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: 

Strange results.

17 REPLIES 17
SOLVED
Reply
Message 1 of 18
JohnTomasik6493
911 Views, 17 Replies

Strange results.

I modeled a simplified version of a PCBA we're already testing in the lab.  With ambient conditions at 26C and a power input of 5.4W with a 100% duty cycle, the thermal image indicates a chip temp of about 131C.

 

I modeled this in the software, applied the same boundary conditions, and the first 100 iterations produced a chip temp of about 500C.  I used an air volume aspect ratio using the Autodesk suggested info.  I thought maybe it didn't have enough iterations to converge properly, so I hit run again, and this time the temp shot up to 5500C  (yes, that's 5500C).  Here's a link to the analysis and the results (it's almost 10MB, so I can't upload it here):

 

http://a360.co/1jEvjMc

 

 

What's the deal?  I am REALLY struggling to replicate what we're seeing in the lab, and I'm on the hot seat to create a predictive analysis of the entire board assembly.  I must deliver this within 2 days (no, not this simplified version).  I'm finding small alterations in just the air volume changes the results significantly, so I'm losing confidence we can use this tool in a predictive scenario.  Now I ran into this "result", which is completely out of range of any reasonable estimate of what we should be getting from the software.

17 REPLIES 17
Message 2 of 18

Oh, I noticed my materials were wrong for the air (don't know how air emissivity was the "default"), but even changing it to "variable air" still results in unreal numbers (+2000C).  

Message 3 of 18

And two more studies.  I noticed I didn't have the variable air environment set.  Regardless, I'm still getting high temps (coolest was around the 205C range).  

 

I noticed if I oriented the board vertically, my temps doubled, which isn't what we see in the lab.

Message 4 of 18

I went ahead and created the assembly, even though I have concerns about the results I was seeing and spoke to in this thread already.  I've attached the CFZ.  At ambient (22C), that one chip (which reached 131C in real life, and was off the map in the above studies) only got to about 120C.  When I elevated the ambient temp to 85C, that chip only reached 115C, which is 5C less at the much higher ambient temp?  How is that possible?

Message 5 of 18
Jon.Wilde
in reply to: JohnTomasik6493

Hi John,

 

I have been looking at the vertical model only. Ideally we need to change the box size, it needs to be wider.:

 

Vertical.png

 

Right now the mesh is too coarse, at the outlet we only have 2 elements across the width, with a wider box also we should aim for at least 10 or so. Ideally we do not want to see any strange velocity profiles when we view the results on a cut-plane, if the mesh is too coarse, this is exactly what we will see.

We also need at least 2 elements through the thickness of each solid part.

 

You had gravity set as components, when it needs to be 'earth' with a 1 value (and I did the exact same on a different model today, very easy mistake to make).

I would run with the Mixing Length turbulence model with natural convection.

 

With these changes (I did not change the box, for some reason it made the model hard to manipulate, easier to draw it in CAD) I got max values of 89C:

 

Temp.png

 

As an aside, the horizontal box must also change size, we need a larger space above the unit:

 

Horizontal.png

 

I hope this helps.

 

Kind regards,

Jon

Message 6 of 18
JohnTomasik6493
in reply to: Jon.Wilde

Jon,

 

That helps, although in real life, that chip's temp in those conditions is 131C.  If you have any thoughts of why the inaccuracy, let me know.  

 

My concern remains that as I alter the air space beyond your recommendations, I'm increasing uncertainty in accuracy of the results.  I've been playing around with different air spaces beyond your recommendations, and the results can be quite different.  Short of my having to show up here begging for guidance, and then relying on your remote input, is 10 elements the magic number that'll provide an accurate study?

 

When I'm in the setup mode, and I've autosized the mesh, do I assume that each teal dot is a node of the mesh?

 

 

Last, attached is the share file from the assembly that diverged.  I ran this same study with an ambient of 26C, and the study converged.  I then changed only the ambient temp to 75C, and it diverged.  I checked to ensure that intelligent solution control was enabled, as instructed by the error box I found when I came in this morning.  Any idea what I can do to resolve this?  Please note that this study is to simulate a condition of an enclosure sitting on a table.  I used the recommended air volume sizing for that scenario as instructed by your web site.

