Community
CFD Forum
Welcome to Autodesk’s CFD Forums. Share your knowledge, ask questions, and explore popular CFD topics.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

No thermal results.

24 REPLIES 24
SOLVED
Reply
Message 1 of 25
JohnTomasik6493
926 Views, 24 Replies

No thermal results.

I've been trying to run a simple static thermal study.  Even with 25X the heat generation applied as boundary conditions, I'm getting no thermal change.  I've gone back through tutorials and previous studies, checked everything I can think of, but I can't identify where the issue is.   Attached is a screen capture showing as much as I could, as well as the flatline temp.

24 REPLIES 24
Message 2 of 25
Jon.Wilde
in reply to: JohnTomasik6493

Hi John,

 

I cannot see any Temperature BC's, so CFD does not have a reference point to start from. If you have heat lost from this box and do not wish to model the external air, the quickest way is through a film coeff. Try 5W/m2/K at your ambient temp on the external faces. (5W/m2/K is an approximation for natural convection, this value would be higher for forced convection externally).

 

Kind regards,

Jon

Message 3 of 25
JohnTomasik6493
in reply to: Jon.Wilde

Jon,

 

What temp boundary conditions do I need?  I referred to the Sim CFD "Electronics" tutorial when setting this up, and the only boundary conditions they had that were temp generating were three "Total Heat Generation" conditions.  They did not have me apply any surface temps in that tutorial, if I remember correctly.  In that tutorial, the "Total Heat Generation" BC's created a change in temperature in that study.  I have two of the same BC's in my study, but, it is not creating a substantial change in temp (it's on the order of E^-13).  I did try to apply a temperature boundary condition to my outside air, but then the whole study simply remained that temp throughout the analysis.

 

At the wattage I applied, this thing should be on fire.

 

 

John

Message 4 of 25
Jon.Wilde
in reply to: JohnTomasik6493

Hi John,

 

It should have had a temp on the inlet, along with a flowrate.

 

For this, use what I said. Film coefficients - if you have no actual inlets or outlets.

 

Kind regards,

Jon

Message 5 of 25
JohnTomasik6493
in reply to: Jon.Wilde

Jon,

 

Applying a temp on either inlet or outlet produced results.  If I set gravity with the temperature BC at the "inlet" side, the temps would skyrocket.  A 20C temp with about 1.5W of heat generation on the board would send temps beyond 500C.   If I placed the temp on the outlet side, I got more reasonable results.  I went back into some of the tutorials, and I noticed temps were on all surfaces of the air external volume, yet those studies (with heat generation on the order of 5W+) didn't do that, even though the temp BC was also on the inlet side.  I'm trying to compare studies thoroughly to understand this. 

 

Let me describe the situation.  The client has 3 boards they've prototyped and ran in the lab (outside of an enclosure, exposed to ambient air in the lab).  They've taken thermal image photographs.  They're able to give me input power and also Jc and Jb for some components.  I'm trying to replicate their results, because we'll eventually take those three boards, put them all in one enclosure, and put them in outdoor environments in a variety of environmental temps.  I'd like to be able to quickly predict hot spots in those conditions on the boards, and create thermal conductor solutions to relieve those hot areas and minimize component temps.

 

I thought I'd use an external air volume and get an idea what my heat generation loads on the hot spot chips (identified in the thermal photographs) needed to be to reproduce the thermal image.  

 

If I use the film coefficient, I can't use a two-resistor (compact thermal model).  This might produce questions by the client.   I'm just guessing.

 

I'm setting up that analysis now and am going to run it.  I'll post updates.  But, in the interim, I'd like to know what I need to show/upload so that someone can tell me why I see over 500C from the board if that temperature BC is put on the "inlet" side of the air space, where it doesn't do the same in the tutorials.

Message 6 of 25
JohnTomasik6493
in reply to: Jon.Wilde

Jon, to use the film coefficient, and since this board is presently being tested on a bench in open air, are there any rules of thumb that will help me estimate air volume/size/aspect ratio around the board?  In fact, are there any guidelines that would help me size an air space around any object so that I'll get the closest results to an open-air environment?

