Which phase is dispersed in pre and post nozzle spray?

Torque_Converter · February 20, 2013, 13:56

Which phase would be considered continuous and dispersed when the domain physics is very different before and after fluid leaves the nozzle? Would this be a good case for non-constant domain physics?

Basically, oil is flowing through a pipe (with air entrained/dispersed within), which then exits nozzles but not parallel to the nozzle so there is an angle of streamline center. In this case it seems good to model the fluid flowing through the pipe, getting to the outlet, and then see it keep moving into this next environment (the atmosphere). But this atmosphere is now mostly air, with some dispersed oil.

Which fluid should be modeled as the dispersed phase, or should the two domains linked at this nozzle interface be non-constant with oil being dispersed phase in the atmosphere and air being dispersed in the oil? Will this be stable and accurate? Should I model this as one continuous domain but model the air/oil some other way? I don't think a continuous fluid model for both is appropriate in this case.

ghorrocks · February 20, 2013, 17:28

You cannot answer this question without further details. What are you trying to achieve with the simulation? How does the dispersed air in the inlet oil affect things? How does the dispersed oil in the outlet air affect things? What is the volume fraction of the dispersions in both regions? Any other physics going on?

Torque_Converter · February 20, 2013, 19:11

A lube tube has been manufactured with punched holes along its length with the axis of each hole pointed towards the gear mesh. However, in testing they found that in the high pressure areas not only was there the expected wide cone angle dispersion, but the spray was pointed at an angle to the axis largely due to the momentum of the moving fluid inside the tube before entering the raised ridge/lip of the material caused by the punch hole.

I would like to predict two things, the angle from the axis formed due to this manufacturing method (already seeing this qualitativly), and the spray dispersion (also seeing this occuring). However, I would like to increase accuracy and repeatability. The angle from the punch hole "nozzle" axis can be measured against test. However, the dispersion cloud is not directly validate-able. Thus I am interested in using best practices to reduce the chance of inaccuracy.

I have the proper mass flow going into the lube tube, and at the end of the nozzles is an "infinite" atmosphere of air. What I have done so far is to model the air as a dispersed fluid with 100 micron mean diameter (a number from literature) with the oil being continuous. I did this to cover the dispersion/entrainment of air in the oil. I don't think this is correct because the oil will not disperse then once it is in air outside the tube. I know that the mean diameter of oil in air is likely 75 micron from literature again. I am starting with a homogenous, no heat transfer, no free surface, no surface tension, no drag model, but am open to trying those from last iterations to study the sensitivity. However, with the dispersed/continuous fluid issue I feel there is no good solution. I can model the air as dispersed which is great for the tube area where it is entrained, but then it should be continuous in the opening atmosphere. But the oil should be dispersed after exiting the tube, but continuous inside.

I read in a previous thread comment of yours that non-constant domain physics is not applicable in this scenario. The best solution I have come up with is to make the air continuous, oil dispersed, no air entrainment in the tube oil (seems to be a normal assumption made in non-pump/tc/retarder auto applications due to lack of massive pressure differential), and hope that the 75 micron mean diameter dispersed oil in the tube acts as a continuous phase. If you have any additional advice, or think this may be the way to go, I would also appreciate any input you have on homogeneity, free surface modelling, surface tension inclusion, drag model choice, or any other general improvements to a multispecies analysis of this type.

Thanks

ghorrocks · February 21, 2013, 05:19

This sounds a really tricky problem - air bubbles inside oil droplets.

Correct, the non-constant domain physics will not help. You might be able to separate this into two simulations - one to get the air bubbles in the oil up to the injector, then a second using that as the inlet boundary for the oil forming droplets in air. Then you can use the correct continuous phase for each sub-model.

You will also probably want to use a spray breakup model for the oil in air - this is only available with air as the continuous phase.

Also - it is not clear to me what is the point of the point of the punched holes is. Is it to aerate the oil so it breaks up into fine drops easier? If so then this is going to be very tricky - there is no built in model for CFX to model the breakup of an aerated jet. You would have to fine out what people do in the literature for this type of thing.

Torque_Converter · February 21, 2013, 08:43

What is making it trickier is that the oil leaving the tube holes is not leaving normal to the pipe. So I would likely be unable to replicate not only the mass flow, but the vectors involved as the oil leaves the tube holes. I guess the only way I can make it continuous from pipe flow to air is to not entrain the air in the oil, have the oil in the tube enter as a dispersed phase itself, then the air will only be outside the pipe and be continuous.

The holes are punched in order to be cheap. It is a chronic problem that things like aeration as you mention, or solid streams of fluid (what would be ideal here), and other things take a back seat when a penny can be saved.

Torque_Converter · February 21, 2013, 10:38

The spray breakup model is also relatively useless I am finding. It does nothing to predict the cone angle (the reitz bracco method is independent of several key factors in cone angle like pressure ratio). It appears the only way to do this is by using the traditional dispersed phase model.

ghorrocks · February 21, 2013, 17:24

The spray breakup model is designed for automative fuel injectors, where the spray angle is defined by the nozzle geometry. So I guess it is not a surprise it does not work here.

I think you are going to have to do a literature search on this. There is nothing built into CFX which will do this, so you will have to get ideas from other researchers.

