Sim CFD 2014:
I'm trying to set up a velocity boundary condition with fully developed flow at the entrance to a round pipe full of air created using void fill tool. I'm told my surface is an invalid shape.
What could I be doing wrong?
Solved! Go to Solution.
Probably the accuracy of the CAD package? I have faced similar problems with no apparent reason. Sometimes remodelling and reimporting to SimCFD helps. Otherwise, you have to model the necessarily long inlet for fully developed flow.
The model was direct from inventor 2010: Sketched circle, extruded then shelled and sent to Sim CFD using Inventor add-in button.
If I have to use the workaround, how long is 'necessarily long' ?
Sure, I understood it was a direct import from Inventor, but I have seen such incosistencies happening occaisionally. A conjecture would be that the insuficient accuracy (or precision) of Inventor CAD definition is causing this. Perhaps Autodesk personnel can add more on this. Btw, why model a shell, why not just model the flow domain inside?
As for the workaround, the development length for fully developed flow (for a circular pipe) is well documented:
Turbulent flow: L/D = 4.4 Re^(1/6)
Laminar flow: L/D = 0.06 Re
That said, of course the best measure of a developed flow is the one that has no velocity gradients in the flow direction, ie, velocity in streamwise direction along any line parallel to axis should be constant.
Well this was just an experimental simulation in preparation for something more complex using existing CAD models. Are there any advantages on the CFD side of things to starting with a flow domain cad model over viod filling a hollow cad model?
Thanks for developed length info.
Often the 3D models used for creating drawings are very detailed and have many small components/features that may not be too influential on the flow field. Moreover, if there are any gaps, you will have to do a lot of cleanup before you begin meshing. Hence I typically model the domain separately, omitting the unnecessary details.
The other advantage I see is that you can easily decompose/slice the geometry to have separate parts in the critical areas of high gradients where you can use a fine mesh. You can use "regions" feature in SimCFD for this, but I don't think it is robust and recently discovered a bug in it as well.
Filling the void may be very useful in cases like castings. But even there, I tend to use Inventor (Delete faces > Sculpt/Stictch etc) to extract the domain, and then decompose it wherever necessary to have a better mesh distribution.
That said, of course, every engineer has their own style. I was talking about my personal preference
From the sounds of it you generated the solid pipe in Inventor and then (i would imagine) used the Geometry Tools within CFD to create the interior fluid?
There are some instances where I've seen that the Surface generated by the Geomtetry Tools does prevent the Fully Developed condition from being applied.
You may want to try cad'ing a 'cap" to seal the geometry (as this is your test case and you could do this feasibly for your real model) and then assign the Fully Developed condition to the external face of the cap (which would be assigned as part of the fluid domain).
'From the sounds of it you generated the solid pipe in Inventor and then (i would imagine) used the Geometry Tools within CFD to create the interior fluid?'
Thanks for the work-around.