×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Radiosity Solver and RSURF

Radiosity Solver and RSURF

Radiosity Solver and RSURF

(OP)
Hi - I'm having problems using the radiosity solver.

I am trying to model a thin plate.  Heat is generated on the plate and then there is radiative cooling.  For a single plate I think I have the model working correctly.

However, I also require to simulate a double plate scenario, where the plates radiate between themselves, as well as the surroundings.  

flash3780 kindly sent this useful link:  http://www.ansys.com/staticassets/ANSYS/staticassets/resourcelibrary/article/AA-V1-I1-View-Factoring-Radiation.pdf

But I am still having trouble in getting radiation between the plates.  Presently I am only heating one plate, to see if I can see any heat transfer to the other - but I see nothing :(

I have attached my macro file in case anyone can see anything that I'm doing obviously wrong?  Or can give me any tips for succeeding?

http://files.engineering.com/getfile.aspx?folder=98714087-98c8-4280-9bd0-b9f4994997b8&file=KEKRAD.mac

Thanks for any help you are able to offer, all very much appreciated.

HVSmith  

RE: Radiosity Solver and RSURF

I think that one problem is that you're problem is issuing the RSURF command more than once for the same enclosure. I think that if you use SFE, you must first issue RSURF to create the elements, select those elements, and then issue SFE to apply the boundary condition. From the Ansys command reference:

Quote:

If you have already issued RSURF for a surface and you issue RSURF again, ANSYS creates a new set of radiosity elements and nodes over the existing set, resulting in an erroneous solution.

Also, if you're radiating between infinite(?) plates, you may want to issue the VFSM command to prevent your model from radiating into space. But, I've found that even when scaling the view-factor sum to zero, I still need to define a SPCTEMP for the enclosure... not sure why.

You may want to start with a static problem before jumping into a transient problem... just for easier debugging.

RE: Radiosity Solver and RSURF

Oh, I forgot to mention: If you're radiating across small gaps, contact elements can handle the behavior much more efficiently (though the functionality is not well documented in the ANSYS help). Check Sheldon's page for details (the website seems to be down at the moment, but I'm sure it'll be back soon):
http://ansys.net/?mycat=search&mytype=Tips&;mycategory=HeatXfer

Basically, you need to apply your boundary condition to a frictionless, symmetric contact pair (CONTA172) in near-contact (i.e. within the pinball region) using the SFE command. Here's an example that I've used recently in one of my Workbench models (input as a command snippet inserted under a contact pair):

CODE

!   Commands inserted into this file will be executed just after the contact region definition.
!   The type number for the contact type is equal to the parameter "cid".
!   The type number for the target type is equal to the parameter "tid".
!   The real and mat number for the asymmetric contact pair is equal to the parameter "cid".
!   The real and mat number for the symmetric contact pair(if it exists) is equal to the parameter "tid".

!   Active UNIT system in Workbench when this object was created:  Metric (m, kg, N, s, V, A)

nropt,full
a = cid        ! Store the contact ID in some variable

!*********ENTER EMISSIVITY HERE*********!
e1 = 0.950    ! Microsil Insulation (http://www.zircarceramics.com/pages/microporusinsulation/microporous.htm)
e2 = 0.950    ! Microsil Insulation (http://www.zircarceramics.com/pages/microporusinsulation/microporous.htm)
e12= e1*e2/(e1 + e2 - e1*e2)

MP, emis, a, e12,               ! Define the emissivity as a material property to the material used for contact elements whose ID is 'a'
!*********ENTER CONVECTION HERE*********!
mptemp,        1,      0,    100,    200,    300,    400,    500,    600,    700,    800,    900,   1000
mpdata, hf, a, 1,   5.77,   7.56,   9.26,  10.79,  12.14,  13.34,  14.25,  15.57,  16.72,  17.86,  19.09    ! Define Gap Convection (4.20mm)

keyopt, a,  1, 2
rmodif, a, 14, 0.00e00
rmodif, a, 16, 5.67e-8        ! Modify real constant number 16 for contact id 'a' to input steffan boltzman constant
!*********ENTER VIEW FACTOR HERE*********!
R1=38.55e-3
R2=42.75e-3
VF=R1/R2
rmodif, a, 17,VF            ! Modify real constant number 17 for contact id 'a' to input radiation viewing factor

esel,s,type,,a
esel,r,ename,,conta174

sfe,all,1,conv,1,-a
sfe,all,1,conv,2,100

allsel

RE: Radiosity Solver and RSURF

^ Erm... mind you, later on I've issued a TOFFST command...

