Erosion Model

[proudgrover47]

Hi there, I'm getting to grips with using traces and erosion however I seem to be encoutering a problem which I cannot find a remedy to. I am using a converging-diverging nozzle and then applying traces to them, however the traces stop at the choke point and dont go any further, could this be because of the size of the particles being too big to pass through the choke point? 

On another note, do you know if it is possible to put a material plate on the outside of the nozzle and see the erosion on it, see what I am trying to do is simulate an abrasive air jet erosion model. (like water jet but the fluid is air)

Thanks

Al

[OmkarJ]

It is a bit strange what you observe regarding the traces stopping. Can you post a cfz/image? And yes, you should be able to see the erosion on the plate outside the nozzle (and any solid in the path of your tracelines).

[proudgrover47]

OK so i attached a print screen of the simulation with traces, let me describe the scenario;

The simulation is for a converging diverging nozzle so there is a part which is converging, then a small part with a constant diameter and finally a diverging part. There are no walls, it is just the shape of the fluid.

I seleceted materials and applied Fluid-Air.

For the Boundary conditions I have 15 Bar Gauge Pressure on the larger diameter (inlet - bar set from a compressor) and 0 Pa Absolute pressure on the smaller diameter (outlet - atmospheric pressure).

Then I autosized the meshing and went on to solve.

For solving, I went on physics and selected it to be compressible and left the default temperatures and hit the solve button with 100 iterations.

Once the results came out I set a plane on the Y axis to see the velocities and then another plane on the inlet diameter, I then edited it to put in a grid and set the traces for the grid, the result is what you can see in the attachment, but somehow it stops just before going into the diverging part of the nozzle. 

Any tips would be greatly appreciated, also I wanted to ask whether the particles could be fed at a flow rate rather than all at once from the grid intersections?

Thanks

Al

[OmkarJ]

Can you post cfz file? It would probably point to something. Also if you want outlet as atmospheric pressure, you should set it as 0 gage pressure, not absolute.

[proudgrover47]

Ok I will do so as soon as I get to a pc, thank you!

[proudgrover47]

Sorry can you please specify what a CFZ file is because I can't seem to find out how to save it

Thanks

Al

[OmkarJ]

Click the upper left button, hover over the arrow against "Save as", select "Save share file" and write the cfz file. Alternately, you can also find the cfz file in the directory you have saved your simulation. 

[proudgrover47]

Thank you for the speedy replies as usual, they are very much appreciated.

I have attached the cfz file.

Thanks

Al

[OmkarJ]

I had a look at your model and the mesh is so coarse that it had distorted the shape of the nozzle! You want a far more refined mesh than that. Do a mesh sensitivity study for this. WIth just a bit of refining the mesh, I was able to see the trace lines...

Also, I realise that you have started another thread with the similar subject, maybe it's best to keep the discussion to either of the threads?

[nhahn]

I have done a bunch of similar nozzle designs and looked at your CFZ file.

First, review the Autodesk guidance on internal compressible flow here: http://help.autodesk.com/view/SCDSE/2014/ENU/?guid=GUID-D763685E-39F1-4CCE-B6C7-CDAC3217A5B2

Per my experience:

1. I agree with OmkarJ your mesh is way too coarse.  Drag the slider on autosize way down (perhaps to .25 or so, then enable mesh adaptation for 2-3 cycles).  Run many more than 100 iterations to allow it to get to a converged solution.
2. You need to use Variable Air in order to get the proper behavior for compressible flow. The DeLaval nozzle won't work without this (it will act like a bad venturi-- you can see the flow separation in OmkarJ's picture) and your results will be useless.  Go to the air material properties, click environment and select variable.
3. Make sure you have inlet & outlet properly selected.  Your description seems to be the opposite of the BCs in the model.
4. Sometimes it helps to have a bit of a pipe section ahead of the nozzle inlet to establish the flow conditions prior to nozzle entry and help it stabilize.  Compressible flows naturally are less stable than incompressible ones. 
5. Set advection scheme 5 when analyzing compressible flow (per the guidance here: http://help.autodesk.com/view/SCDSE/2014/ENU/?guid=GUID-F691B334-CCE2-47E9-B6C4-21666712C163 )

Finally, if your nozzles are axisymetric I would suggest doing 2D models first.  They run faster and you can mesh the heck out of them (which is better for capturing shocks and flow separation).  If you need the 3D one for visualization, do that last when you've settled on a design.

[nhahn]

I tried running your model and actually you may need a much finer mesh than I said, and probably a refinement region around the narrow section and the area downstream of it.  All the more reason to go 2D... I actually quit because by the time I got enough elements to make it stable it was running too slow for me (I need the computer for other things today).  Make sure there are no rapid transitions in the mesh size or you will get artifacts. 

You might also need to properly specify the total temperature in the environment settings to get the energy of the inlet flow right (perhaps an Autodesk person can confirm?)  Don't know if you care about temperatures but the air does behave differently at different temps.

[nhahn]

Last note -- see the tutorial here, it actually runs through a nozzle case. They use a mass flow on the inlet and unknown on the outlet. If I recall, using mass flow or volume flow instead of pressure or velocity at the inlet did help me in the past.

http://help.autodesk.com/view/SCDSE/2014/ENU/?guid=GUID-065F43DD-806B-4209-800F-8E61A0B23D9C

[proudgrover47]

Thank you all so very much you have no idea how much I appreciate the time you have taken to help me!

Unfortunatley I cannot try all the suggestions tonight but I will do so first thing in the morning and get back to you!

Thanks again!

Al

[proudgrover47]

OK so I tried to apply the five steps that nhahn outlined, including variability, advection and a staright pipe before the nozzle, however now an error pops up during analysis, I have attached a screenshot of the error.

Thanks 

Al

[OmkarJ]

Your mesh still seems a lot coarse (6k elements). I have seen instances of divergence with unreasonably coarse mehs. As has been emphasized in earlier posts, it needs to be a lot finer. Unless you sort out the basic issues, you can not hope to move towards your larger objective. Also, as nhahn mentions, using axisymmetric analysis can help you quickly make sure your setup is correct, without modelling a large fine 3D mesh and subsquently, you can move to 3D.

[apolo_vanderberg]

As omkar mentioned you will need 10x the mesh you have or more to properly capture the physics.
Please watch the Basic Meshing SimTV video to get a better understanding of the minimum requirements on meshing. In a situation like this we will need ~10-20nodes around the circumference at the throat as well as 8+ across the gap to capture the shock itself.