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.

[Anonymous]

What are you trying to solve for? Air-side pressure drop? Heat transfer?

You will want to take advantage of any geometric and flow symmetries to reduce your overall model size. 

[Jon.Wilde]

Consider resistances also, might be useful here 🙂

[Anonymous]

Yeah?  And?  Nobody's done this with the software?  I'll be looking at pressure drop and heat dissipation.  Since the condenser configurations vary dramatically, symmetry is limited and and I'm not sure at what point I'd be over-simplifying the model.

[Anonymous]

Users have solved models with tube-fin heat exchangers before, but each application may have unique assumptions or boundary conditions. To determine at which point you are over-simplifying depends on the degree of accuracy you're aiming for and whether you want an upper bound or lower bound estimate.

Although you haven't stated it, I'm assuming you're trying to determine the total heat rejection capacity of the condenser coil and the static pressure requirement of the blower/fan. I'm also assuming that you do not know your heat rejection rate as a function of face velocity (something which is sometimes provided by coil manufacturers).

You could start by isolating the most basic repeated geometry for a single heat exchanger (depends on whether or not tubes are staggered and if the fins have any rifling/enhancement geometry) and modelling that with appropriate symmetry conditions to give nominal values for pressure drop and heat flux. Develop a resistance curve by varying the face velocity. As for the heat flux, multiply it through to get an estimate of the value per each coil.

To run your full model, substitute each coil with a rectangular prism with appropriate bounding dimensions. Assign the "Heat Exchanger" material type to each coil and assign the air pressure loss information you obtained from the smaller model. Also, assign the total heat rejection rate as estimated from the smaller model.

There's many ways to solve this problem and I've only outlined one. You may choose to pursue it differently based on the assumptions you're willing to make. 

[Anonymous]

In my post previous to yours, I stated I'm looking at pressure drop and heat dissipation.  

What do you mean by representing the fins as a rectangular prism?  One "part"?  Any examples?

[Anonymous]

One other question.  I started modeling this, and realized that the thermal energy carried within the condensor tube should be carried outside of the modeling environment, except for the thermal energy that's conducted through the material into the condensor fins.  Correct?  If so, would the "Tutorial: Electronics" be an example of how to set up my model?

[Anonymous]

So my approach is two-fold.  I want to see if a more geometry-accurate model makes much of a difference compared to a simplified model (I've attached a jpg).  I modeled a very small section of the heat exchanger and tried to mesh and analyze.  I was going to create a second simplified geometry model, and see if I could come up with some sort of feel for what's necessary and what isn't.

I haven't got there yet because it won't mesh.  My first issue is meshing.  The edge length of the thin fins seems to be causing issues with the surface mesher.  I'm in the process to get it to mesh, but since I'm time limited, I thought I'd post it here looking for assistance so I can expedite the solution.

Also, the "fluid" in the line only provides heat (I don't care about where it comes from or goes, since in the real world its source of temp/pressure/phase change is far away from this condenser.  So, should I just model it with a heat load on both ends?  Or, should I try to conduct it to an air volume outside of the heat exchanger region itself (you'll see what I did if you open the model).

The file size exceeds the upload max to this thread.  I haven't done this in awhile, so how do I upload a 16MB .cfz to your team?

[Jon.Wilde]

Hi John,

Might you be able to send it in reply to my email? I sent you one from the case you requested.

What is flowing around the fins, are you going to need to model that too or could you simplify with film coefficients?

It sounds like you are going to need to pump the fluid through the tube as well?

Thanks,

Jon

[Anonymous]

I tried the resistance material, but I can't get flow through it.  I messed around with the free area ratio numbers, and no matter what I do, nothing seems to flow through it.

The correct K value, per the help page that explains free area ratio and calculating K-value is 0.25.  I even messed around with the "Normal Direction 1K" and "Normal Direction 2K".  Still no flow the the resistance.  I'm going to refine the mesh and close the gaps on the side, but I'd like someone to look at this and see if there's something else I'm doing wrong.  I have an open case on this, but my email replies haven't been responded to.  I've attached the share file of my last pass.

