating in space? Add some table thickness and feet on the enclosure if they exist, bury the CD into the table. Make sure the mesh, especially around the heat sink and heat source components, is sufficient, so use local mesh controls and manual meshing (instead of auto-levels) if that is called for; always create the mesh and turn off solve so that you can view and evaluate(!) the mesh before solving. The original mesh will be based on the geometry but you'll have flow and thermal gradients developing in the fluid where there is no geometry, so refine the mesh using automatic adaptive meshing to capture these gradients. Are the temps getting really toasty, then radiation should have been enabled because this cooling method starts to become significant (unfortunately may have to start the calc over from beginning).
Forced convection is a different story, but actually somewhat easier to solve than a natural convection problem. Make sure the fan curves, flow rates or velocity is actually representative.
Validation examples in the following document is good location to find some setups: "C:\Program Files\SolidWorks Corp\SolidWorks Flow Simulation\lang\english\Docs\technicalreference.pdf"
If your installation language is different than English, you will have to modify the above for it.
Actual model locations are here: "C:\Program Files\SolidWorks Corp\SolidWorks Flow Simulation\Validation Examples"
Be warned that the setups may be set at a mesh level of 8 and take a long time to run.
Hi. I've read Joe's post.
I agree that you shouldn't set wind velocity unless you know it exists.
The general settings attachment (in the earlier post) looks correct. The analysis should be external. Gravity should also be selected.
If you open the enclosure.zip file from Keven then you see that the enclosure is floating.
If you attach the enclosure (or just have it rest on a table) then you have what Joe is describing. Here you need to set the computational domain and bury it in the table. Just like this post: https://forum.solidworks.com/thread/38166
buried the CD in the ground.
However, Keven did not chose to do this.
Joe says you need to increase the CD box. This sounds correct. For the simulation to yield correct results then you need to look at the CD boundary temperature results. They need to be 85 degrees C in this example (since this is what is set as outside air temp).
How can you test this? In the goal setting?
Keven asks for 2 things: 1. Determine the inside temperature of the enclosure and 2. The skin, Outside temperature of the enclosure.
I would like to know who to do this as well.
Since the analysis is external he can't set the thermal coefficient for the enclosure to dissipate the heat to the outside (units in W/m^2/K).. by setting the outer wall condition..external analysis doesn't allow you to do this. Should this be set? Or is this set already because the solid enclosure is defined as aluminum?
Keven has 3 heat sources inside the enclosure set to 100W each. Do a boundary condition need to be set for the heat source , or is setting a heat source enough?
Also, does a boundary condition need to be set for the CD (for the temp outside the enclosure) and the enclosure itself..so you can specify the ( W/m^2/K) ?
I would like to know the answers to this basic simulation and I think it would be helpful for others as well. Thanks.
"They need to be 85 degrees C in this example (since this is what is set as outside air temp). How can you test this? In the goal setting?"
Try to make it as big as one could reasonably while keeping cell count (and thus RAM usage) and solve time in mind. A Surface Goal could possibly be done by creating some geometry and disabling the body in Flow, but just simply creating a cut plot and probing on it is sufficient... I just use visual inspection now as I gain more experience.
"Keven asks for 2 things: 1. Determine the inside temperature of the enclosure and 2. The skin, Outside temperature of the enclosure.
I would like to know who to do this as well."
If you are looking for wall temperatures on the inside or outside walls, I recommend just creating Surface Goals for those. If you want it for the fluid volume inside the enclosure, then follow this procedure: create another part in the assembly inside the entire enclosure, remove any internal solid from that part by a cavity feature; now after part is created it is a solid in the CAD model, but in Flow you can use Component Control to disable the part so that Flow now sees this volume as whatever is behind it (in this case since a cavity is created then it is all internal air); finally create a Volume Goal and make your selections such as min, avg and max temperature of fluid. I recommend hiding the part/volume so that you don't see it in the CAD model but it is still there for Goal purposes.
