[Tech]

Hi everybody,
I carried out a CFD simulation of an electronic device using FloWorks.
Now I'm comparing the results of the simulation with the real thermal measurements got from the first real prototipe.
The data came out from the software simulation are quite different respect the real measurement.
In the electronic device there are two axial FANs to cool the electronic components and it seems that the temperature of the component near the two FANs is overestimate (more than 40% respect the real thermal measurement).
Is it possible that Floworks in case of air turbulence has some difficulties to estimate the temperature of the electronic components?

Thanks if someone can help me in this topic.

[Boris_M]

This can have several reasons.

How close is the fan to the next flow blocking component?
The fan curves don't work well if you have a component blocking the fan partially and therefore disturbing the flow too close to the fan. The fan curves works by pressure difference and if the pressure at the fan surface is disturbed unevenly due to the partial blockage the volume flow rate is wrong.
Imagine the fan is half blocked by a heat sink that is very close to the fan. The heat sink cause a higher pressure between the fan and the heat sink but the part of the fan that is not blocked has a lower pressure. Now the pressure on the fan outlet is calculated in an average and therefore somewhere between the higher and lower pressure at the fan and also the pressure difference is then at the wrong part of the fan curve, causing either a higher or lower flow rate.
In your case I could imagine the air flow is too low and therefore the pressure was too high.

Other reasons might be due to wrong setup but if you are experienced with SWFS then this might not cause the issue.

Boris

[Tech]

Hi Boris,
yes, there are two FANs placed very close to electronic components, you can see a detail in the picture attached.

In our devices, but also in general, we need to reduce the outline dimensions and compact the electronic components, often we have problems in terms of dissipation and cooling of electronic components.

I've checked the value of the pressure drop and the flow rate of the FAN, the equivalent working point does not match with the FAN curve.
It seems that pressure drop is too high respect the flow rate or vice versa (picture #2) .
It could be the reason for the over estimated temperature of the electronic components?
From the solver I didn't find any type of error for the FAN component?
What is the maximum deviation of the FAN curve acceptable for Flow simulation?

What is the possible solution to evaluate better the performance of the FAN in these cases and get better results in the temperature of electronics components?

Is it a limitation of Flow simulation or it is a common mistake in all simulators?

I appreciate your collaboration in this topic.
Kind regards

[Boris_M]

Hi Tech,

yes, that's what I thought, too close and too much blocked by the geometry after the fan. The best way of doing it in this case is ideally simulating the fan as actually rotating as the error is then much less.

Did you measure the flow rate and pressure for the other graph with the working point?
If you use a surface plot on the fan outlet surface and plot the pressure, you should be able to see an uneven distribution.
Unfortunately for fan curves I don't think there is a solution for that as you face the issue that the part that is blocked should work in the left part in the graph and the part that is not blocked should work in the right part of the graph. In reality the flow is backed up on the bottom part which the fan curve doesn't know as it just sees the average of the whole surface and not pieces of it.

The way the fan curve works is that depending on what type of fan curve boundary condition you use it uses the inlet pressure either specified or coming from the calculation in case of an internal fan and the pressure from the outlet fan for the pressure loss and then according to the graph uses the flow rate for the inlet boundary condition. This of course is iteratively so it can only use the pressure from the previous iteration for the flow in the next iteration. But in a converged state there shouldn't be a big difference.

Boris

[Tech]

Hi Boris,
Do you suggest to replace the Fan Smart part with a rotating geometry?
Please clarify, thanks.

[Boris_M]

Yes, this should give you better results.

Boris

[CFDfan]

Originally Posted by Tech

Hi Boris,
yes, there are two FANs placed very close to electronic components, you can see a detail in the picture attached.

In our devices, but also in general, we need to reduce the outline dimensions and compact the electronic components, often we have problems in terms of dissipation and cooling of electronic components.

I've checked the value of the pressure drop and the flow rate of the FAN, the equivalent working point does not match with the FAN curve.
It seems that pressure drop is too high respect the flow rate or vice versa (picture #2) .
It could be the reason for the over estimated temperature of the electronic components?
From the solver I didn't find any type of error for the FAN component?
What is the maximum deviation of the FAN curve acceptable for Flow simulation?

