CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

need tutorial guide of residence time of tracer

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 16, 2006, 14:39
Default 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
  Reply With Quote

Old   June 20, 2006, 02:59
Default 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
  Reply With Quote

Old   June 21, 2006, 02:31
Default 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

  Reply With Quote

Old   June 22, 2006, 02:23
Default 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
  Reply With Quote

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

Old   June 22, 2006, 23:23
Default 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
  Reply With Quote

Old   June 23, 2006, 13:54
Default 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

  Reply With Quote

Old   June 24, 2006, 02:19
Default 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
  Reply With Quote

Old   June 24, 2006, 14:55
Default 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.
  Reply With Quote

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

Old   June 25, 2006, 22:51
Default 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
  Reply With Quote

Old   May 21, 2010, 02:11
Default Hi..mohamed and Rajeev
  #12
New Member
 
Srinivas
Join Date: Mar 2010
Posts: 3
Rep Power: 7
srinu7257 is on a distinguished road
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?
srinu7257 is offline   Reply With Quote

Old   June 4, 2011, 06:00
Default
  #13
New Member
 
elham
Join Date: Jun 2011
Posts: 1
Rep Power: 0
elhamchemical is on a distinguished road
Hi
Thanks for your good explian.
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
elhamchemical is offline   Reply With Quote

Reply

Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Residence Time Distribution with Periodic Boundary Conditions sanjose FLUENT 0 October 18, 2010 10:11
directMapped problem panda60 OpenFOAM Bugs 4 July 8, 2010 10:23
Pathline colored by time = residence time pkleb FLUENT 0 June 20, 2010 17:52
Could anybody help me see this error and give help liugx212 OpenFOAM Running, Solving & CFD 3 January 4, 2006 19:07
residence time Sugen Chetty Main CFD Forum 0 January 28, 2002 10:50


All times are GMT -4. The time now is 12:30.