need tutorial guide of residence time of tracer

 Register Blogs Members List Search Today's Posts Mark Forums Read

 June 16, 2006, 14:39 need tutorial guide of residence time of tracer #1 mohmed Guest   Posts: n/a i am working with simulation of rtd of tracer(dye) in reacteur. can any one give me a tutorial guide (example in fluent) thank's in advance

 June 20, 2006, 02:59 Re: need tutorial guide of residence time of trace #2 Rajeev Kumar Singh Guest   Posts: n/a There is no tutorial available. But I have been doing RTD in different types of vessel. Both C-curve or F-curve can be drawn. Use levenspiels book as a guide. For this you have to use species transport. Create a material of the type tracer (material prop similar to bulk phase). Then you make a pulse injection in unsteady state for C-curve and continuous injection for F-curve. Monitor the mass fraction of tracer at the point of interest. Finally from the curve you can calculate the various fractions (dead, plug and mixed volume). I hope you get what I mean

 June 21, 2006, 02:31 Re: need tutorial guide of residence time of trace #3 mohmed Guest   Posts: n/a hello rajeev , i have read read your messages in forum about how to introduce tracer but i have found a lot of difficulties, i am praparing to simulate water in tundish and inject the dye ( water) for to get residence time distributions (rtd) in an isothermal and steady case , my problemes are : 1-when i use mixture , the energy equation appears, how to remove this equation and how to put the values of properties of mixture(rho, lunda, cp,...) in the mixture panel ,(mixture :water, dye (water)). 2-i have found negative (static,absolute)pressure.i ask you how to work with operating pressure.(tundish with submerged ladle shroud). thanks in advance

 June 22, 2006, 02:23 Re: need tutorial guide of residence time of trace #4 Rajeev Kumar Singh Guest   Posts: n/a Send me ur e-mail id. I too work in steel industry and you have had ur good luck. I regularly find RTD in tundishes, ladles regulary. I will send u the details then

 June 22, 2006, 14:52 Re: need tutorial guide of residence time of trace #5 mohmed Guest   Posts: n/a my e-mail is :mohamednajoura @ caramail.com best regards

 June 22, 2006, 23:23 Re: need tutorial guide of residence time of trace #6 Rajeev Kumar Singh Guest   Posts: n/a I would suggest you read the chapter on species transport model first. Then you will have some idea and it will be lot easier to explain to you. Keep in mind that energy automatically comes into picture because the mixture-template contains some gaseos terms which you will later delete. You need only water and tracer(same property as water) i.e. you will need density and viscosity and the molecular weight. But this all may sound Greek to you. So I still suggest that you first have a go at the Species Transport Model first. It will be lot easier then Rajeev

 June 23, 2006, 13:54 Re: need tutorial guide of residence time of trace #7 mohmed Guest   Posts: n/a dear sir it is easy for you but it is very difficult for me . i have tried for 6 months but no success . if you want to help me 1000 thanks and if you refused 100000000000000000000 ..... thanks .bye best regards

 June 24, 2006, 02:19 Re: need tutorial guide of residence time of trace #8 Rajeev Kumar Singh Guest   Posts: n/a Ok, since you have written that you have tried it for 6 months and not able to do it so i assume that you have labored hard for that or else in this forum you will find messages where people expect that everything is spoon fed. Here are the steps. Note carefully 1. Go to Model and Enable Species Trabsport model. (Since the default mixture template contains oxygen, nitrogen and water vapor so energy gets automatically enabled). Do not get bothered. 2. Next go to Materials panel and copy any other fluid from database. I usually take mercury. Now change its property. Change name to tracer. Change its density to that of bulk phase (if it is water then tracer should have density of water. I think you get the point). Similarly change the viscosity values as well as the molecular weight. 3. Now go to the drop down list where you select fluid/solid. Here you will find mixture template. No go to the first parameter in the lower half and press edit. A new panel will open up where it shows the water and tracer on the left hand side and oxygen, nitrogen and water vapor on the right hand side. Click on tracer and then add. Similarly click on water and press add. Keep in mind that the bulk phase should be the second. Now remove oxygen, nitrogen and water vapor from the list. Now you have a new mixture consist of tracer and water only. 4. Now go to the density panel and select volume-weighted-mixing law. 5. Change the viscosity value to reflect the viscosity of water 6. Use a value for binary diffusion coefficient. The default value works fine. 7. Now again go back to fluid and see to it that the molecular weight of tracer and water are the same. 8. Once you have created the new mixture with volume weighted mixing law you can disable energy. 9. Now you go to boundary conditions and ensure that the mass fraction of tracer is 1 at the inlet. 10. Create point monitors near your tundish outlet and monitor the mass fraction of tracer using vertex average 11. Run the simulation in unsteady state for 1-10 second as you wish. 12. Go back to boundary conditions and make sure that the mass fraction is set back to zero and then run the simulation for fairly long time. At least 6 times of nominal residence time 13. Now you have the C-curves and then you do the analysis Hope this helps. I have tried to make it as clear as I can Please let me know if you need any further clarifications

