8 Replies Latest reply on Mar 9, 2015 10:19 PM by Jared Conway

    Ceiling fan simluation questions

    Logan Vaught


      I want to first apologize if these questions have been asked before but I didnt see any when browsing.  This is for a senior engineering design class where our group is tasked with designing fan blades for a company that are efficient.  What I am trying to do is recreate the Energy Star test for ceiling fans in Solidworks(picture included of test below).  I have a model of a known fan from the company I am working with, but I have a few questions on how to set this up more correctly than I have.  I have a basic understanding of how to do these simulations and have run a few, but my simulations seem off.  I have been reading a ton into this but I would like to get some insight from you all and see what is possible, necessary, or what I may be missing.



      Test so far -

      I have based my testing method is based on a series of youtube videos showing a fan simulation in an enclosure. (https://www.youtube.com/watch?v=xvZgyJ2V-bE)  This is the first of the videos for this simulation.  However my set up with the fan, cylinder, and enclosure are different(like a fan rotating about the y axis vs his on the x) but the concepts remain the same.




      So far the flow rate is low compared to the listed values and drops off entirely at lower rpm.  The fan is listed at 5400CFM at 178 rpm but I get closer to 4000CFM.  For the project I wouldnt need to get exactly 5400 for a fan like this, but it would be nice to have a closer value therefore we can be a little more sure our designed fans are performing as expected. 




      Simulation Questions

      1. Meshing – What settings are most important for this?  I have been using simple settings at first for faster calculation just to figure out how to get things running and then will crank up the refinement, if needed, when I run my final simulations.
      2. Goals – Surface of each bit of the fan blades or volume goal based on rotating domain cylinder
      3. Set-up – Is this possible or accurate?  Internal or external?  What separate settings
      4. Boundary conditions – When using the enclosure I have them set at the standard atm pres
      5. With my cylinder that is set up like the physical test, do I need to define anything associated with it like a boundary layer or separate fluid domain?  Ive  seen that this type of external/internal stuff can be difficult so any suggestions as to recreate this test or make something similar would be very appreciated.
      6. Calculation options - Any specific settings to change to my analysis goes long enough to measure steady state flow or at least the airflow after it has been going for a minute or two?


      Any other advice would be greatly appreciated. 

        • Re: Ceiling fan simluation questions
          Bill McEachern

          1) The domain doesn't look big enough. Make it the same size as the actual test room or much bigger than you have if it is not known

          2) you need to realize that he descretization method in flow sim puts flat facets to approximate the geometry of he blades - you will need a fine mesh to get a good approximation to the surface.'

          3) you likely want to have 3-5 cells or more between the fan tip and the edge of the rotating region - you might have to explore this a bit.

            • Re: Ceiling fan simluation questions
              Logan Vaught

              Thanks for the quick response. 

              1 - That makes sense and was easy to change.

              2/3 - So youre saying my initial mesh needs some tweaking along the blades so it actually knows where the fan blades are touching the fluid?  Is it possible to refine them along the flat parts of the blades and how would I go about that?  Just go into local mesh and crank it up or is there an easy way to see the local mesh along the blades and refine it from there?

                • Re: Ceiling fan simluation questions
                  Amit Katz


                  What I typically do when refining a mesh is start with the basic mesh. Put your control planes where you want and tweak the basic cell size. That will tell you how many levels of refinement you need in your local mesh to accurately capture the geometry.


                  The next step would be to mesh your model and use cut plots to see the real mesh. BE SURE you turn off "use CAD geometry" in the cut plot options, otherwise the program will cheat and will show you what you want to see, instead of the real mesh.


                  Now you can see if your mesh is fine enough. If not, then it's time to iterate and either increase the refinement level or shrink your basic mesh cell size.


                  One more thing: Before you start getting crazy with the mesh refinement, do some simulations with your more coarse mesh sizes so you can compare your results and see how well they converge as you shrink the mesh. This is what the "clone project" command is good for.

                  • Re: Ceiling fan simluation questions
                    Bill McEachern

                    On blade mesh refinement: I find the curvature control to be pretty effective but be careful a small change can dramatically affect cell counts. Things will blow up if you just drag it to a very small angle.

                • Re: Ceiling fan simluation questions
                  Vikram Manthri

                  Yes, I do agree with Bill. Use narrow channel refinement. Specify the minimum cell size manually. Or else you local refinement. That would definitely improve the results. 

                    • Re: Ceiling fan simluation questions
                      Jared Conway
                      1. Meshing – check the tutorial on mesh refinement and also the solving engineering problems document on meshing for rotating regions. in the long run, start with a mesh and then refine it.
                      2. Goals – fan blades doesn't really make sense. flow rate at the top of the cylinder seems ok. what gets measured and how in the real world?
                      3. Set-up – if it is tested in a room, internal makes sense to me. it should match physical if you are trying to match the results exactly. something to consider, what are the assumptions that you are making and what do you think the effects will be. 5400 is physical, 4000 seems not bad to start.
                      4. Boundary conditions – what boundary conditions?
                      5. Not sure what you are talking about here. set to turbulent. don't touch the parameters if you don't have specific info.
                      6. Calculation options - not something you have to worry about here, the results will converge. just don't let it stop early. ie let the goals converge.
                        • Re: Ceiling fan simluation questions
                          Logan Vaught

                          Sorry for the super late reply, been a busy semester but I really appreciate the help.

                          I changed how my goals were set up so now I'm measuring mass flow, velocity, and volume flow rate through the cylinder.  Also measuring the force on the blades as Im assuming thats the drag force unless they calculate something else.  In the real test the measure the airspeed about an inch from the bottom of the cylinder and multiply that by a specific area that the sensor covers.  So I have a surface that I suppress to measure the flow rate and bulk velocity at the bottom of the cylinder to mimic the test.  It generally gets to 300-400 iterations before finishing if I have about 150k fluid cells.


                          As far as the mesh goes I have been adding planes in the initial mesh around the area of interest and adding a local mesh around my blades. I have also made the set up completely match the 20x20x11 foot room they test it in.


                          For the boundary conditions I have the inner walls set as environmental pressure, as the youtube tutorial suggested.


                          Im still left with a few questions though.

                          1. is 150,000 fluid cells still low for a study of a 54 inch diameter fan with flow through a 36 inch tall cylinder?  I could increase it but 250k but any more seems to take 4+ hours and Id like to avoid that.  Mostly because the remote desktop to my school seems to boot me out before then.


                          2.  Using the bulk average velocity and the area of the surface that I get the data from, I get a different volumetric flow rate than the program and Im not sure why.  Taking the bulk average multiplied by the surface area I get around 5800 CFM from multiple runs, which is close to the target of 5450.  However I get maybe 1000 less if I use their value of the flow rate, which doesnt make sense to me.  I would assume they would use the given area and either the average or bulk velocity but it always seems to be low.


                          Also, if I were to test other fans would I assume this same percentage error, or would I just want to assume that my results might be maybe 400 CFM higher than the real world?

                            • Re: Ceiling fan simluation questions
                              Jared Conway

                              is 150k cells enough? only running with different level mesh will tell you that. but that seems low for a rotating region problem.


                              "their value of flow rate" > what do you mean here? the software is integrating over the area. you may want to take a look at what bulk average is defined as.


                              same percentage error > I think that is a reasonable assumption but well worth testing. 2 data points is better than 1