Anyone model an A/C condenser coil?

[Anonymous]

Curious whether the software can handle high aspect ratios of the condenser fins?  There are 16 fins/inch, and with a 30 inch condenser, I'm looking at close to 480 fins.  Add to that we're playing around with multi-sided condenser configurations (e.g., 3 condensers at 90 degrees to each other, forming a U shape around a central fan).  I honestly can't get a feel for whether all of that detail is necessary to get a good flow analysis, so I'm posting here hoping others who have done this can share their experience.  My analysis time is very limited, so I was hoping the community can help short-cut my work so I can get to the answers we need.

[Jon.Wilde]

This looks OK, although I think you could do without the P=0's on the side walls - we call this the 'bucket' approach 🙂

[Anonymous]

It doesn't seem there's much flow recirculation, with no boundary condition on the sides.  

Next question (yes, one day this will end...lol):  Is there a way I can query total fluid volume flow rate on the face of a 3D part?  The wall calculator doesn't provide that info.  I want to know air volume flow rate on the three surfaces of the condenser shown in blue in the attached pic.

[Jon.Wilde]

Hi John,

No worries. Don't worry, I'm still with you on this 🙂

Have you tried the Summary File at all? That should give you the flow through each reistance, assuming those are all individual parts.

Not sure if we can just capture those faces. The ideal way to do this would be the bulk calculator, hiding the fluid volumes you are not interested in but this really needs a CAD change, so you can only have smaller sections of fluid displayed. This might work through the resistances but there is one more issue - we cannot have a curved cut plane through the central region.

Do you need to know how the flow is distributed between each? Could you calculate the outer two and subtract the flow to calculate the central one?

Thanks,

Jon

[Anonymous]

Jon,

When the summary file calculates the volumetric flow through a part (in this case the resistance material), does it calculate simply the scalar value?  Or, does it consider the effects of the vector (direction)?  In other words, and as an example, if you have a section experiencing flow in a negative direction of 10 in^3/s, and the rest of the flow is at 30 in^3/s, would the total flow volume reported be 20 in^3/s, or 40 in^3/s?

What also didn't make sense is I compared two summary file results of the flow through the condenser (resistance material), and the flow is higher in the study where the pressure drop was higher.  I would've expected the opposite.  The flow through the condenser in study #1 is 771 cfm with a delta P of .007 psi.  In study #2, the flow is 869 cfm with a delta P of 0.045psi.  The difference between the two studies is in study #1, the fan is closer to the exhaust port of the housing, and it appears there is less recirculation within the housing than in study #2.

Oh, the fan is movig 2400 CFM (the summary file confirms that).  Since there's recirculation, I'm assuming that the more recirculation we're seeing, the bigger disparity we see between flow through the condenser and the fan.  In the third study (see next paragraph), that unit is sealed, and should I expect that if there's next to no recirculation, we'll see flow through the condenser close to what's flowing through the fan?  

I'm re-running a third study that places the fan flush to the housing exhaust port.  It appears there's hardly any recirculation at all.  I don't have those results yet (the study is still running).

The client is looking for a volumetric flow rate so they know whether they're passing enough air through the condenser to phase change the freon within.  Any suggestions on how I can provide that number would be good.

[Jon.Wilde]

Hi John,

The summary file would predict 20 in this case.

If there is recirculation near the filter, I suspect CFD might struggle to give you meaningful results - although this should be far better in CFD 2016 as the methodology was pretty well reworked. Are you running this now?

Thanks,

Jon

[Anonymous]

Really?  Uh, recirculation in an application like this is commonplace.  No, I'm not running 2016 yet.  How much more accurate is it?  And, you didn't answer my questions.  Also, I tried logging a case, but in addition to the site telling me I have no authority to access my case account, tech support can't help either?  If tech support is really this unavailable, we're going to have to look elsewhere for our CFD solutions.  Tech support has really fallen off for this product.

[srhusain]

The filter model is a finite element idealization/approximation which presupposes that the flow within same is unidirectional. The alternative to using this model is to have a mesh that is fine enough to capture the geometry details of the actual filter, which can be prohibitive. IMO, an actual filter where the flow is recirculating should be avoided.

[Anonymous]

It's not a filter; it's a condenser.  Read the thread.  If I try modeling this with its actual geometry, it'd be prohibitive in analysis time.  So, you guys are saying you have no solution for this, correct?   Recirculation should be avoided?  Really?  So much for the real world...

[Jon.Wilde]

Hi John,

Syed's is one of our developers, I suspect he can be really helpful here once he fully understands the problem 🙂

If you are unable to log a case I can help. I suggest we do two things:

1. I see the case you have to get help logging cases - I am going to track this and have it escalated
2. Regarding the model, I think it might be sensible to get into more details. Perhaps through a call but let's see

You have 2400 cfm from the fan - is this a fixed flow rate like last time and with no leakage paths back out around the fan? It looks as though there might be a gap?

Typically an axial fan needs a shroud around the outside of it to prevent leakage, like your last model, which was set up perfectly.

I suspect that the values we get from the Summary File here might not be so useful as the curved resistance is going to be tough to calculate, but I feel that there must be a way. The bulk calculator might be more useful.

A couple of questions:

Is the goal to ensure good coverage of the coil?

And your main concern as I understand it is that CFD seems to be losing a large percentage of the air coming into the box somehow?

We really are here to help you but from my perspective at least, the model is developing pretty quickly and so I need to catch up with the design changes before being useful.