 June 24, 2006, 14:55 Re: need tutorial guide of residence time of trace #9 mohmed Guest   Posts: n/a thankyou sir for your precious help , i want to confirm my work, i have only these questions : 1-i have put in surface monitors" mass wheighted average "for to calcule concentration , is it true ?. 2-how to put operting pressure?, because i have got negative pressure (static and total...)when i have used default value of pressure location . 3- I have a nominal time equal to 232 seconde and i have used a time step size equal to 1e-3 for seven iteration in order to converge my calcul for each time step size , i have found a large and very slow calcul .i ask if you have met a same problem and how to solve it . help me sir singh , my supervisor has leaves me and he lets me alone and he refused to help me , i am in very complicated situation , i want just to acheive my master . best regards , i am very shocked by your help , i remercie you sir.

 June 25, 2006, 22:46 Re: need tutorial guide of residence time of trace *NM* #10 Rajeev Kumar Singh Guest   Posts: n/a

 June 25, 2006, 22:51 Re: need tutorial guide of residence time of trace #11 Rajeev Kumar Singh Guest   Posts: n/a Mass weighted average is fine. As for the operating pressure make sure that the default operating pressure of 101325 Pa is located somewhere inside your domain. Also for a case of tundish flow you are using a very small time step. Keep it at 1 second and run for at least 1500 seconds. Could you care to send your case and data file to me to have a look. Send it on vinitraj3@yahoo.co.in

 May 21, 2010, 02:11 Hi..mohamed and Rajeev #12 New Member   Srinivas Join Date: Mar 2010 Posts: 3 Rep Power: 7 This is srinivas...I am going to start the same problem...getting RTD curves in tundish. I think the flow behavior as well as RTD gets effected with the volume of liquid in the tundish and when the ladle change takes place the height of the liquid changes significantly. Can anyone suggest me, wat schemes should i use to solve this phenomenon...I think VOF can be used for this... so pls let me know to wat extent my assumption is true?

June 4, 2011, 06:00
#13
New Member

elham
Join Date: Jun 2011
Posts: 1
Rep Power: 0
Hi
I have two questions.
1)Is this procedure the trace seems be pulse input?
2)can I use this procedure for gas flow(my mail flow is gas)?
thanks a lot

Quote:
 Originally Posted by Rajeev Kumar Singh ;133568 Ok, since you have written that you have tried it for 6 months and not able to do it so i assume that you have labored hard for that or else in this forum you will find messages where people expect that everything is spoon fed. Here are the steps. Note carefully 1. Go to Model and Enable Species Trabsport model. (Since the default mixture template contains oxygen, nitrogen and water vapor so energy gets automatically enabled). Do not get bothered. 2. Next go to Materials panel and copy any other fluid from database. I usually take mercury. Now change its property. Change name to tracer. Change its density to that of bulk phase (if it is water then tracer should have density of water. I think you get the point). Similarly change the viscosity values as well as the molecular weight. 3. Now go to the drop down list where you select fluid/solid. Here you will find mixture template. No go to the first parameter in the lower half and press edit. A new panel will open up where it shows the water and tracer on the left hand side and oxygen, nitrogen and water vapor on the right hand side. Click on tracer and then add. Similarly click on water and press add. Keep in mind that the bulk phase should be the second. Now remove oxygen, nitrogen and water vapor from the list. Now you have a new mixture consist of tracer and water only. 4. Now go to the density panel and select volume-weighted-mixing law. 5. Change the viscosity value to reflect the viscosity of water 6. Use a value for binary diffusion coefficient. The default value works fine. 7. Now again go back to fluid and see to it that the molecular weight of tracer and water are the same. 8. Once you have created the new mixture with volume weighted mixing law you can disable energy. 9. Now you go to boundary conditions and ensure that the mass fraction of tracer is 1 at the inlet. 10. Create point monitors near your tundish outlet and monitor the mass fraction of tracer using vertex average 11. Run the simulation in unsteady state for 1-10 second as you wish. 12. Go back to boundary conditions and make sure that the mass fraction is set back to zero and then run the simulation for fairly long time. At least 6 times of nominal residence time 13. Now you have the C-curves and then you do the analysis Hope this helps. I have tried to make it as clear as I can Please let me know if you need any further clarifications

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post sanjose FLUENT 0 October 18, 2010 10:11 panda60 OpenFOAM Bugs 4 July 8, 2010 10:23 pkleb FLUENT 0 June 20, 2010 17:52 liugx212 OpenFOAM Running, Solving & CFD 3 January 4, 2006 19:07 Sugen Chetty Main CFD Forum 0 January 28, 2002 10:50

All times are GMT -4. The time now is 10:45.