RE: Radiosity Solver and RSURF

(OP)
Hi - thanks for your replies - they've been useful to read and I think I have it working now.  

I am also trying to model a single plate case where it is heated and then radiates to ambient.  

Initially I was using RDSF to do this, but the viewfactors were all zero (can't decide if this is a problem or not, in radiating to ambient) so I tried using RAD but keep getting the warning:  

"RAD option on SF/SFE command is only supported by FLOTRAN elements (Fluid141, Fluid142).  Elements Surf151 and Surf152 with Keyopy(9)>0 without the SF/SFE command should be used for further analyses."

Now, I'm using Shell131 and then the RSURF command to generate Surf252's - am I better sticking with RDSF (even though there are no other surfaces) or change what I'm doing with RAD?

Thanks again for your continued help.
HVSmith

RE: Radiosity Solver and RSURF

Check out my previous thread on Ambient Radiation: thread569-298500: Radiation to Ambient... third post in has an example of radiation to ambient. The SF/SFE command is not required; you simply need to apply SURF152 elements which are tied to a "space node" with the proper keyopts and real constants to the surfaces radiating to ambient.

Convective coefficients can also be applied, but that does, in fact, require the SF/SFE command (also discussed in the aforementioned thread).

RE: Radiosity Solver and RSURF

(OP)
Hi - yes, I had read that a few times (and have read it many times again since) but I'm still having trouble - are you able to offer any further advice to my questions below?


Here's a small section of the code, relating to the radiation:

!----------------------------
!DEFINE ELEMENT TYPES
!----------------------------  

ET,1,SHELL131            !THERMAL SHELL
KEYOPT,1,3,2
KEYOPT,1,4,1
R,1                    !REAL CONSTANT
SECTYPE,1,SHELL
SECDATA,1E-6,1

!----------------------------
!GEOMETRY AND MESH
!----------------------------
BLC4,-L/2,-L/2,L,L          !FOIL GEOMETRY
AESIZE,ALL,L/20            !MESS FOIL GRID 20X20    
AMESH,ALL

ASEL,S,AREA,,1
ESLA,S
NSLA,S,1
CM,FOIL,NODE
CM,FOIL_E,ELEM
IC,FOIL,ALL,300
ALLSEL

!----------------------------
!RADIATION EFFECTS
!----------------------------

ET,2,SURF152    !CREATE SURFACE ELEMENT FOR RADIATION TO AMBIENT
KEYOPT,2,5,1    !KEYOPT TO HAVE ONE EXTRA NODE (SPACE NODE)
KEYOPT,2,9,1    !KEYOPT TO USE DEFAULT (1) FORM FACTOR
R,2,1,5.67E-8    !REAL CONSTANTS FOR ET 2
ESURF        !APPLY SURF152 TO SELECTED AREAS OF SHELL131
N,5000,1000,1000,1000         !CREATE AN EXTRA NODE FAR AWAY
NSEL,S,NODE,,5000,5000        !SELECT NODE
ESURF,5000    !CREATE SURFACE ELEMENTS FOR EXTRA NODE    
D,5000,TEMP,300            !SET TEMPERATURE OF EXTRA NODE



(I attach a macro file to this post too, incase that is easier).

I keep getting the error "The active element type cannot use and extra node.  The ESURF command is ignored".  

I have searched for a solution to this for a long time - do you know what the problem may be?

In many ANSYS documents regarding this subject it says "simply overlay the surface effect elements" - this hasn't been this simple for me - I think this is where I'm going wrong?

Is this all that is required for radiation to ambient then?  This is quite surprising to me - my last efforts (looking at surface-surface radiation) seemed more intuitive to me (using the radiosity solver) - maybe I'm missing something?

