Lost .... new injected particles on last node_DPM Fluent
 

Dear Fluent users,

I am working with a cooling tower and using DPM to model my droplets injecting to the towers. During my DPM simulation I see a warning that "lost 200 new injected particles on last node". I searched a bit but couldn't find any solution or similar question. Is there any solution to this warning?

Best Regards,

Amir.

hey,
i have the same problème as you, also i dont no how to get the final mass flow injected.

if you resolve your problème please post the solution.

best regards

Yes, my apologies. I'will delete my answer before someone takes it seriously.

Vasava, I don't think the particle will be "lost" when it touches the wall or outlet. I am using Wall-film for walls and escape for inlet and outlet. To me "lost" means that it could not be tracked.

Here is a thread on this topic. Are you injecting the particles outside of the computation domain? Do you receive this error while running Fluent in serial mode?

Actually, the injection points are inside the computation domain but some of them are close to the wall. Suprisingly, when I change their location it works, but I am sure that their initial locations are inside the computation domain.

What initial conditions have you provided your particles (position relative to wall and velocity)? If there are nonzero velocities assigned to these particles, could they send the particles outside of the domain within one time step?

Try injecting stationary particles near the wall and double check that these particles are within the computation domain or not. Consider a curved geometry, for example a pipe, and if particles are injected on the border of this pipe then they could be located outside of the domain because the mesh has linear connections between nodes.

Well, do you mean that the particles can go outside the computation domain, eventhough I have wall-film BC on my walls?

I am using solid-cone droplets and the injection points are positive relative to the wall. My simulation is steady state both for continous flow and particle tracking.

I'm wondering how the particles are lost considering your problem occurs at the injection of particle streams ("new injected particles") for particles near a wall. Perhaps Fluent injects the particles and provides a portion (or complete) time step for these particles and bypass a boundary condition (unlikely, but a similar bug could be present). Try injecting stationary particles (zero velocity) to test this hypothesis. I've not experienced your error when using DPM very close to a wall (but had zero initial wall normal velocity).

What are the nominal (or otherwise) diameter of the solid-cone droplets and how does this dimension compare to the normal distance from the wall? If you're injecting say a 1 mm diameter particle 0.1 mm from the wall then this particle has already collided with the wall.

Mesh - Geometry Tolerance...
 

I had same issue and this image shows why it is....

https://www.cfd-online.com/Forums/at...1&d=1481643960

In above image, point (for getting location for defining injection, twelve injections were required in total) was created on the curve, but since in mesh mapping is linear from node to node through straight line, so the point(s) which is originally on geometry, is now outside the domain (Mesh). Same is true for all 12 injection created on 12 points.

No flow was going inside the domain through injections...

Here is remedy

Since I needed 12 injections, so i created blocking in such a way that i have twelve points and they are associated to corresponding vertices(4 original edges and 8 extra edges created by splitting block in ICEM CFD Hexa). Which can be seen here :

https://www.cfd-online.com/Forums/at...1&d=1481644311

Now issue is resolved and DPM simulation is running successfully.