I am using CFD 2013 to model a small chamber into which I pump one fluid (liquid) to displace the previous (also liquid). My flow is very slow, laminar, and the exhaust port is open to ambient pressure. All fluids will be liquid throughout the analysis, no chance of phase change at all. The chamber I'm filling is 15.5in^3, I'm applying a 0.1gpm flow rate boundary condition to fill this chamber, meaning it should fill in less than 45 seconds. However, when I run the analysis for 45 seconds in 1 second intervals, the volume is only about 5% full with the new fluid.
My BCs are:
Inlet: volume flow rate
Inlet: scalar = 1
Outlet: pressure = 0 gage (ambient)
My ICs are:
Whole volume: scalar = 0
I'm not interested in temperatures or heat transfer, but I've been recommended to turn on heat trans anyway so I can apply gravity effects (not sure why I cannot do this with regular flow analysis?). I've applied a manual mesh. No motion.
Flow: laminar, incompressible
My solver is setup according to:
Transient, time step of 1second, total time of 45seconds, saving results every 1 second
Advection method 2 (for scalar transport)
I have tried:
- Changing the diffusivity constant from 0 to a nonzero estimate
- Turning heat transfer off
- Setting the manual solution control for the Scalar to 0.5, instead of 1. All others are left alone
- Changing my fluid material to one of the default Autodesk materials
- Reapplying my BCs
- Reapplying ICs
- Reapplying all material properties
- Changing all my input to the default units (based on colleague recommendation)
- Changing my volume flow rate BC to a velocity BC (based on colleague recommendation)
Thus far none of these have worked. This is not a complex part, but my fluid seems to be at least an order of magnitude slower than it should be.
Has anyone else run into this problem? What can I do to troubleshoot this problem? Also, I'm not using the cloud version, so I cannot try many changes without spending lots of time.
Also on my list of observed bugs/errors:
- Material properties and boundary conditions sometimes not saved to setup card, despite updating values. Have to restart program
- Solver "hangs up" so that I cannot "Solve" or "Stop", and I have to reimport my model and start over from scratch
- Setup card (correctly) shows BCs that do not appear in the Design Study Bar
What is the criteria used to judge that the model is 5% filled with the new fluid?
Unless the two materials are the same properties, I think that you need to set up your own material which varies its density and viscosity according to the scalar value.
That is exactly what I did. I could look up the current scalar percentage in the analysis output. As well as it was quite easy to visually inspect the results.
As far as I know, I don't think there are any problems with what you have described. I examined with my own model but with the same BC and IC and got expected results, even when using constant density/viscosity, no diffusivity, with/without heat transfer.
Perhaps you might want to share your cfz file so others can take a look?
Thank you for the suggestion, but it is against my company policy to share files.
However, I may have reduced the overall problem to a simpler one:
The inlet tubing to my chamber is roughly 10.25 inches long. At an inlet flow rate of 0.1gpm, I expect this volume should be displaced in approx. 1 second. I know there will be some friction losses because I've got three 90degree bends and one 60 degree bend, but currently my simulation shows this volume displaced by the scalar in about 10 seconds. This is where my confusion lies. I do not expect the results to differ by an order of magnitude.
Another question I have is: because I've suppressed the exterior material, is it correct to apply the surface roughness of the exterior material to the fluid I'm using in my volume? In other words: I modified the fluid surface roughness from 0 (initial) to that of the exterior material. The CFD help is fairly sparse, in my opinion, on how the program uses the surface roughness. Is this the correct way to model the walls?
I forgot to mention: the other parameter I'm uncomfortable with is the diffusion coefficient for the scalar. The fluids I'm modeling are liquid water and liquid silicone oil. I'm not familiar enough with physical chemistry to know if I should be using a nonzero number here or just zero since these fluids are generally considered immiscible.
Ok. I finally found the answer to my question in the Help files concerning the surface roughness, so that is no longer an issue.
However, I am still stumped as to the slow filling. I've been told by a colleague that sometimes CFD handles a velocity BC instead of the equivalent volume flow BC. I suppose I could try that next, but I'm not sure if it would work. Confirm?
I don't know the details of the computation, but I'm pretty sure that both BCs should give you roughly the same results, provided that the input is physically the same.
How about this simplification:
I just created a simple model of a straight section of pipe (fluid) based on the scenario I described above. It has radius 0.109375 inch and is 10.25 inch long. At 0.1gpm, the fluid should be displaced in just over 1 second. I still have the BCs:
Inlet: flow rate = 0.1 gpm steady state, scalar = 1
Outlet: pressure = 0psi gauge
IC: scalar = 0
Even in this simple scenario, it takes approx. 10 seconds for the scalar to reach 0.99 (99% filled with the new fluid). I do not believe this. Even with friction losses, this should not be happening. Does this mean my problem must be elsewhere, such as the material properties?
Edit: My solving parameters are:
Transient, 0.2s step size x 50 steps = 10 seconds, 5 inner iterations
Laminar, incompressible, heat trans is ON, but only to turn on gravity, which is acting against the flow. Still not enough to make an enormous impact on the displacement time as mentioned above.
Here is my take on your simulation. I don't think it would be easy to get 99% scalar in the expected time due to the no slip condition of the wall. Regardless, I managed to get more than 90% scalar filled in the expected time of 1 sec. Try running it to see if you get the same results.
I appreciate your feedback, Ilyas! I agree with you, actually, but I don't think it should be 10 seconds.
Fortunately, I think I may have fixed my problem: I have the intelligent control feature disabled and I had lowered the manual control sliders for both pressure and scalar down 75% or so (I cannot recall the exact values). Bumping these sliders back to their default positions resulted in much more reasonable values (< 2 seconds to fill tube). I think I'm in much better shape now that I understand those controls a little bit better. I do not think this model has the need for changing control parameters, because I don't expect things to go "screwy" due to extra-fast flow, wild geometry, various heat inputs. Because it's so simple, I suppose I should just opt to leave those settings the way they're defaulted to.