What is the possible solution to evaluate better the performance of the FAN in these cases and get better results in the temperature of electronics components?

Is it a limitation of Flow simulation or it is a common mistake in all simulators?

I appreciate your collaboration in this topic.
Kind regards

Tech,
1. how/where did you get the pressure - on the fan's air-in surface, or on the fan's air-out surface, or you calculated it as a difference between the pressures on the air-in and air-out surfaces?
2. Did you average the pressures on these surfaces?
3. Did the solid model of your fan have a hub?

[Tech]

Hi CFDfan,
I used the FAN Smart part of Flow simulation, I created a new item, imported the PQ curve from the data sheet of the vendor, fixed the FAN speed, then I associated this feature at the geometry as internal FAN. The air inlet pressure is calculate from the system starting from environmental set up. The air outlet pressure is calculated from the system as the result of the impedence made from the electronic components placed after the FAN.
The pressure drop of the FAN is calculate sa difference between the two pressure.
The pressure of the two surface is an average and it is an output from FlowSim.
Yes, the solid model of the fan has a hub where I apply 1.5 W as power loss relative to the Fan.

could you suggest some ideas to solve this issue? The error in the Electronics temperature placed after the fan is aroud 40% and it is not acceptable.
Now I'm tryng to replicate the PQ curve only with a fan inside a simply tube and seem that the re are some error in the Flowsimulation computing.
Do you have experience with this software?

[CFDfan]

Originally Posted by Tech

Hi CFDfan,
I used the FAN Smart part of Flow simulation, I created a new item, imported the PQ curve from the data sheet of the vendor, fixed the FAN speed, then I associated this feature at the geometry as internal FAN. The air inlet pressure is calculate from the system starting from environmental set up. The air outlet pressure is calculated from the system as the result of the impedence made from the electronic components placed after the FAN.
The pressure drop of the FAN is calculate sa difference between the two pressure.
The pressure of the two surface is an average and it is an output from FlowSim.
Yes, the solid model of the fan has a hub where I apply 1.5 W as power loss relative to the Fan.

could you suggest some ideas to solve this issue? The error in the Electronics temperature placed after the fan is aroud 40% and it is not acceptable.
Now I'm tryng to replicate the PQ curve only with a fan inside a simply tube and seem that the re are some error in the Flowsimulation computing.
Do you have experience with this software?

1. Yes I have long experience with SWFS, but I have never bothered to check the operating point of the fan, so no input there. It is a good time for Boris to interfere to confirm if your measurement setup of the pressure/airflow is correct, i.e. it is the one determining the operating point of the fan.
2. You are talking about 40% error (higher temperature) of the components near the fan. What about the components further away from the fan. What is the error there?
3. I wouldn't put 2.5W loss in the fan's hub. If this was the power consumed by the fan at full speed then it was wrong because most of that power gets converted into mechanical power to push the air through with very small thermal loss which can easily be ignored.
4. If you are referring to 40% error in the temp. of the CM chokes near the fan, remember that the surface of these chokes is very rough (because of the magnet wire).. their cooling area is significantly larger than the cooling area of your "smooth" choke models. Finally try with enabled radiation from the surface of these chokes with a reasonable emissivity (say of 0.8) and see what happens.
5. One final thing is to increase mesh density (resolution level of 5 or 6) and see if this changes anything.

[Boris_M]

I heard my name :-)

1. It depends on what type of Fan you've used. If you created your own fan, you can select what pressure drop was measured. You can select between Static pressure increase, Free blowing pressure increase and total pressure increase.
You can have a look at "Fan - Basic Information" in the Help of SWFS by clicking on one of the "?" in the menus of a boundary condition and search for it.
Depending on what pressure difference you measure in FloEFD or was measured in the fan data sheet you might be using the wrong one.
For an external inlet fan the pressure and temperature you specify in the BC is what is applied at the inlet of the fan. FloEFD measured what pressure is at the outlet surface and determines where on the curve the fan is running.

