at first I want to excuse my english-I'm from Germany :-)
I have great problems with the boundary conditions. If I only assign one inlet the flow seems to be plausible but does not go through the whole model - understandably.
But If I assign a p=0 area at the outlet, the velocity goes to extreme values.
And if I assign a volume flow to simulate the outlet the program defines it as a second inlet.
Actually I just want to simulate the following:
I want to assign the inlet conditions with the values: volume flow=20 l/min, p=8 bar and the wheel rotates with 48 rpm
And I want to get the values velocity and pressure at the outlet respectively in the model.
I hope you can help me because I am using this simulation for university and my grade depends on it ;-)
If the velocity values are very different from your expectations, it is likely that the CFD geometry units do not match your CAD units ("m" instead of "mm" or "ft" for example). I have made this mistake as well and had velocity faster than the speed of sound!
You will need to "edit" your geometry units to convert them to match your geometry. You will need to do this before you apply mesh settings, or you will need to delete the mesh settings before you can apply the changes.
A few pointers here
- Extend the inlet 3x and the outlet 5x
- Be aware that if you have a velocity/flow rate at the inlet, you cannot also assign a pressure at the inlet and outlet, you must leave something to calculate. How about 8bar at the inlet and 20 l/min at the outlet, then CFD will calculate the pressure at the outlet
- You are probably better off not using strict motion here but utilising a rotating region (RR) (in materials), you will need to add an additional cylinder in CAD, splitting the distance between the impellers and the wall - this is what you assign the RR material to and can then suppress the solid parts from the mesh
- Ramp the RR up over 50 iterations
- Ramp the BC's up over 100 iterations
- Each iteration intially should be blade to blade (360/8 = 45deg), you will need to base this off the rpm
- Run with Intelligent Solution Control (ISC) on (Solve -> Solution Control)
- In the same window, switch to Advection Scheme 5 - better for RR analyses
Hopefully that lot helps!
those are some really good pointers. The point with the rotating region I have already found myself and it works better now.
The only thing I don't understand ist what you mean with "Ramp up" and "BC's" - maybe a language problem
I will definitely try the other advices. And yes, the diameter ist 80 mm.
Tank you very much, I hope it woks out :-)
One more question- Why should each iteration be blade to blade? This way I can't see the movement and so I can't see what happens when the wheel is in diffrent positions, but this would also be interesting.
Thanks for helping me!!!
OK, I didn't want to bomabard you with everything at once.
Once the blade to blade looks good - the convergence should be repeating.
Then switch to 3 deg/timestep for better convergence.
THEN when it is done you could save some intermediate results for an animation - overall we should avoid saving out more than 30-50 or so as the files can become very large.
By ramping up, I mean that we should not start the RR or BC's at full flow. Increase the RR speed to the max over 50 iterations and the BC's over 100, this helps convergence.
Many of these setup concepts are discussed in this guide: