[potatoning]

There‘s a face in the flow field, i want to set the property of this face is that the droplets escaped from this face and the continuous phase passed this face as an interface. How can i do that??
sincerely~

[`e`]

Here's a couple of possible methods (not checked or validated) for creating a quasi-internal boundary face for your DPM phase:
1) split the geometry into two cell zones and apply a DPM wall type of escape at the interior face
2) at each DPM step, determine whether or not the particle stream has passed this quasi-face and either continue or escape

[potatoning]

Originally Posted by `e`

Here's a couple of possible methods (not checked or validated) for creating a quasi-internal boundary face for your DPM phase:
1) split the geometry into two cell zones and apply a DPM wall type of escape at the interior face
2) at each DPM step, determine whether or not the particle stream has passed this quasi-face and either continue or escape

tks alot
i saw the reply about another dpm problem which I asked.
my propose is to get the temperature and flow rate of droplets in that interface, and the droplets calculation is ended in that interface also.
Now, I have divided the flow field into 2 cell zones, and coupled the contact surfaces in mesh interfaces. I can't find the way to set the surfaces into interior in FLUENT.
I'll try to split the flow field and check the results.
thank you

[potatoning]

Originally Posted by `e`

Here's a couple of possible methods (not checked or validated) for creating a quasi-internal boundary face for your DPM phase:
1) split the geometry into two cell zones and apply a DPM wall type of escape at the interior face
2) at each DPM step, determine whether or not the particle stream has passed this quasi-face and either continue or escape

I can't find the way to set the dpm wall type in interior face edit...
it's empty..how can i do that?

[`e`]

Hmm, it's unfortunate the DPM BC can't be applied to an interior face, that would have been the easiest way. Could you set the interior face to a pressure outlet (DPM BC can then be applied) and then use that velocity profile as the inlet to the next cell zone? This approach might only work if you have developed flow because of the pressure outlet.

Otherwise, try method 2, where you check the position of all particles at each time step (DEFINE_EXECUTE_AT_END) and remove the particles which have passed your interface.

[potatoning]

Originally Posted by `e`

Hmm, it's unfortunate the DPM BC can't be applied to an interior face, that would have been the easiest way. Could you set the interior face to a pressure outlet (DPM BC can then be applied) and then use that velocity profile as the inlet to the next cell zone? This approach might only work if you have developed flow because of the pressure outlet.

Otherwise, try method 2, where you check the position of all particles at each time step (DEFINE_EXECUTE_AT_END) and remove the particles which have passed your interface.

I found a way to add DPM BC. Changing the BC from interior to porous-jump could active the DPM BC type. But it is strange that i set the DPM BC type into escape or use the udf DPMBC to set the particles abort, the particles still pass through this BC interior.

[`e`]

The porous-jump boundary condition type works for me by setting the DPM BC to escape (only a quick test case, not the same model as you have). Also, be careful the settings are such that they don't inadvertently impact your continuous phase!

[potatoning]

Originally Posted by `e`

The porous-jump boundary condition type works for me by setting the DPM BC to escape (only a quick test case, not the same model as you have). Also, be careful the settings are such that they don't inadvertently impact your continuous phase!

just one question: did you split the model into two cell zone by icem? I used the porous-jump BC after mesh interfaces, it didn't work.
Now I'm trying to split the model in icem. I think that the interior built by mesh interface is the problem.

[`e`]

It was simply the interior face type within Fluent (I didn't split zones or anything).

[potatoning]

Originally Posted by `e`

It was simply the interior face type within Fluent (I didn't split zones or anything).

the droplets still passed through the porous jump interior..
I don't know what happened.
Could you sent your test file to me?
Email: Martin.ningtao@gmail.com
tks a lot~

[`e`]

See the attached figures for the settings and before and after changing DPM BC to escape at the interior plane (respectively).

[potatoning]

Originally Posted by `e`

See the attached figures for the settings and before and after changing DPM BC to escape at the interior plane (respectively).

too strange
I set it in the same way。。
wtf。。。
what is the role of another interior upper？

[`e`]

Originally Posted by potatoning

what is the role of another interior upper？

Can you explain what you mean by this question?

[potatoning]

Originally Posted by `e`

See the attached figures for the settings and before and after changing DPM BC to escape at the interior plane (respectively).

i couple 2 overlapping interface to 1 interior with mesh interfaces
and set the new interior to porous jump
after calculation, I checked the particle residence time in results.
The droplets still passed the porous jump face.
DPM BC trap/ escape/ reflect are all tested.

[`e`]

I created two cuboids in DesignModeler and formed one part leaving a single interior boundary between the two halves.

Do you have source and target interfaces which overlap? See the attached figure for a complete list of my cell and boundary zones. Try creating the separate regions in the geometry stage rather than at the mesh or Fluent stage.

[potatoning]

Originally Posted by `e`

I created two cuboids in DesignModeler and formed one part leaving a single interior boundary between the two halves.

Do you have source and target interfaces which overlap? See the attached figure for a complete list of my cell and boundary zones. Try creating the separate regions in the geometry stage rather than at the mesh or Fluent stage.

two overlapping interfaces belong to 2 independent cell zones, and defined their property in GAMBIT.
Do you use mesh interfaces to couple the interfaces of startcell and endcell?
i haven't added the UDF source yet

[`e`]

I did not use mesh interfaces, you can create two cuboids in DesignModeler and then select the two bodies > right click > form new part.

[potatoning]

Originally Posted by `e`

I did not use mesh interfaces, you can create two cuboids in DesignModeler and then select the two bodies > right click > form new part.

you mean that you create cuboids in DM, then form new part in ICEM?

[`e`]

No, the entire geometry is created in DesignModeler. See attached figures for before and after screenshots of forming the new part (this action allows Fluent to treat the two cuboids as one continuous domain instead of having interfaces with source and target faces).

[potatoning]

Originally Posted by `e`

No, the entire geometry is created in DesignModeler. See attached figures for before and after screenshots of forming the new part (this action allows Fluent to treat the two cuboids as one continuous domain instead of having interfaces with source and target faces).

Then,How did you create the mesh?
unfortunately, i haven't used the DM or Workbench before...
I just trying to figure out in ICEM