2. As far as I understood the error is only close the fan so the fan curve problem compared to an actual rotation is my first guess where the deviation comes from.

3. I also never did that. I'm not sure if it will make a big influence, I never tried it.

4. Radiation could play a big role in general and you can use surface parameter to evaluate how much radiation was emitted from a body compared to the convective portion from the fan to see how big of an influence it plays in relation.

5. I would avoid simply using the automatic mesh settings and use 5 or 6 etc. I usually run a level 3 mesh to get the first idea of how it looks and then apply local meshes and the manual settings.
If you work with the same application every time, you will get some feeling for the mesh settings and don't run the level 3 for the first start but jump right in to your manual mesh and local mesh settings. For me I have different models every time and usually they are not my models and therefore it is easier for me to look at the mesh in a cut plot sliding through the model to identify the quality and some areas of improvements.

Boris

[CFDfan]

Originally Posted by Boris_M

I heard my name :-)

1. It depends on what type of Fan you've used. If you created your own fan, you can select what pressure drop was measured. You can select between Static pressure increase, Free blowing pressure increase and total pressure increase.
You can have a look at "Fan - Basic Information" in the Help of SWFS by clicking on one of the "?" in the menus of a boundary condition and search for it.
Depending on what pressure difference you measure in FloEFD or was measured in the fan data sheet you might be using the wrong one.
For an external inlet fan the pressure and temperature you specify in the BC is what is applied at the inlet of the fan. FloEFD measured what pressure is at the outlet surface and determines where on the curve the fan is running.

2. As far as I understood the error is only close the fan so the fan curve problem compared to an actual rotation is my first guess where the deviation comes from.

3. I also never did that. I'm not sure if it will make a big influence, I never tried it.

4. Radiation could play a big role in general and you can use surface parameter to evaluate how much radiation was emitted from a body compared to the convective portion from the fan to see how big of an influence it plays in relation.

5. I would avoid simply using the automatic mesh settings and use 5 or 6 etc. I usually run a level 3 mesh to get the first idea of how it looks and then apply local meshes and the manual settings.
If you work with the same application every time, you will get some feeling for the mesh settings and don't run the level 3 for the first start but jump right in to your manual mesh and local mesh settings. For me I have different models every time and usually they are not my models and therefore it is easier for me to look at the mesh in a cut plot sliding through the model to identify the quality and some areas of improvements.

Boris

Thank you Boris, very educational.

5. Is you concern about the automatic resolution level of 5-6 just related to larger computer resources and simulation time, or you always prefer manual and local meshes to the automated ones?
I personally use automated local meshes with higher (than the global setting) resolution factor. The manual meshing is probably the best but I am just lazy.

[Boris_M]

My concern is less about the larger computer resources but there are some methods behind the automatic settings that change at a certain level and simply include the adaptive refinement only. It is automatic not extremely smart.
If you get more experienced with the mesh settings you often can create a resource saving mesh for high accuracy much better than the automatic settings. In many applications level 3 is good enough but often the automatic settings can cause high levels cells at body edges where it is not really necessary. Especially where you have not important geometry detail that suddenly gets a lot of cells that are wasted and cause higher CPU time for the solver. For example the automatic settings try to resolve the geometries that have a boundary condition applied to. Now if one of the components has for example a radiation property applied to on its surface, some surfaces in a CAD model can be very small due to the way the geometry is created. The automatic settings will then sometimes increase the small feature refinement level to 6 or higher and this setting is valid for the whole computational domain so every small edge is resolved with fine cells although not needed. Therefore I usually leave the automatic settings and the settings you find then is what was behind the automatic settings. If you chose a higher level automatic settings the mesh definition with automatic settings switched off also change according to what would apply behind these settings. Then you can easily see if some of the levels are just way too high and reduce them manually.
If you run a mesh first time and have a look at the mesh you can easily spot regions where you need a little finer mesh and with a local mesh you just select either fluid or solid cells etc. 1-2 level finer. Done.
In the latest version you are able to use geometric shapes for local meshes without creating a separate body. This is very convenient as it is done very fast.
Sure if you are lazy and don't care about 1-2 more hours of CPU time for the solver then this is not a problem but if you get close to memory limits or need results faster, 10 minutes of manual meshing can save 2 hours of solver time or more. Depending on model etc.

