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

how to put resistance in ansys

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 20, 2014, 04:32
Default how to put resistance in ansys
  #1
Member
 
hashim chaudhry
Join Date: Jun 2014
Location: turkey
Posts: 44
Rep Power: 3
chaudhry_hashim is on a distinguished road
Send a message via Skype™ to chaudhry_hashim
Hi I am working on the simulation of axial fan I want to put some resistance at the end of downstream duct in order to chock some flow. I am wondering to put 2d resistance element at the end of downstream duct.

Can anyone guide me how can I put resistance and what values should I required for this ?
chaudhry_hashim is offline   Reply With Quote

Old   August 20, 2014, 06:15
Default
  #2
Senior Member
 
amin.z's Avatar
 
Amin
Join Date: Oct 2013
Location: Somewhere on Earth
Posts: 297
Rep Power: 5
amin.z is on a distinguished road
Quote:
Originally Posted by chaudhry_hashim View Post
Hi I am working on the simulation of axial fan I want to put some resistance at the end of downstream duct in order to chock some flow. I am wondering to put 2d resistance element at the end of downstream duct.

Can anyone guide me how can I put resistance and what values should I required for this ?
Hey!

Do you need a heat resistance?
You can model a block and use heat flux for its!
__________________
Best regards,
Amin
amin.z is offline   Reply With Quote

Old   August 20, 2014, 06:24
Default Air resistance
  #3
Member
 
hashim chaudhry
Join Date: Jun 2014
Location: turkey
Posts: 44
Rep Power: 3
chaudhry_hashim is on a distinguished road
Send a message via Skype™ to chaudhry_hashim
No Sir, I want to put air resistance in downstream duct so that I can block some flow and is there any option in fluent to a put 2D resistance element but my model is 3D.
chaudhry_hashim is offline   Reply With Quote

Old   August 20, 2014, 06:30
Default
  #4
Senior Member
 
amin.z's Avatar
 
Amin
Join Date: Oct 2013
Location: Somewhere on Earth
Posts: 297
Rep Power: 5
amin.z is on a distinguished road
Quote:
Originally Posted by chaudhry_hashim View Post
No Sir, I want to put air resistance in downstream duct so that I can block some flow and is there any option in fluent to a put 2D resistance element but my model is 3D.
Sorry! I don't understand your meaning!
Can you attach some pictures?
__________________
Best regards,
Amin
amin.z is offline   Reply With Quote

Old   August 20, 2014, 09:08
Default hi
  #5
Member
 
hashim chaudhry
Join Date: Jun 2014
Location: turkey
Posts: 44
Rep Power: 3
chaudhry_hashim is on a distinguished road
Send a message via Skype™ to chaudhry_hashim
I have attached the layout of my setup unfortunately I dont have any proper setup picture to show you sorry for that.

As you can see in the picture that I rotating fan with extruded duct on both sides of fan. In the end of the downstream duct I want to put some blockage or resistance as mentioned in picture so that I can get pressure rise across the fan in order to get the fan performance curve at different flowrates. So I am confused that should I have make another region in the downstream duct then asssign as a porous region region in fluent or is there any other way in fluent to do this. It should be similar like we introduce grill in ICEPAK in which we give free area ratio

Thanks

Hashim
Attached Images
File Type: jpg layout.jpg (21.5 KB, 16 views)
chaudhry_hashim is offline   Reply With Quote

Old   August 20, 2014, 10:44
Default
  #6
Senior Member
 
amin.z's Avatar
 
Amin
Join Date: Oct 2013
Location: Somewhere on Earth
Posts: 297
Rep Power: 5
amin.z is on a distinguished road
Quote:
Originally Posted by chaudhry_hashim View Post
I have attached the layout of my setup unfortunately I dont have any proper setup picture to show you sorry for that.

As you can see in the picture that I rotating fan with extruded duct on both sides of fan. In the end of the downstream duct I want to put some blockage or resistance as mentioned in picture so that I can get pressure rise across the fan in order to get the fan performance curve at different flowrates. So I am confused that should I have make another region in the downstream duct then asssign as a porous region region in fluent or is there any other way in fluent to do this. It should be similar like we introduce grill in ICEPAK in which we give free area ratio

Thanks

Hashim
Oh! amazing!
Sorry! But I haven't experience in this case!
But I think if the resistance isn't too small respect to duct size you don't need to use another option for solution...!
__________________
Best regards,
Amin
amin.z is offline   Reply With Quote

Old   August 20, 2014, 11:49
Default
  #7
Senior Member
 
Andrew Kokemoor
Join Date: Aug 2013
Posts: 116
Rep Power: 4
Kokemoor is on a distinguished road
Porous jump is probably the way to go. You'll need to have two zones so that you have an interior interface between them, but porous jump is simpler and more robust than a porous media zone.