A little help, please...

[Anonymous]

I've moved on to the next phase of this project.  I'm looking at a variety of condenser orientation configurations.  I'm trying to use my resistance material on a three-sided condenser.  I've attached the share file.  Unless I'm looking at it wrong, I don't see the software pulling air through the material.  Can someone confirm if I'm seeing that?  If so, any thoughts on what's wrong with my model?  The resistance material represents the condenser.  It's the part called "Sharp Corners".  There's a steel housing sealing it.  A fan is suspended within the air space in the housing.  In many condenser units such as this, there aren't baffles (which surprised me).  

[Jon.Wilde]

Hi John,

You may need to model this a little differently. We should avoid situations where flow can pass in two directions over a boundary condition - is it possible to do this here? Maybe have a cuboid of air on each resistance?

Remember that we need a good uniform mesh on all resistances and fans.

Advection Scheme 5 every time.

Here's a quick snapshot with just those changes, looks OK to me? Did you right click on the legend and tweak the scale? I think you will need to do this to show the lower velocities through the resistances.

I would definitely suggest moving up to CFD 2016 for this model too. Worth it for the changes made to the resistace modeller.

[Anonymous]

Jon,

In your model, did you include the cuboid of air over each resistance? Or, did you just refine the mesh on the resistances and fan, as well as set advection to advection 5?

If I need to have a cuboid over the resistance material, there really is only one resistance material, albeit in a U-shape.  If I need a cuboid of air over each leg of that U, how should I set those up, geometrically speaking?

Just a note: the client has since told me that they're primarily interested in only air flow. This allowed me to simplify the model (luckily). I only imposed thermal loads to help me spot any unforseen problems.

[Jon.Wilde]

Hi John,

I used the same model, only changing the mesh and advection scheme. The resistance just needs air on each entrance and outlet. 

Hope that helps,

Jon

[Anonymous]

Jon,

Attached is one of the two studies I've been working on.  Let me know if the mesh looks ok.  I seem to be getting good flow.  I didn't think the advection setting would matter since I didn't care about thermal transfer results.  That might've been an incorrect assumption.

Oh, quick other question...is there documentation that better explains how/where CFD generates and saves files?  I seem to be getting these sub-folders that I have conscously created, and they are a bit confusing at times.  

[Jon.Wilde]

Yup, always use ADV5 with volumetric resistances.

Our help has details on the folder structure.

I am still a little concerned about all of the external pressures giving you an unrealsitic solution - they are all pretty close to the model also.

[Anonymous]

Jon,

Thanks for the info.  I am reviewing my model compared to the volume strategies in the link below.  Note that this unit will sit outside, all sides exposed, mounted about 6" off of the ground.  

However, if you have insight or information why my external air volume should be different, I'd appreciate that, along with an explanation why.

http://help.autodesk.com/view/SCDSE/2016/ENU/?guid=GUID-E0609A21-541D-4D11-9663-93476E26CF8F

[Jon.Wilde]

Hi John,

We really need to try to avoid flow entering and exiting over a single boundary. The only time when we might is when we have the 'table mounted' option in the link you shared. It can hinder convergence and also leave us with an innaccurate energy balance (especially if we are running thermal as the flow re-entering has no reference temperature).

[Anonymous]

So I modeled the attached similar to the guidelines in the following link:

http://help.autodesk.com/view/SCDSE/2016/ENU/?guid=GUID-974D404E-9073-43D9-96FF-A3A4728F2B9D

I didn't apply zero pressure on the sides, hoping the air space was big enough to not get recirculation because the flow can't exit the air space.  It didn't work.  I've attached the cfz file and there's a picture attached showing the air recirculating.  If I allow the condenser to flow heat via its coolant, we'll be reintroducing the hot air through the condenser.

Do you have any suggestions so air doesn't recirculate?

John Tomasik

[Anonymous]

Jon,

I ran that same model with 0 pressure sides.  Attached is both a pic and the cfz file.  Let me know your thoughts.