Boris

[Tech]

Hi,

1- I cretaed a new own FAN as axial fan coping the data from an other similar FAN and updating the PQ graph with the data get from the actual FAN manufacturer.
I made a trial to simulate many point of the PQ graph in a separate file usin a the same FAN geometry inside a simply tube.
The result of the plotted data got from this calculation is quite different you can see the new picture attached.
The pressure drop is the difference between the inlet static pressure and the outlet static pressure (please correct me if it is wrong)
In my actual product the FAN is an internal FAN since I hace a fan guard applied in the inlet surface of the FAN.

2- The error is about 40% in the temperature of the component after the FAN ( from 5 to 100 mm) and decrease to 10% in the components placed far from the FAN (we can define between 100 and 200 mm).
I consider 10% acceptable but not acceptable an error of 40% (40% means 25-30°C and it is a big value).

4. I made a trial appling the emissivity of 0.8 on the surface to the inductances and I got an improvement of 5-10% (6 to 10°C).

5. I set the meshing at 3 and i made several manual refinement in the most critical components.
If I set an automatic mesh to 5-6 I think that the PC can't do the computing.
I have to simulate a PWA with several electronic componets, heat-sink and also some SMD componets that I need to measure the temperature.

Do you have any other suggestion to improve this simulation with SWFS?
Do you have experiace with other CFD software? What do you think of ANSYS? Could be more precise in the simulation of PQ FAN?
Thanks

[CFDfan]

Originally Posted by Tech

Hi,

1- I cretaed a new own FAN as axial fan coping the data from an other similar FAN and updating the PQ graph with the data get from the actual FAN manufacturer.
I made a trial to simulate many point of the PQ graph in a separate file usin a the same FAN geometry inside a simply tube.
The result of the plotted data got from this calculation is quite different you can see the new picture attached.
The pressure drop is the difference between the inlet static pressure and the outlet static pressure (please correct me if it is wrong)
In my actual product the FAN is an internal FAN since I hace a fan guard applied in the inlet surface of the FAN.

2- The error is about 40% in the temperature of the component after the FAN ( from 5 to 100 mm) and decrease to 10% in the components placed far from the FAN (we can define between 100 and 200 mm).
I consider 10% acceptable but not acceptable an error of 40% (40% means 25-30°C and it is a big value).

4. I made a trial appling the emissivity of 0.8 on the surface to the inductances and I got an improvement of 5-10% (6 to 10°C).

5. I set the meshing at 3 and i made several manual refinement in the most critical components.
If I set an automatic mesh to 5-6 I think that the PC can't do the computing.
I have to simulate a PWA with several electronic componets, heat-sink and also some SMD componets that I need to measure the temperature.

Do you have any other suggestion to improve this simulation with SWFS?
Do you have experiace with other CFD software? What do you think of ANSYS? Could be more precise in the simulation of PQ FAN?
Thanks

1. I didn't get if the simulated temperatures are always higher than reality or they go above and below (for the 10% error components)?

5. Another source of error in your case could be the fan guard you have. Is it properly simulated, with the correct free area ratio, geometric pattern, thickens, etc? Also for the pressure take the difference between the fan's outlet and the ambient pressure (not the fan's inlet pressure as you've done) and see if this matches the entered fan curve. If yes then ask master Boris why is so.

If you use SW for your mechanical design then SWFS is teh best there is in my opinion (I work in electronic cooling area as well). Master Boris was promoting FlothermXT which is tightly integrated with SW as well, but I don't have experience with it. It uses however the meshing and the engine of FloEFD (basically the same as SWFS), so you could expect similar results there, but its libraries are more tailored to Electronic cooling applications.