Even simpler would be to just set the outlet pressure as a parameter and make the parameter a function of the flow rate.
Kokemoor is offline   Reply With Quote

Old   August 20, 2014, 13:51
Default hi
  #8
Member
 
hashim chaudhry
Join Date: Jun 2014
Location: turkey
Posts: 44
Rep Power: 3
chaudhry_hashim is on a distinguished road
Send a message via Skype™ to chaudhry_hashim
Thankyou so much for your support. You mean I have total four regions upstream region, rotating region, downstream region and porous region. Is that you mean ?
chaudhry_hashim is offline   Reply With Quote

Old   August 20, 2014, 18:40
Default
  #9
Senior Member
 
Andrew Kokemoor
Join Date: Aug 2013
Posts: 116
Rep Power: 4
Kokemoor is on a distinguished road
Sort of. Yes, you would have four regions. You could use a porous region, or instead basically have two downstream regions separated by a porous jump. I suggest you read about porous jump in the Fluent manual and see if it suits your needs.
Kokemoor is offline   Reply With Quote

Old   August 21, 2014, 02:09
Lightbulb
  #10
Member
 
Anonymous
Join Date: Mar 2014
Posts: 57
Rep Power: 3
marauder is on a distinguished road
Radiator boundary condition will be the easiest way to go.
However if you want to have much better control over pressure drop and write UDF's for it then Porous zone is the way to go.
marauder is offline   Reply With Quote

Old   August 21, 2014, 11:08
Default hi
  #11
Member
 
hashim chaudhry
Join Date: Jun 2014
Location: turkey
Posts: 44
Rep Power: 3
chaudhry_hashim is on a distinguished road
Send a message via Skype™ to chaudhry_hashim
Thanks everyone for guiding me. I have attached the formula that I am going to use for Pressure drop calculation. I have a little confusion regarding the formula that how can I calculate the Pressure jump coefficient and should I use the pemiability of specific material
Attached Images
File Type: jpg porous.jpg (83.5 KB, 8 views)
chaudhry_hashim is offline   Reply With Quote

Old   August 21, 2014, 23:05
Default
  #12
Member
 
Anonymous
Join Date: Mar 2014
Posts: 57
Rep Power: 3
marauder is on a distinguished road
If your goal is to apply specific amount of pressure drop then I suggest you to use radiator instead, it'll be much easier to calculate.

Use the below formula and calculate Kl as required, as all other values will be known.

Keep it constant in fluent and input the value
Attached Images
File Type: jpg 123.JPG (45.3 KB, 10 views)
marauder is offline   Reply With Quote

Old   August 22, 2014, 03:43
Default hi
  #13
Member
 
hashim chaudhry
Join Date: Jun 2014
Location: turkey
Posts: 44
Rep Power: 3
chaudhry_hashim is on a distinguished road
Send a message via Skype™ to chaudhry_hashim
Thanks marauder, I am trying to use radiator which you told me. My goal is to get the fan curve. I am selecting the interior surface between the downstream and porous region that I made at the end of the downstream, one face of porous region is interface with downstream and the other face is pressure outlet. I am giving the value of loss coefficient as a constant and I have ask one thing that should I divide the value of loss coefficient by the thickness of the porous region or not ?

Thanks again for your precious time and guidance
chaudhry_hashim is offline   Reply With Quote

Old   August 22, 2014, 07:36
Default
  #14
Member
 
Anonymous
Join Date: Mar 2014
Posts: 57
Rep Power: 3
marauder is on a distinguished road
Quote:
Originally Posted by chaudhry_hashim View Post
Thanks marauder, I am trying to use radiator which you told me. My goal is to get the fan curve. I am selecting the interior surface between the downstream and porous region that I made at the end of the downstream, one face of porous region is interface with downstream and the other face is pressure outlet. I am giving the value of loss coefficient as a constant and I have ask one thing that should I divide the value of loss coefficient by the thickness of the porous region or not ?

