My company manufactures dust collectors which periodically use compressed air pulses through a nozzle to clean the filter media.
Some additional details about what a pulse entails is listed below:
- A pulse duration is 100 ms.
- Each pulse releases 1.7 ft^3 of air. (This works to a mass flow of 1020 ft^3/min over the 100 ms)
- The pulse is activated by a solenoid valve which triggers flow from a compressed air manifold (90 PSI) into the valve.
As a CFD simulation I currently have a valve sitting in a rectangular duct (see attached screen shot). I am using compressible air as the fluid (as shown in the internal compressible flow example), and I will be using a transient boundary condition, but I'm not sure exactly what boundary conditions to use, or how to model the compressed air. Are there any tips on the best modeling and boundary conditions for this application?
There are a few things to mention here:
- You may as well suppress everything except the air from the mesh
- Compressible analyses are not simple - we need to be sure to define as much as possible at the inlet. A mass flow rate is perfect (as it is a constant) but could you assign a Total Temperature also? Take a look in the help for this, there is an equation to calculate it, which will be easy as you know the cross sectional area and velocity
- The opposite end might be OK with a p=0, I presume the flow is not compressible by this point? Be sure to have the outlet face far enough away from the nozzle so that you have no recircualtion over it, ideally all flow over a BC should be in one direction only.
- Run is steady state to start with, just to check that it does mesh and run OK
- Have you considered running a 2D axisymmetric analysis? This seems like the perfect model for it. The reasons for this are the reduced model size, yet you can have more elements, giving higher accuracy but still have a lower runtime
I think those points should give you a good starting point, please let me know how you get on. Feel free to share a support file (.cfz) once you have applied all this and we can take a further look if needed.
Thanks for the tips!
I am still having some troubles with this however, as I have tried many variations of boundary conditions and I typically end up with diverging results, especially if I let it run for 200 iterations or more. I have been sticking to steady state so far. In regards to axisymmetric...I like the idea of performing the analysis this way, however the end goal of this project is to study how the pulse will move around various shapes that are in the path of the blast. Some of these shapes will not really fit into an axisymmetric analysis so I'm hoping to maintain the full model if my computer can manage (it's been OK so far). I have not done anything in terms of refining the auto mesh at this point.
I have attached my most recent analysis .cfz. Let me know if you need any other additional information. This is my first attempt at using CFDesign so please bear with me!
This has been escalated to a Support case with Product Support.
For others that might follow this, notes to keep in mind.
As a quick recap of the file posted:
There should not be internal boundary conditions (namely the Unknown that is in the model)
For compressible flow, the inlet will have to be properly constrained (depending on assumptions). As-is we are assuming a steady state flow so not a 'pulse' of air.
Meshing may need to be refined to preoperly capture the characteristics of the flow field.
Evolving this to include motion and the pulse of air moving the solid will require notably more mesh as the solid body motion will have its own meshing concerns to properly capture the masking.
Taking this as a 2D slice will be the best approach forward to get a handle on meshing requirements for all of the above and then applying those lessons to the 3D geometry.
Taking a leaf from this thread, I am currently doing a similar simulation. I have posted a thread earlier, but I repost the same here, since it is kind of in alignment with this subject.
I am trying to simulate an automobile silencer (muffler) which contains an assymbly of concerntric cylinders with inlet and outlet. Inner cylinder is perforated so represented with surface resistance with adequate resistance coefficient. The inlet is transient mass flow, represented by piecewise linear function, such that at every ulternate interval of time, the flow is on and off, thus realising a periodic step function.
Is it fair to say that is recommended to do a sensetivity study for timestep for transient analysis? As of now, I select a timestep that is typically 50 times smaller than the period of mass flow cycle. And I keep decreasing the timestep till I see that for every timestep, the last portion of plots of inner loops is flat, indicating that every timestep is converged. This should ensure adequate temporal accuracy.
I was wondering if this approach was right, to assess the adequacy of timestep, or are there better measures?
Sorry for the delayed response on your post here.
yes I would say that the path you are mentioning is appropriate if you wanted to do a Timestep size sensitivity study.
Accurately representing the input condition is one consideration, the other would be to ensure we have a small enough timestep to capture the flow through any other interesting passages (choke points/etc)
As you start getting in to a small enough timestep you may find that some iterations we only use 3 inner iterations (with the rest flat/steady) and others we might need 5-10.
One item taht can help save inner iteration calculations is the flag AutomaticInnerIteration. This flag will allow you to set a percentage change between inner iterations, such that when it is reached we will skip to the next global timestep
So in the example above, when we only need 3 inner iterations it will then jump to the next timestep, but for steps that we need more, it will allow to go up to the value set in the Solve Dialog
Typical value used here is 5 (as in 5%)