And ideally I'd like to have radiation from both sides of my thin plate - but from extra reading it seems this is only possible on one side if using a shell?  Is there anyway to get around this (like reversing normals?)?

Thanks again for any help/advice you are able to give - it really is very much appreciated.

HVSmith




PS,
I was unable to open the .wbpz file attached to your post in the other thread.   

RE: Radiosity Solver and RSURF

Why do you issue ESURF twice? I think you want to delete the first one. If you're working in APDL you should be able to see the elements when they're created (esel,s,ename,,surf152) just to make sure that it was done correctly. I'd step through the commands one-by-one so you can confirm that they're doing what you think that they should do.

I'm also not seeing where you're selecting the nodes that you'd like to apply the surface effect elements to... or your emissivity. I'd think that you'd want that last part to look something like this:

CODE

!----------------------------
!RADIATION EFFECTS
!----------------------------

ET,     2,SURF152   !CREATE SURFACE ELEMENT FOR RADIATION TO AMBIENT
MP,EMIS,2,0.15      !SET EMISSIVITY
KEYOPT, 2,5,1       !KEYOPT TO HAVE ONE EXTRA NODE (SPACE NODE)
KEYOPT, 2,9,1       !KEYOPT TO USE DEFAULT (1) FORM FACTOR
R,      2,1,5.67E-8 !REAL CONSTANTS FOR ET 2

N,5000,1000,1000,1000   !CREATE AN EXTRA NODE FAR AWAY

NSEL, S,NODE,,5000,5000 !SELECT NODE
CMSEL,A,FOIL            !SELECT DESIRED SURFACE (NODES)

TYPE,2                  !SET ELEMENT TYPE
REAL,2                  !SET REAL CONSTANT SET
MAT, 2                  !SET MATERIAL

ESURF,5000              !CREATE SURF152's ATTACHED TO SPACE NODE (5000)
D,5000,TEMP,300         !SET TEMPERATURE OF EXTRA NODE

Warning: I didn't test any of the above code; no substitutions, exchanges or refunds.

RE: Radiosity Solver and RSURF

(OP)
OK, so I was misunderstood...I was calling ESURF twice as I thought I was initially creating the surf152 on top of the shell131 I had and then later on the extra node I created.  

This has now been corrected in the code.

With only the latter ESURF command I see that it is indeed creating the extra element.  However, this then throws up errors such as:

 *** ERROR ***                           CP =      33.828   TIME= 16:04:22
 Radiation element 401 has zero or negative absolute temperature.  The   
 offset temperature (TOFFST) and/or the uniform temperature (TUNIF)      
 must be positive.                                                       

The same message is also displayed about radiation element 421.
This is odd.  I'm not really sure what the problem is?  I thought I had already defined initial temperatures and the temperature of the space node...

None the less, I tried to fix this with

ESEL,ALL
IC,ALL,TEMP,300
       
after giving the ESURF command and setting the temperature of the space node, but this still doesn't help - I then get errors of "The value of TEMP at node 261 is 90168629.7 which is greater than the current limit of 1000000.  This generally indicates rigid body motion as a result of an unconstrained model.  Verify that your model is properly constrained."

I'm working in Kelvin, so the temperature offset is not required, as far as I am aware.

So something is going very wrong somewhere...

Is the problem obvious/trivial?  
Do I actively have to allow radiation in /SOLU or is this implicit from the creation of surf152's?

Thanks again for any help, it's very much appreciated, this is definitely a steep learning curve for me...

HVSmith
                                            
 

RE: Radiosity Solver and RSURF

Apart from the radiation, what are your other boundary conditions?

RE: Radiosity Solver and RSURF

Make sure your model runs and gives the expected results before applying radiation.

RE: Radiosity Solver and RSURF

(OP)
Um, as in what other constraints I've put on the model?

I apply pulsed heating and then cool by radiation.
There is conduction in the plane.
I set an initial condition of 300K for everything.

(The pulsed heating is described by a Gaussian function).

Is this what you mean by boundary conditions?  Or should I be applying other constraints since this is a radiation dominated cooling effect?