Forget about the general purpose codes (Fluent, CFX, CCM+ ESI-CFD, etc). They are too unfriendly for your application with old fashioned UI and if you are not working with them every day they will become pain on the ass. In addition they are obscenely expensive.

I've heard good words about the HeatDesigner and scStream from Cradle-CFD, but have no experience with them.

[Boris_M]

1. As I mentioned, in the help of SWFS you'll find a table that shows you how the pressure difference for the fan is defined. If you used the Axial fan then the pressure loss is "P_static outlet - P_total inlet" for the radial and fan curve you can chose the pressure loss definition, so if it is the same as mentioned above or total pressure increase or static pressure increase.
From your graph it looks to me that at very low pressure loss the graph fits only at higher pressure loss the difference gets bigger and that could imply a unknown pressure component. I would say you should try to use a "fan curve" definition and test the other pressure difference settings, depending on what you get from the datasheet.

2. Looking at your graph and considering the pressure loss is higher due to the blockage, the horizontal difference (volume flow rate) between the test and the original data shows a lower flow rate in the simulation which would result in not as much cooling power and therefore higher temperatures.
SWFS uses the data from the fan curve as it is, if you get other volume flow rates vs. pressure drop then the most likely issue for me would be the difference in the pressure drop definition you measured and SWFS uses as per definition in the software.

4. Sure the emissivity can improve it but only a little it seems. I think the issue is really with the fan curve definition.

5. Yes, if the computer RAM is the limitation than a manual mesh setting and some local ones can help control the mesh size much better than the automatic option.

As for other CFD tools, of course there are other that can do the job as well but as always every tool has their advantages and disadvantages. SWFS is directly in SW and works based on your geometry. Before you jump to another tool you should carefully sort out the issue you have and see if it is a user problem, a bug or simply a limitation for the software. It might take some trials until you get it sorted. Ideally you should send the model to the support and ask them for help. If you just go for another software and have to start learning it first and get to the point you are now with SWFS it takes you weeks and you might end up having the same problem there because you do the same mistake if it really was a user error.
I would say try the other fan curve definition with the different pressure drop setting and see if it works. If it works, you saved yourself a lot of time and money to switch from one tool to another. If it doesn't, I can only offer you to look at your model but I guess it is confidential so talk to your SW support as it is getting harder and harder for us to help with wild guesses to find the error without being able to look at the model and find the problem. We'll keep trying but often there might be something that you didn't mention at all such as another boundary condition which causes this which we didn't know about.

Please try the other fan curve setting and let us know.

Yes, FloTHERM XT uses FloEFD/SWFS mesher and the basic solver but has more electronics cooling features and possibilities than FloEFD/SWFS which come from the FloTHERM product. FloTHERM is one of the market leader in electronics cooling and XT was developed to get a closer CAD link and handle more complex geometries such as design aspects better. The user interface for FloTHERM XT is different from FloEFD/SWFS, only the CAD side stays the same.

Boris

[CFDfan]

1.I run an old model with a front fan guard and found that if the pressure is calculated as the difference between the fan's outlet pressure and the ambient pressure (not the fan's inlet pressure as Tech does) then the fan characteristic generated by SWFS matches almost perfectly with the one in the fan's library

Regarding the temp. error in some of the components we all forgot the biggest source of error - our own estimation of the power loss in these components. In Tech's case, who's model is of a switched mode power supply, he got most probably the power loss in the components from a circuit simulation which inevitably added another level of error and uncertainty (compared with the reality).

I somehow assumed that Tech knows precisely (in terms of reality) the power loss in each component, but thinking more about that and being in this (power electronics) business for a long time I know this cannot be the case.

In short, I wouldn't blame the code.

P.S. Boris I've got a question - Normally one would use internal analysis in cases like Tech's. How in such (internal analysis case) to consider the heat transfer (radiation + convection) from the enclosure (enclosing the internal solids and the fluid) to the ambient. I know if I select external analysis this can be done naturally at the expense of more cells and calculation time, but I wander if there is another, besides the heat transfer coefficient in the wall property, way to do this in internal analysis cases.