Might you be able to share your latest model?

Thanks,

Jon

[Anonymous]

Syed needs to read the thread accurately to understand the problem.

1.  I chatted with Autodesk yesterday via online chat, trying to explain the simple problem that logging in to my account on Autodesk, and following the prescribed paths of accessing tech support and open cases simply did not work.  When I tried to do so, the site told me I didn't have authorization to do so.  The individual I was chatting with seemed incapable of understanding this.  She opened a case that I couldn't access, then it was cloned to another case, which was closed without solution.  I tried contacting Autodesk both through the email as suggested by Autodesk, and also through their website.  Neither produced a response.  I'm curious...are you the last tech support person available for SimCFD?

2.  

     a.  The 2400cfm is a fixed flow.

     b.  In typical condenser A/C units, there is in reality leakage around the fan.  In the real world, many don't have shrouds, so within the device there will be leakage.  

     c.  In the two design configurations I'm testing, the fan is mounted about 4" off of the outlet port, and the other is with the fan flush to the outlet port.  Neither has a shroud in the real application, so this is the environment I must somehow replicate within the analysis.  Placing a shroud around the fan will not be real-world conditions.

     d.  What geometry do I need to create to use the bulk calculator so I can determine what the actuall flow volume is through the curved condenser in both design scenarios?

     e.  The goal is to understand air volume flow rate so we can understand whether the client is getting sufficient flow through the condenser to perform the phase change of the freon in an ambient temp of 90 degrees F.

     f.  I've performed multiple analysis while changing the resistances of the material representing the condenser coil.  I performed a baseline study to try to determine those resistances.  I used the formulas provided on your website to create the resistance values.  However, when I use those values, the baseline did not perform equivalent to the manufacturer's specifications.  I had to change the resistance value to duplicate what they claimed.

     g.  When I used those resistance values in a modified geometry of the condenser, the flow through the condenser significantly dropped off, and the pressure drop increased far beyond what the manufacturer claimed for their unit.  I thought this was a result of the modified geometry and recirculation, but since I'm being told that might not be accurate, I have no clue what I'm seeing.

     h.  With reduced recirculation, I'm seeing only 1/6th the flow through the condenser than I am through the fan.  That increased to that amount when I used the values I had to use to run the baseline study to determine the resistance values mentioned in step "f".

     i.  By hand calculations, your formulas for resistance material properties told me to use 0.25 as the resistance.  I did, and it did not produce what the manufacturer claimed.  I subjectively changed that until I got the proper thermal results of the baseline model...which required a resistance around 0.4~0.5.  

The latest study share file, stripped, is 12.4MB.  Here's the link to download:

https://www.hightail.com/download/ZWJYNnFPcTIzMWwzZU5Vag

[srhusain]

I think I understand the problem a bit more clearly.
Nevertheless, there are three things you need to be aware of in the context of using the resistance model to idealize the hydrodynamics of your condenser coil:
1) Backing out a resistance value with a given geometry and mesh will not yield the correct intrinsic value of the resistance that you can subsequently reuse in a different geometry and mesh.
2) You will need to re-characterize the resistance value of your model whenever you change the geometry and/or the mesh.
Like your effort in item (i), it is a trial and error process.
3) Mesh sensitivity studies to ensure mesh independent results is a critical part of your design goals.

[Anonymous]

Replying to your comments:

1)  Then if the calculated value does not replicate the manufacturer's data, given their boundary conditions, what is the software telling me?  Is the software inaccurate?  Is the manufacturer's data inaccurate?

2)  How can I re-characterize the resistance if I have no baseline?  How do I know what's correct in a new design, trying to use this software as a predictive tool?

3)  I'll run the mesh adaptation study to arrive at a mesh independent solution, although I'm not sure what value this will have given the information that the software can't handle multi-directional flow through a resistance material.

[Jon.Wilde]

Hi John,

Bypassing the resistance discussion for a moment, I am looking over this model and have some comments about the geometry.

Do we need to include the wire mesh on the inlet and oulet? I suspect they will play very little part in the result and they are not very mesh friendly. What would be better is to have the part overlap rather than meet at an infinitely small angle or with a tiny gap. Without them we might be able to significantly reduce the mesh size and speed up the run time.

With the refined mesh I am trying to apply, they are actually causing a meshing failure:

[Anonymous]

Jon, I'm running 2015 and it meshes fine.  Todd has me using a surface for my resistance material in place of the simplified condenser geometry (which is now air).  I went back to an old analysis I did to use a surface resistance in that study, and I noticed that the software is telling me:

"

*** Warning: DR shells detected. Use of Advection Scheme Adv5 may produce inaccurate results. Adv1 is recommended"

Should I switch to advection 1, as recommended?

[Jon.Wilde]

Yes, ADV 1 for surface resistances.

I wanted to test 2016 for you too, just incase the new resistance approach made a difference to the results.

In 2015 I am getting just over 20,000 cfm through the larger filter and for some reason I cannot measure the smaller planar one (I get a zero). I was going to measure these two and then subtract the difference from the 2400 to give the result for the curved resistance.

Todd's suggestion is good, if we use surfaces, we will still have the air blocks in place to measure the flow within, which ought to work better.

We can at least see the flow distribution really nicely:

Just a quick check, the fan is pulling air out of the box yes?

Thanks,

Jon

[Anonymous]

The fan pulls air through that condenser and blows it out of the top of the enclosure.