[pdhyani96]

I am trying to emulate the effect of jet injection on a surface using source points. I want to create a 1 mm diameter of injection size. From the manual, I have understood this so far. Source points are 3D volumetric sources applied applied over a single element. The source is distributed equally over the vertices of a given element.


The question I have is, how do I make a injection hole using source points that is of 1 mm diameter? I had an idea to select all the nodes that lie within the circle boundary of 1-mm diameter hole. But, if the source is distributed among all the vertices of the selected 3-D elements, there will be some elements that intersect circle boundary causing some vertices to be outside of the circle boundary. In that case, how do I make sure that the size of the injection is exactly 1 mm?

All in all, is this a valid approach to create the effect of an actual jet of a given diameter using source points?

[Opaque]

May I ask which version of the software you are using?

Since ANSYS CFX 19.2, there is a feature to deal exactly with these models.

Using source points your solution will be smeared. Using boundary sources once you get it right will give you a better solution, but there still be some issues (a source does not remove the wall presence for that area).

Finally, the injection region approach will behave nearly like an inlet. Of course with the error associated with no resolving mesh nearby to capture the jet spread.

If you will be doing injection modeling w/o resolving the mesh, you are better off upgrading (at least) to ANSYS CFX 2020R2 or better yet 2021R1

[pdhyani96]

I am using academic ANYS 18.2 provided by my university. I can't upgrade as the node count is greater than 512 k nodes. I have made sure that the yplus is <0.25 to account for the jet injection. But, I am just concerned about the validity of claiming an injection area. There is little to no literature on source points, which make its extremely difficult to work with.

Any suggestions about getting as close as possible to the desired injection size will be much appreciated.

[ghorrocks]

Source terms can be applied to a point (where it is actually applied to a single element, as previously mentioned) or a volume. So just define a volume which is 1mm in diameter and make it a sub-domain and apply a source term to it.

But why can't you model your jet as a simple inlet condition? Much simpler. You only need source terms when you are recirculating the fluid inside the domain. If you are not recirculating then just use a normal inlet boundary.

[Opaque]

Originally Posted by pdhyani96

I am using academic ANYS 18.2 provided by my university. I can't upgrade as the node count is greater than 512 k nodes. I have made sure that the yplus is <0.25 to account for the jet injection. But, I am just concerned about the validity of claiming an injection area. There is little to no literature on source points, which make its extremely difficult to work with.

Any suggestions about getting as close as possible to the desired injection size will be much appreciated.

May I ask how you came to the conclusion of using source points instead of a boundary source?

[pdhyani96]

One of my main goals is to validate the use of source points and compare it with an actual jet injection. What I still don't understand is how source points are modelled. There is little to no explanation given in the manual. And if I cant decide on the injection size, I am comparing apples with oranges.

The source points get distributed over all the vertices of a volume. I was under the impression that the source is applied from the selected node. Now this makes is difficult for me to create an similar setup that acts like a 1-mm diameter jet

[ghorrocks]

I will repeat my previous post:

Source terms can be applied to a point (where it is actually applied to a single element, as previously mentioned) or a volume. So just define a volume which is 1mm in diameter and make it a sub-domain and apply a source term to it.

Doesn't that do what you want? Then you can define the source volume to have whatever shape and size you want.

[pdhyani96]

Yes, forgive me for not clarifying the main problem.

My injection size is overpredicted. The effect of sourcing (injection) is also seen in the nearby cells where I dont apply the sourcing.

[ghorrocks]

Yes, because the flow generated in the source entrains adjacent fluid and drags it along with it.

If you want to stop this then put a wall around the source volume.

[Opaque]

Originally Posted by pdhyani96

One of my main goals is to validate the use of source points and compare it with an actual jet injection. What I still don't understand is how source points are modelled. There is little to no explanation given in the manual. And if I cant decide on the injection size, I am comparing apples with oranges.

The source points get distributed over all the vertices of a volume. I was under the impression that the source is applied from the selected node. Now this makes is difficult for me to create an similar setup that acts like a 1-mm diameter jet

As stated above, your goal is to validate the use of source points for a reduced model of injection. Then, you have already setup a case, and verified (not told) that the injected amount is spread through the mesh regardless of the size of your injection, correct?

Conclusion: modeling of injection using source points as implemented in ANSYS CFX is dependent of mesh distribution because the source is applied on the element, and NOT on the control volume. There is nothing else you can do at this point except accepting the constraints, i.e. the mesh should be fine enough that the spread is tolerable/acceptable for your simulations.

Not sure how to best tell you have already arrived at your goal.

[pdhyani96]

Mesh refinement is the key! Thank you. I didn't realize I had the solution in front of me! Apologize for going around the circle.