February 20, 2013, 13:56	Which phase is dispersed in pre and post nozzle spray?	#1
Torque_Converter Member Join Date: Jan 2012 Location: Edmonton, CA Posts: 87 Rep Power: 14	Which phase would be considered continuous and dispersed when the domain physics is very different before and after fluid leaves the nozzle? Would this be a good case for non-constant domain physics? Basically, oil is flowing through a pipe (with air entrained/dispersed within), which then exits nozzles but not parallel to the nozzle so there is an angle of streamline center. In this case it seems good to model the fluid flowing through the pipe, getting to the outlet, and then see it keep moving into this next environment (the atmosphere). But this atmosphere is now mostly air, with some dispersed oil. Which fluid should be modeled as the dispersed phase, or should the two domains linked at this nozzle interface be non-constant with oil being dispersed phase in the atmosphere and air being dispersed in the oil? Will this be stable and accurate? Should I model this as one continuous domain but model the air/oil some other way? I don't think a continuous fluid model for both is appropriate in this case.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
different CFX Pre and Post mesh region	mactech001	CFX	9	April 11, 2010 22:08
Objects in PRE and POST ?	Felix	CFX	0	January 16, 2008 16:53
clarification in LS Pre post	David	Main CFD Forum	0	July 19, 2007 14:02
Instable Post, Pre and Build	Pascale Fonteijn	CFX	5	December 23, 2003 07:31
PRE and POST processing package	Astrid Barros	Main CFD Forum	6	November 16, 2000 11:31

February 20, 2013, 17:28		#2
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,870 Rep Power: 144	You cannot answer this question without further details. What are you trying to achieve with the simulation? How does the dispersed air in the inlet oil affect things? How does the dispersed oil in the outlet air affect things? What is the volume fraction of the dispersions in both regions? Any other physics going on?

February 20, 2013, 19:11		#3
Torque_Converter Member Join Date: Jan 2012 Location: Edmonton, CA Posts: 87 Rep Power: 14	A lube tube has been manufactured with punched holes along its length with the axis of each hole pointed towards the gear mesh. However, in testing they found that in the high pressure areas not only was there the expected wide cone angle dispersion, but the spray was pointed at an angle to the axis largely due to the momentum of the moving fluid inside the tube before entering the raised ridge/lip of the material caused by the punch hole. I would like to predict two things, the angle from the axis formed due to this manufacturing method (already seeing this qualitativly), and the spray dispersion (also seeing this occuring). However, I would like to increase accuracy and repeatability. The angle from the punch hole "nozzle" axis can be measured against test. However, the dispersion cloud is not directly validate-able. Thus I am interested in using best practices to reduce the chance of inaccuracy. I have the proper mass flow going into the lube tube, and at the end of the nozzles is an "infinite" atmosphere of air. What I have done so far is to model the air as a dispersed fluid with 100 micron mean diameter (a number from literature) with the oil being continuous. I did this to cover the dispersion/entrainment of air in the oil. I don't think this is correct because the oil will not disperse then once it is in air outside the tube. I know that the mean diameter of oil in air is likely 75 micron from literature again. I am starting with a homogenous, no heat transfer, no free surface, no surface tension, no drag model, but am open to trying those from last iterations to study the sensitivity. However, with the dispersed/continuous fluid issue I feel there is no good solution. I can model the air as dispersed which is great for the tube area where it is entrained, but then it should be continuous in the opening atmosphere. But the oil should be dispersed after exiting the tube, but continuous inside. I read in a previous thread comment of yours that non-constant domain physics is not applicable in this scenario. The best solution I have come up with is to make the air continuous, oil dispersed, no air entrainment in the tube oil (seems to be a normal assumption made in non-pump/tc/retarder auto applications due to lack of massive pressure differential), and hope that the 75 micron mean diameter dispersed oil in the tube acts as a continuous phase. If you have any additional advice, or think this may be the way to go, I would also appreciate any input you have on homogeneity, free surface modelling, surface tension inclusion, drag model choice, or any other general improvements to a multispecies analysis of this type. Thanks

February 21, 2013, 05:19		#4
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,870 Rep Power: 144	This sounds a really tricky problem - air bubbles inside oil droplets. Correct, the non-constant domain physics will not help. You might be able to separate this into two simulations - one to get the air bubbles in the oil up to the injector, then a second using that as the inlet boundary for the oil forming droplets in air. Then you can use the correct continuous phase for each sub-model. You will also probably want to use a spray breakup model for the oil in air - this is only available with air as the continuous phase. Also - it is not clear to me what is the point of the point of the punched holes is. Is it to aerate the oil so it breaks up into fine drops easier? If so then this is going to be very tricky - there is no built in model for CFX to model the breakup of an aerated jet. You would have to fine out what people do in the literature for this type of thing.

February 21, 2013, 08:43		#5
Torque_Converter Member Join Date: Jan 2012 Location: Edmonton, CA Posts: 87 Rep Power: 14	What is making it trickier is that the oil leaving the tube holes is not leaving normal to the pipe. So I would likely be unable to replicate not only the mass flow, but the vectors involved as the oil leaves the tube holes. I guess the only way I can make it continuous from pipe flow to air is to not entrain the air in the oil, have the oil in the tube enter as a dispersed phase itself, then the air will only be outside the pipe and be continuous. The holes are punched in order to be cheap. It is a chronic problem that things like aeration as you mention, or solid streams of fluid (what would be ideal here), and other things take a back seat when a penny can be saved.

February 21, 2013, 10:38		#6
Torque_Converter Member Join Date: Jan 2012 Location: Edmonton, CA Posts: 87 Rep Power: 14	The spray breakup model is also relatively useless I am finding. It does nothing to predict the cone angle (the reitz bracco method is independent of several key factors in cone angle like pressure ratio). It appears the only way to do this is by using the traditional dispersed phase model.

February 21, 2013, 17:24		#7
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,870 Rep Power: 144	The spray breakup model is designed for automative fuel injectors, where the spray angle is defined by the nozzle geometry. So I guess it is not a surprise it does not work here. I think you are going to have to do a literature search on this. There is nothing built into CFX which will do this, so you will have to get ideas from other researchers.