Thanks
HVSmith  

PS, macro file attached in case what I've said isn't clear

RE: Radiosity Solver and RSURF

(OP)
Yes, without radiation the heat just continues to increase, as I think I would expect.

I've tried implementing radiation from both sides of the plate before in many ways, using RDSF seems to work, but I can't help but feeling it's not true, since there is no other surface to radiate towards.  But the results are roughly similar to a numerical solution I have.

Hopefully I'll be able get this SURF152 working and it should be a more accurate representation and closer match to the numerical model.   

RE: Radiosity Solver and RSURF

I'd test the script on a well-posed steady-state problem before moving on to a transient problem... fewer things to go wrong there. Also, perhaps a TOFFST,0 wouldn't hurt anything. The radiation end of things seems correct.

I apologize, I'm not able to run your script at the moment because I've got a few things in the cue. I am a bit suspicious of the volumetric heat input...

RE: Radiosity Solver and RSURF

(OP)
OK, simple mistake on my part I'm afraid.  I was counting elements (required for my Gaussian do-loop) after creating the SURF152, but this needs to be done before, otherwise temperatures go hay-wire.

I've included a TOFFST,0 as you suggested, for completeness, it can't harm as you say.

The volumetric heat input was calculated at the very beginning of the project.  I've been through it again since you remarked upon it and all the numbers seem fine to me and give reasonable temperature results (at least in the expected ball-park).

However, the results obtained using SURF152 are somewhat different to those when I use the radiosity solver method to apply RSURF's to either or both sides of my shell element, results summarised as follows:

SURF152:
Time 0.9805s, Temp 2597K
Time 1s, Temp 771K

RDSF (2 sides):
Time 0.9805s, Temp 2490K
Time 1s, Temp 613K

RDSF (1 side):
Time 0.9805s, Temp 2618K
Time 1s, Temp 785K


All of these numbers are in the right ball-park (I have a separate numerical solver that I'm benchmarking against which has T~2350K at 0.9805s and T~800K at 1s).

I'm still confused as to which method (RDSF or SURF152) to actually use.  

I also need to convince myself that the SURF152 is actually working correctly.  Do you have to do anything to "call" the radiation into action, or is it just going to happen given the prescence of the SURF152?  

The numerical analysis I have assumes heat radiating from both sides - from what I understand SURF152 can only be applied to one load-key of a shell, is this correct?  I've tried moving the space-node around (+/- in the z direction) seeing if this makes any difference but as far as I can see it does not.  Do you have any suggestion for a way to implement radiation from both sides via the SURF152 route, or similar?

Thanks again for your help - really useful to get feedback from folks on this :)

HVSmith
PS, most current macro attached if required

RE: Radiosity Solver and RSURF

(OP)
Hi - again!

I tried to check that the SURF152 radiation implementation was working by doing a test without any radiation defined at all, and, as expected the temperature just continued to rise.  

However, I am still struggling to decide why the results of the SURF152 and Radiosity Solver method are inconsistent.  I attach some .jpeg images of the final results so you can see.  My gut instinct says that SURF152 is the way forward.  

I've also still been struggling to find a way to implement SURF15s on both sides of my 3D shell - do you happen to know if there are any work-arounds for this?

Thanks again for your recommendations/suggestions
HVSmith

RE: Radiosity Solver and RSURF

It's not surprising that the two different (numerical) radiation solvers end up with slightly different results. You might try tightening your convergence criteria to match the two results more closely.

I'd imagine that your SURF152s will solve much faster, since the Radiosity solver is trying to calculate view factors.

To complicate things further, there is a third radiation solver, the AUX12 radiation matrix method (which is supposed to be more accurate than the Radiosity solver, though more computationally expensive). I think that SURF152 elements are probably most appropriate for your problem as well, since you're only radiating to space.

I believe the RADOPT command adjusts the convergence criteria for the Radiosity solver, whereas (I think) the CNVTOL command sets the convergence tolerance for SURF152 elements.

Also... a quick tip: When comparing results it's a good idea to match scales to get a better idea of what's going on.

RE: Radiosity Solver and RSURF

(OP)
Thanks for your comments, it's been really helpful to get your take on things.  I will certainly look into matching the scales.