Thanks again for your precious time and guidance
I can't understand what you mean by porous region here. There is no need to create a solid zone as you are not going to study this region. Just create a plane (or a slice) before your outlet parallel to it and define it as a radiator boundary condition. Since, it'll be a plane you don't require to divide the coefficient by thickness.
marauder is offline   Reply With Quote

Old   August 22, 2014, 07:50
Default hi
  #15
Member
 
hashim chaudhry
Join Date: Jun 2014
Location: turkey
Posts: 44
Rep Power: 3
chaudhry_hashim is on a distinguished road
Send a message via Skype™ to chaudhry_hashim
Thanks Ok I got it now
chaudhry_hashim is offline   Reply With Quote

Old   August 25, 2014, 03:09
Default hi
  #16
Member
 
hashim chaudhry
Join Date: Jun 2014
Location: turkey
Posts: 44
Rep Power: 3
chaudhry_hashim is on a distinguished road
Send a message via Skype™ to chaudhry_hashim
I make the plane in the desired location in downstream but I am unable to give boundary condition to that plane although it didnt appear in boundary condition panel. How can I give boundary condition to the plane that I made ?
chaudhry_hashim is offline   Reply With Quote

Old   August 25, 2014, 03:18
Default
  #17
Member
 
Anonymous
Join Date: Mar 2014
Posts: 57
Rep Power: 3
marauder is on a distinguished road
Quote:
Originally Posted by chaudhry_hashim View Post
I make the plane in the desired location in downstream but I am unable to give boundary condition to that plane although it didnt appear in boundary condition panel. How can I give boundary condition to the plane that I made ?
Easiest way is to go to your solid model and create a slice at that place. Give it a name while meshing if you are using ansys meshing. Then it'll appear in your BC's.
marauder is offline   Reply With Quote

Old   September 5, 2014, 03:40
Default hi
  #18
Member
 
hashim chaudhry
Join Date: Jun 2014
Location: turkey
Posts: 44
Rep Power: 3
chaudhry_hashim is on a distinguished road
Send a message via Skype™ to chaudhry_hashim
As you can see from the model image that the downstream duct is comprising of two parts in which there is a interface and i am giving radiator boundary condition to the interior surface at the location. I calculated the value of loss coefficient by considering the pressure drop value from the curve and velocity corresponding to pressure drop but I didn't get the required results kindly take a look whether the model is OK ?
I am giving 0 Pa pressure at both inlet and outlet boundary condition and in radiator boundary cond. I am giving a constant value.
Attached Images
File Type: jpg model.jpg (29.2 KB, 5 views)
chaudhry_hashim is offline   Reply With Quote

Old   September 5, 2014, 03:52
Default
  #19
Member
 
Anonymous
Join Date: Mar 2014
Posts: 57
Rep Power: 3
marauder is on a distinguished road
Quote:
Originally Posted by chaudhry_hashim View Post
As you can see from the model image that the downstream duct is comprising of two parts in which there is a interface and i am giving radiator boundary condition to the interior surface at the location. I calculated the value of loss coefficient by considering the pressure drop value from the curve and velocity corresponding to pressure drop but I didn't get the required results kindly take a look whether the model is OK ?
I am giving 0 Pa pressure at both inlet and outlet boundary condition and in radiator boundary cond. I am giving a constant value.
What do you mean by velocity corresponding to pressure drop?
You want loss coefficient for a given pressure drop. The values of density and velocity should be taken at that plane from fluent or by calculating the density and velocity yourself using basic principles. This method will work fine if you are using constant density.

If your pressure drop does not vary linearly in your graph then use a curve fit to find a equation for the curve and define your K as polynomial in fluent.
marauder is offline   Reply With Quote

Old   September 5, 2014, 04:32
Default hi
  #20
Member
 
hashim chaudhry
Join Date: Jun 2014
Location: turkey
Posts: 44
Rep Power: 3
chaudhry_hashim is on a distinguished road
Send a message via Skype™ to chaudhry_hashim
My main task is to plot fan curve i.e pressure rise across the fan vs. flowrate so for that reason I have to put some resistance at the end of the downstream so that I can get the pressure difference between the total pressure at the upstream and static pressure at the downstream.
I am confuse about one thing that you said I have calculate the density and velocity at that plane then how would I calculate the value of loss coefficient which I have to give before running the case.

Thankyou for your precious time
chaudhry_hashim 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
Putting Boundary Conditions in ANSYS CFX 12.1 palofpinaki CFX 7 January 5, 2015 06:51
Command Line Run for ANSYS Liaquat ANSYS 9 February 1, 2013 02:32
Pro/E to ANSYS Parameterization Guide Trues ANSYS 1 September 21, 2012 10:05
FSI simulation in ansys cfx Arash67.m CFX 0 August 11, 2012 07:18
ANSYS LS-DYNA export, mechanicaldesign ANSYS 0 July 22, 2012 03:30


All times are GMT -4. The time now is 20:29.