Message 7 of 25
Jon.Wilde
in reply to: JohnTomasik6493

Hi John,

 

I suggest you refer to the guide here for domain sizing.

 

If this is a natural convection study, is the unit placed on a bench or will it have airflow beneath it also? It looks as though it will have air all around it so you should use the 'chimney approach'.

 

This means Ambient Temp and a P=0 BC on the bottom surface and just a P=0 on the top surface of the air domain.

 

Feel free to share a CFZ (support/share) file once you have it setup.

 

Kind regards,

Jon

Message 8 of 25
JohnTomasik6493
in reply to: Jon.Wilde

Attached is the CFZ file.  Note the lack of temperature differential on the board.  The real-life unit has a delta T on the board assembly of at least 30C.  

Message 9 of 25
Jon.Wilde
in reply to: JohnTomasik6493

Hi John,

 

You have air set to fixed, so it was only a conduction analysis. Select the air and switch to variable so that the density can change.

 

 

Air Variable.jpg

 

With that change the model looks like this after 100 iterations. You can also set the temperature scale to the board by right clicking on the legend and choosing 'set to part' like I have below. You do have a rather conductive PCB so that may explain the uniform temperatures. It is mainly copper.

 

PCB Temps.png

 

I hope that helps.

 

Kind regards,

Jon

Message 10 of 25
JohnTomasik6493
in reply to: Jon.Wilde

Ahhhh....basic gas laws stuff.  I'm feeling real smart about now....lol.  Thanks much, Jon.

Message 11 of 25
Jon.Wilde
in reply to: JohnTomasik6493

Hi John,

 

No problem, it is easy to miss these things.

 

Kind regards,

Jon

Message 12 of 25
JohnTomasik6493
in reply to: Jon.Wilde

Jon,

 

Attached are two files for your review.  I've used variable air for the fluid material, and the result for the study using the film coefficient, with the suggested air space provided by the program, was much more representative than what I saw before.  The thermal drops across the board looked good.

 

However, I have a few questions, and here is the first.  Attached are two share files using the ambient air/0 pressure approach (not the film coefficient).  I noticed that if gravity was applied with the thermal load on the downstream side of the air (i.e., gravity was in the direction of the face of the thermal load), the thermal result was much larger than if gravity was in the direction so that the thermal load was on the upstream side.  I'm curious why this happens?  I would've thought that gravity would carry the thermal load away from the air space in the first condition, but it seems to be the opposite.  

Message 13 of 25
Jon.Wilde
in reply to: JohnTomasik6493

Hi John,

 

To be honest, these models are not set up in such a way to be useful.

 

The air domain is far too small and we do not run with pressures on the side walls.

 

My suggestion is to stick to the recommended setup, which sounds like it works well for you. Tt did look well set up how you had it previously.

 

Kind regards,

Jon

Message 14 of 25
JohnTomasik6493
in reply to: Jon.Wilde

Will do.  

 

 

One other (hopefully last for this analysis) question: you guys recommend static pressure with the thermal load on the inlet side per the air volume dictated on the below web page link for an air-suspended device.  

 

http://help.autodesk.com/view/SCDSE/2014/ENU/?guid=GUID-E0609A21-541D-4D11-9663-93476E26CF8F

 

 

The reason I ask is I'm trying to determine the heat generation of the devices on the board by attempting to replicate the results of their emperical study with their lab boards.  But, these boards will be combined in an enclosure and table mounted, so in that case I imagine I'd use the recommended setup, which is a film-coefficient approach.  So, would it be safe to transfer those same pre-determined heat generation from the previous study to this new study?  I'm assuming the first study has given me a heat-generation load that was backed-into thanks to the emperical work guiding the initial study.

 

 

I hope that makes sense.

Message 15 of 25
JohnTomasik6493
in reply to: Jon.Wilde

Jon,

 

Attached is a file of an analysis with the air space modeled with the recommended aspect ratio.  The thickness of the board isn't very much, so the air space isn't very thick itself.  It seems that the board generates a lot of heat for very little power.  I'm wondering if there's some other adjustment to the air space aspect ratio that isn't mentioned in that instruction you provided?  Also, the heat is pulled towards gravity, and I doubt that actually happens.  What am I missing?  Should the air space be thicker than your site's recommended 5*X dimension, and if so, by how much?   Again, my objective is to figure out how much thermal heat power is being generated by the chip to result in matching the thermal output of the actual board.  It's important the software provide that info.