 

 

John T.

 

 

Message 7 of 18
Jon.Wilde
in reply to: JohnTomasik6493

Hi John,

 

I would say that any innaccuracy is likely down to model setup here.

If the unit is on a table, we should not be using the 'chimney' approach (top and bottom both open) where the unit needs to be a good distance from the bottom. We should be using the 'bucket' approach. Where only the top is open with a P=0 and also a film coefficient (as per the guide here).

Model the bench thickness in CAD and also the air domain, the size you have it but sitting on the bench. The unit should also be on the bench and not floating a little.

 

Let's see what the flow regime looks like on a cut-plane first. Looking at the flow and whether it is seperate to the lines of the elements is the first check we can make to understand if we have sufficient mesh - if the flow look jagged, we know we need more mesh (and that will bring increased accuracy).

The key to accuracy is now not domain sizing (as it is nearly OK) but meshing, the results should all be the same as you increase the domain size but you need a very good mesh to ensure they are accurate. I often run mesh sensitivity sutdies. Refining the mesh to 0.7 and seeing if the results change. If they change by more than 5%, I know that my results are not yet independent of the mesh sizing and that I should refine futher.

 

When I'm in the setup mode, and I've autosized the mesh, do I assume that each teal dot is a node of the mesh?

Yes, exactly that. 

 

I hope that helps.

 

Kind regards,

Jon

Message 8 of 18
JohnTomasik6493
in reply to: Jon.Wilde

Jon,

 

The first set of boards (development boards) and their associated studies were held in a vice, elevated off a table.  So, they were more of the chimney effect, which is what we were first discussing (where you said my air volume was too small).  When I went to the desktop assembly, I modified my simulation model to reflect the bench mounted scenario, as suggested on your site.  That's just for clarification.  Noted about using the film coefficient.  I'll modify the model to use that.

 

Much thanks about the meshing input.  I'll be sure to look at that from here on out.

 

 

John T.

Message 9 of 18

I have a somewhat unrelated question, but I didn't want to start a new thread for this relatively small item.  I want to present some key IC chip temps to my client from an electronics thermal study that has far more IC's than I want to discuss.  I started using the decision center to pick parts and include them in a summary.  When I went to the decision center, I couldn't select any radio buttons or retrieve an values for those chips.  The documentation I've looked at online mention critical values.  I tried figuring out where to enter these numbers, but I ran out of time.  Where would I enter those values?  Are no selections available in the decision center because I don't have critical values assigned?

Message 10 of 18
Jon.Wilde
in reply to: JohnTomasik6493

Hi John,

 

You should be able to do this post run. Try going to 'Part' within results and selecting just one chip. Then tick the small box.

Then within the Decision Centre you should be able to see the part. You will need to right click it to update values (CFD will grab the value from each design/scenario) and then you should have the temps listed. Does that work?

From there, where to type in the critical value should be straightforward as it's on the same page.

 

Kind regards,

Jon

Message 11 of 18
JohnTomasik6493
in reply to: Jon.Wilde

Here's my first pass at a table-mounted device.  It seems like there's a bit much heat, and that not much is being transferred to the case and environment.  I know it didn't converge yet, but it seems like the temp isn't changing much.  Any improvements that suggest?  The temp seems a bit high, and I expected more transfer to the external environment.  Or, does this look correct?

 

 

 

 

Message 12 of 18
Jon.Wilde
in reply to: JohnTomasik6493

Hi John,

 

I would model a thickness for the table and draw the air volume in CAD - then you don't have the small gap beneath.

What temps are you seeing? It might be the case that you need to consider radiative heat transfer also.

 

Regards,

Jon

Message 13 of 18
JohnTomasik6493
in reply to: Jon.Wilde

Jon,

 

I need to pick a path and stay with it, since I must provide a summary of three different analysis (one with no heat conducting on the three primary heat generating chips, one with simple heat sinks, and one with some form of heat conductor to the enclosure) by Tuesday of next week, and each analysis has required a run time of about 8-10 hours.   So, I have 4 opportunities between now and Monday to create 3 good analysis.  That doesn't leave me much time for mistakes or changes to my approach, since I must maintain the same approach so we can get a valid comparison between the analysis.

