I tried multiple settings and read almost all the tutorials, but I'm still not sure how accurate my simulation is. It's a fan to which a long motor is attached.
I made big Inlet and Outlet models and set the boundary conditions: pressure = 0 Pa.
RPM is 10000, but I'm not sure if the rotational speed table is correct I made. Could anyone check and give any advice?
I solved 100 steps, should it be more? I measured the velocity in z-axis, which is approx. -1.8 m/s, this seems to me to be little?
I attached the cfz file. Thanks everyone for any help and advice!
Solved! Go to Solution.
- Why the big inlet and outlet? Wouldn't keeping them the same diameter minimise recirculation over the boundary conditions? This will improve stability and also help with measuring the flow speeds produced by using the bulk calculator
- The Rotating Region (RR) should ramp up over the first 50 iterations. Use 3deg/timestep in the Solve window (5e-5s) and then just multiply this value by 50 within the material
- Suppress the impeller from the mesh but also add a good deal of refinement to the leading and trailing edges and then finally a uniform mesh to the outer surface of the RR
- You could make the RR fit the geometry a little better, so it would look more like a 'T' shape in section
- Run for 1000's of iterations, until the convergence is smooth and repeating and the torque is constant (Results -> Review -> Rotating Region Results)
I am in the middle of preparing a hangout session on just this subject for the 16th of July, keep an eye out on the forum for the invite.
First at all, thank you a lot for the fast answer!
To your 1. point:
I chose a bigger inlet and outlet because it was described in the following article:
"Extend the suction (inlet) and discharge (outlet) at least 3-4 hydraulic diameters from the impeller. This is necessary to prevent the boundary conditions from directly influencing the results."
But I changed the geometry as you said.
To your 2. point:
Thank you very much for the speed table. As you maybe noticed I used (or at least tried) the 3 phase strategy, also explained in the link above. But there are still many incomprehensibilities in their explanation. Could you please explain in your hangout session how such a table is designed. For example why are 50 steps needed for the ramp-up? Is it program specific? Also would be nice if you could explain the relation between time-steps and number of iterations.
To your 3. point:
Did it exactly as you said. Thanks! But a tutorial about how to apply a good mesh would be nice (for different geometries and scenarios). I hope I did it as you have been meaning it.
To your 4. point:
I did as you said, but after reading in the model with the T-shape RR, CFD divided the impeller and the motor in two parts, also the RR "Impeller-part" and the RR "Motor-part". So i just applied to both RR the same RR specifications, but then the solver exited unexepectedly. So I just deleted the Motor part. Now it's working fine.
To your 5. point:
In the attached file I iterated 100 times, just as a first try. Will let compute it now longer.
Thanks againg, I'm looking forward to seeing your hangout session.
No problem at all, when I can I like to help as much as possible. I think sometimes coffee helps me work a little faster
1) I understand what you mean about the inlet and outlet now - it actually means extend the length along the axis and not the radius. So the outlet here needs to be much longer, 10x it's diameter in length
2) 50 steps are just what we use from experience, I am sure that other values would work but it is good to have just one message.
There is not such a great relationship between timesteps and number of iterations. Only really that with a transient simulation, you would typically need more iterations the smaller the timestep to reach the same 'real-time' value.
The actual number of timesteps we run for is not important, what is, is that we run enough to achive a stable solution.
The torque output and also monitor points help to quantify this.
3) The issue here is that your blades are a single surface. Ideally the leading and trailing edges are separate so you can give them an extra refined uniform mesh, much like this from a different model:
It is hard to know when we have an optimum mesh without a mesh sensitivity study. Really you need to clone the scenario, refine the mesh futher (say to 0.7) and compare the results. If they are different (by more than 5%), then the change in mesh had a significant impact, so refine and try again.
4) Really the RR should split the gap between the turbine and the wall, not be the wall. I would reduce it's diameter so that it sits halfway between impeller and wall of the tube. This should help, although I would also ask - is there really a wall in existence? Maybe there is for testing?
5) Great, it will surely need to run a long while.