[Boris_M]

Ok, Just to make sure we are correct here I did a quick test with the Tutorial model of the electronics enclosure and moved the heatsink and chip closer to the fan curve inlet and also made it in another simulation much bigger to block it even more.
So we have three data points, one in the far distance and original size, one much closer in the original size and then again much closer but bigger and therefore more blockage.

The fan in the tutorial is an axial fan from the database (Pabst 412), which means the pressure difference is the "P_static out - P_total in". Since the inlet is not calculated inside the computational domain and is in the outside environment the total pressure there is basically the environment pressure.

I posted several images below that shows the change in the location and the size of the heatsink and also the Excel evaluation of the model results where I used a goal to get the static bulk average pressure and volume flow rate at the outlet of the fan which is blowing into my enclosure.
You can see the three points are even exactly on the fan curve no matter how much the heat sink blocks the fan. So the error might even be much smaller than I expected. I never tried it and thought it would influence the result but it doesn't really seem to influence it.
So I guess it really is a problem with the boundary condition of your component as CFD-Fan suggests. (You never learn out )

I think you said in another post you measured current and voltage to the component or got it from somewhere. This is the overall power consumption but you have to consider that this is not the heat loss. Just like in an LED the power you supply it with does not necessarily represent the heat loss like in a resistor. An LED has some optical power that generates the light and if you use some coils then some of the power is put into the magnetic field generation. So you have winding and iron losses which should only be part of the full power supplied to the coil.
I would guess your electronics colleagues should be able to calculate these losses or maybe you can do it yourself. Usually it is in dependency of the frequency if it is a AC current and some other factors and there might be even something in the datasheet or something you can get from the vendor.

Just do a test and put a constant temperature on the components that are so far off and see if the temperature of the ones in the back of the enclosure are more accurate now. The hotter air from the too hot components might have influenced also the components in the back to be 10% off. You can then also just check what power dissipation the constant temperature would emit in heat and radiation to see how much % of the power it is that you applied to get a feel of how efficient the component is and see what you can get from the datasheet or your hand calculations etc.

Boris

[Tech]

Hi,

A. All the components temperature are always higher than reality, from 40% to 10%. I didn't find temperature below the reality measurements.

B. Regarding the fan curve I did the correction in the pressure calculation, I need time to rum the calculation and get the new data.

C. The power loss are in most components an estimated data, for this reason I consider acceptable an error of 10% in the final data get from Swfs.
I can't accept a deviation of 40%....since the error in the power loss extimation could be 3-4% max.

D. My simulation si anche internal simulation but I applied 5 W/m2 as thermal transmission between the wall of the enclosure and the esternal ambient. Could be reasonable this value for the transmission in conventional air?

C. Regarding the choke, it is made With core and external copper winding, so my 3D model May be too to semplified, the external surface in contact with the air in the reality is much than the simulated model. Is there a way in Swfs to increase the thermal transmission of the simulated sempified model?

D. Regarding the electrolitic capacitors, what kind of material do you apply for it ?
it is Made With a can in aluminium and the internal winding foil is not in contact with the external case. Do you have suggestion?

E. Regarding the active components, like mosfet or diode, I used the 2R Smart part included in Swfs. Is it correct to evaluate the Tj using the Tmax of the 3D model ? Do you have other suggestion to misure the Tj of the Mosfets.?

Regards

[Boris_M]

Hi,

C. If you are certain that your assumptions are 3-4% then I have to take your word on that because I cannot check what you did or how you did it. So all my answers will be based on that.

D. This could be a good enough estimation.

2nd C. You can manually define the heat transfer rate just like you did it for external case but that would overrule the fan cooling on those components because you specify a heat transfer instead of using the calculated one from due to the flow from the fan.

2nd D. I have no idea what material should be used for that. I'm not that familiar with electronics materials of single components and what is usually used. Try to find something on the internet or ask the vendor/datasheet in case there is anything on it.

E. 2R model is not as accurate as the more detailed models in FloTHERM but should give you results within 10%.

Boris