 

That said, since this is table mounted, I can either continue with this approach, or if I put a low-conduction table in the analysis, will it interfere with the heat load placed at the bottom of the air volume?  With this approach, you seem concerned about the small gap at the bottom of the air volume.  I'm not sure how well I can match it to the bottom of the enclosure.  Any hints what I should be looking for?

 

 

For a 22C ambient, I'm getting peak temps of around 203C, with board temps of about 180C.  It's not totally unrealistic, since I ran the boards from this assembly independently before, and non-enclosed while suspended in air, and my peak temps were between 102C and 130C, depending on which board was being analyzed.  The client wants to know what their temps would be in a 75C environment, and my peak temp for that analysis is 307C.  So, an increase of 53C in the environment translated to an increase of 100C on the board.  Does that seem right?

 

 

Maybe I need to get tech support one-on-one, due to my time constraints and the amount of work involved?

 

 

 

John T.

Message 14 of 18
Jon.Wilde
in reply to: JohnTomasik6493

Hi John,

 

You do have full support with us and so logging a case might be a good idea, are you able to do this yet?

 

For a table mounted model I would always model the table. To match it to the enclosure, draw it in CAD, do not use the CFD external volume as this cannot touch the model by design.

With a greater than 70-80C temp differential (ambient to max) we likely need to run with radiation, which (as a very rough guide) might reduce the temps by 20%. You can run radiation later though.

 

Typically a 53C rise externally would equate to a 53C rise internally, apart from any smaller buoyancy effects.

 

Kind regards,

Jon

 

 

Message 15 of 18
JohnTomasik6493
in reply to: Jon.Wilde

Been having a heckuva time finding the support page.  I tried the links your team provided on the sticky of this board, but they're taking me to pages that no longer exist.  I've written an email to your support group (I found an old email with them) requesting a link to where I can log this support request.

 

Ok, I'll model the table.  However, once I do, there's basically no going back, since I won't have time to run additional analysis.  I'll post the cfz for that analysis before I run it (since it'll have to run tonight) so you can see what I've done.  I was hoping to avoid having to create the air volume in my CAD sofware, as that creation in your software was one of the selling points of our purchasing it.  So much for that benefit...lol.

 

I would've thought we'd see a direct correlation between ambient and analyzed temps, but that isn't what's happening.  If radiation drops numbers by 20%, we're still not a 1:1 correlation.

 

I'm not familiar with radiation analysis using your software, so I'll read up on that.

Message 16 of 18
Jon.Wilde
in reply to: JohnTomasik6493

John,

 

Here is the link to it. I can always log you a case though, then we can share the model and work on it through there. To be honest though, I know you have an active subscription with us so am treating this thread with the same priority.

 

When you create the air in CAD (it looks like you use Inventor?) you can simply overlap the block with everything and let CFD to the rest of the work for you, so it should be pretty straightforward.

 

Using radiation is pretty simple, the only things to bear in mind are:

  1. Ensure all materials have the correct emissivity values
  2. Keep an eye on your mesh count. I tend to aim for under 2million, it is a processor intensive calculation.

If we log you a case, we can always discuss this on the phone - I have just done so and will email you from it shortly. Then we can chat if it helps, I am based in the UK so only here for another 30 mins but can always send this to a US colleague.

 

Kind regards,

Jon

Message 17 of 18
JohnTomasik6493
in reply to: Jon.Wilde

Jon,

 

Sent you a reply via email to the case notification email you provided.  I gave you my phone number to pass along to a local tech support (in my timezone).  After briefly looking at radiation techniques, it seems that between both the thermal analysis and the radiation analysis, I won't have enough time to provide the answer to the client, so I'd like to talk to your tech support person on what approach can be used without me killing the schedule.  If you didn't get that email, please check your junk/spam email box.

 

 

John

Message 18 of 18
JohnTomasik6493
in reply to: Jon.Wilde

Jon,

 

I got the software to provide chip temps for selected parts in the decision center only once.  I re-ran the study last night, and the decision center would not recognize the new values.  I removed all parts, then added them again.  Now, the temperature data will not appear in the critical values tab of the output bar, even after I right-clicked and updated them.

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

Post to forums  

Autodesk Design & Make Report