 

 

John Tomasik

Message 16 of 25
Jon.Wilde
in reply to: JohnTomasik6493

Hi John,

 

I see what you mean. Yes, we should make this thicker. I would have the width or the air normal to the PCB about half that of the other width.

As it is setup, I expected gravity to be acting in x direction - typically we have more air above the unit - so we can capture the plume.

 

Also keep an eye on your mesh - you only have one element across the thickness of the air volume here, which will probably prevent CFD from finding the correct solution. Once you have a larger domain this should improve.

For improved accuracy through the heatsink we should also ensure we have a mid-node within the solid - a uniform mesh would help you achieve this.

 

If you are trying tro replicate results of this unit within a container - might it be better to model this also and then mount it on a table and use the 'bucket' approach?

Message 17 of 25
JohnTomasik6493
in reply to: Jon.Wilde

Jon,

 

The boards I'm replicating to determine the thermal energy of the chips under operation are development boards, so they are simply on a lab bench, suspended by an edge in a board vise.  The project's path is for me to determine the heat energy of the components based on their operation, then help design board layout and enclosure/thermal conductor design prior to any board design for manufacture.  We're trying to do as much predictive analysis as possible.  Two of the three boards will be combined into one in the production design.  So, there are quite a few mechanical changes to what we have now.

 

My questions are:

 

1.  Can I "back in" to heat power output by the chips using this comparitive approach, and

 

2.  If I transfer those heat power outputs to the same chips in a different board assembly where I place it in a box, I'm assuming the thermal analysis will remain accurate, right?

 

 

John Tomasik

Message 18 of 25
Jon.Wilde
in reply to: Jon.Wilde

Hi John,

 

When you test this unit I guess it would be sitting on a bench - at that stage we would want to model the bench and use the 'bucket' approach - so just the top of the domain is open. To improve this comparison, it may be wise to use this approach for all of the studies.

 

  1. I do not really understand this question, would you mind elaborating?
  2. I am not sure I understand this either, as it follows on from the above..

Thanks,

Jon

Message 19 of 25
JohnTomasik6493
in reply to: Jon.Wilde

Jon,

 

The boards are suspended by an edge in a vise, elevated off of the bench about 8".  We did this so the bench was a small influence on the thermal image.  I believe the "suspended in air" approach applies best.

 

 

We have difficulty determining what heat energy each component will generate when we operate the boards.  We do know what input power is required, but we don't know exactly how much heat each component produces as waste.  Arriving at those values is difficult, using only our electrical design team's knowledge of how they're controlling the components as well as the manufacturer's information.  So, I'm trying to figure out how much total heat energy each component creates.  I'm using the approach of:

 

 

1.  While testing the boards, we took thermal images with a camera that showed temperatures of the boards and the components located on them.  Since I then have a defined mechanical environment (suspended in air), known board and component materials, and now a heat energy output, I believe I have enough information to build the model in the software, and adjust my applied heat generation load to the appropriate components until my analysis model produces a similar thermal image.  That is telling me what heat those components generate during operation, right?

 

2.  I'm assuming my next step would be to apply those total heat generation values arrived at in step #1, and I apply it to the the production board layouts we are planning on creating.  This produces a new thermal image, which tells us what temperatures to expect for each component when they're mounted in their new arrangements for production.

 

 

Does this sound reasonable?  If not, given the fact that we don't know inefficiencies of each component, how would I determine total heat generation by each component to run a predictive analysis?

 

 

John T.

Message 20 of 25
Jon.Wilde
in reply to: Jon.Wilde

Hi John,

 

This is possible, although I would have thought it would be quite difficult to find the exact values. Like you say though, if you do end up with volumetric heat loads applied to various chips that give you results you are happy with, you could carry these over to a larger assembly.

 

To be honest I have never seen anyone work backwards in this way.

 

Best regards,

Jon

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report