"Since the analysis is external he can't set the thermal coefficient for the enclosure to dissipate the heat to the outside (units in W/m^2/K).. by setting the outer wall condition..external analysis doesn't allow you to do this. Should this be set? Or is this set already because the solid enclosure is defined as aluminum?"
One cannot set the convection coefficient because it does not make sense in an external flow... the software will calculate all of the localized convective heat transfer for you. So it does not need to be set because it is in a sense already inherently set.
"Keven has 3 heat sources inside the enclosure set to 100W each. Do a boundary condition need to be set for the heat source , or is setting a heat source enough?"
Heat source is sufficient, it will drive the flow by buoyancy effects. If there happens to be some other independent external source of flow then that will also be considered but it is not required.
"Also, does a boundary condition need to be set for the CD (for the temp outside the enclosure) and the enclosure itself..so you can specify the ( W/m^2/K) ?"
No, I think this was explained earlier in my responses.
Thanks for your reply Joe.
I was able to understand a lot more from your responses.
I loaded the enclosure file and was trying to get the 'Cut Plot' like Rich Bayless (he attached box.jpg earlier).
Unfortunetly I wasn't able to get the picture to look correct (see attachment).
There are 3 things wrong in my pic:
1. the heat source (the circles) are not red.
2. my minimum temp is 25 degrees C. ( I checked my setup and see that 85 degrees C is defined for radiation, solid temp, and pressure temp start)
3. There isn't a smooth transition of heat dissipation like Rich's pic.
Can anyone explain why this is?
My maximum heat source temp is only 200 degrees C. but the plot goes up to 743 degrees..similar to what Rich has.
However, when I look at my goal settings then the lowest temp is 85 degrees C.
Not sure what exactly is wrong with the setup. Thanks.
richBayless_pic.png 21.4 KB
Hi. I actually got it working--my 'Cut Plot' picture matches RichBayless'. I disabled some of the settings (disabled radiation and gravity).. this will make the aluminum rods melt. Thanks for all the posts.
Dear Mr Chris Michalski
Hi can you please tell me for your high voltage transformer simulation.
1- do you first run the simulation without enclosure(core and coil only) then put it in the inclosure
2- can you pleasetell me how you setup your study or can you send me one of your assembly with study.
3- dos solidwork simulation tell you what is the temperature of the side panel of enclosure after 1 or 2 hours
4- should i use external study and tick gravity
I would very appreciate any help that you can give me
Hi Habib, might be worth creating your own post with a description of your application and where you're stuck. Based on a quick review:
1. shouldn't be necessary, you can do an external analysis with a sealed enclosure if you want. just make sure that internal spaces are included.
2. will defer to chris. you may want to email him directly.
3. sure, this could be done with a transient analysis.
4. yes and yes.
I'd highly recommend going through the tutorials if you are new to flow. And if you're looking for some one on one help, we do offer that here at Hawk Ridge Systems, feel free to contact me. email@example.com.
Hi dear Jared
Thank you for your help
1) I only ran my simulation with the enclosure on as this was a fundamental part of the project. The transformer was a part of a larger system which was built in this enclosure and other components were as important as transformer temperature.
2) (see attached picture of feature manager and input summary report) This configuration was for stagnant conditions so it does not have any initial velocity conditions. It includes the power dissipated in each portion of the transformer, radiation to the surrounding parts, the heat sink of an external concrete pad, and solar radiation.
3) I only performed steady state simulations to determine the maximum temperatures. You can run a transient to determine the temperature after a set period of time, but this will take longer to complete.
4) Yes, if you have ambient air surrounding the model and air can move from inside to outside you have to use "external". And you need to include gravity in order for the difference in density due to temperature to cause natural convection.
It has been over 3 years since I have worked on those models so it would take a measurable amount of time to provide more detailed information.
Hi Dear Mr Chris
Thank you very much for helping me and I understand amount of time involve in this kind of work
Again thank you I got my answer from your 2 attachment you are very kind.