Are you able to add any comment/suggestion as to how I can extend the SURF152 elements to look at radiation from both load-keys of the underlying 3D shell?

From what I've read they can only be applied to one load-key, but in reality radiation will occur from both, so is there a way to model this?  Or is it a limitation that I should just be aware of?

Thanks again
HVSmith

RE: Radiosity Solver and RSURF

Do you mean that you want to capture the effects of through-thickness temperature variation by tying two sets of SURF152 elements to TTOP and TBOT, rather than the TEMP DOF?

I think that there is a section of the thermal analysis guide that discusses doing just that, actually (though I haven't tried using through-thickness temperature variations in shell elements). Check section 2.4.1 of the thermal analysis guide. I think you'll want to create two sets of SURF152 elements (one for each side). I believe that you can set KEYOPT(11)=1 to tie the SURF152 elements to the TTOP DOF or KEYOPT(11) to tie them to the TBOT DOF. So... you should be able to set different (space node) temperatures on opposite sides of your foil, if desired... I think.

Here's a link to the documentation: http://www1.ansys.com/customer/content/documentation/130/ans_the.pdf

RE: Radiosity Solver and RSURF

(OP)
Hi - thanks - yes, that's exactly what I wanted to do, converted into ANSYS speak, thanks very much!  I'll give it a go!

HVSmith

RE: Radiosity Solver and RSURF

(OP)
So, I gave that a try and read the section of the manual you suggested.  It all made sense in my head, then as soon as I transferred it to ANSYS the errors began...

I worked my way through them and now only have one (stubborn one) remaining:

 *** ERROR ***                           CP =     838.766   TIME= 16:56:51
 Radiation element 401 has zero or negative absolute temperature.  The   
 offset temperature (TOFFST) and/or the uniform temperature (TUNIF)      
 must be positive.                                                       

 *** ERROR ***                           CP =     838.766   TIME= 16:56:51
 Radiation element 801 has zero or negative absolute temperature.  The   
 offset temperature (TOFFST) and/or the uniform temperature (TUNIF)      
 must be positive.    


This is similar to an error I posted above that miraculously went away with an ESEL,ALL followed by IC,ALL,TEMP,300 but unfortunately this didn't seem to solve the problem this time.

I tried to see what the radiation element 401 and 801 were and from going through line by line and analysing the output I think they are the surf152 on the extra nodes.  

I've tried swapping TBOT/TTOP and +/- z for the extra node but nothing seems to do the trick.

If I set TOFFST,300 then the solution works and the numbers seem reasonable.  But everything else I'm doing is in K, so TOFFST should be 0, right?  This has massively confused me.  I don't want to start adding in TOFFST,300 in when it is already in K and TOFFST,0 works fine when I use KEYOPT(3)=2 on SHELL131, so no through thickness.

Is there something obvious I'm missing?!

CODE

ET,2,SURF152
MP,EMIS,2,0.8
KEYOPT,2,5,1
KEYOPT,2,9,1
KEYOPT,2,11,2
R,2,1,5.678e-8

N,10000,0,0,-0.1

NSEL,S,NODE,,10000,10000
CMSEL,A,FOIL

TYPE,2
REAL,2
MAT,2

TOFFST,0

ESURF,10000
D,10000,TEMP,300

ESEL,ALL
IC,ALL,TEMP,300



ET,3,SURF152
MP,EMIS,3,0.8
KEYOPT,3,5,1
KEYOPT,3,9,1
KEYOPT,3,11,1
R,3,1,5.678e-8

N,20000,0,0,0.1

NSEL,S,NODE,,20000,20000
CMSEL,A,FOIL

TYPE,3
REAL,3
MAT,3

TOFFST,0

ESURF,20000
D,20000,TEMP,300

ESEL,ALL
IC,ALL,TEMP,300


So, as far as I can tell, the TOFFST,0 is OK (in my opinion) and the TUNIF is >0 since I have the IC,ALL,TEMO,300, no?

Thanks again!
HVSmith
 

RE: Radiosity Solver and RSURF

Did you successfully run your previous model changing only KEYOPT(11) to "1" or "2"?

RE: Radiosity Solver and RSURF

(OP)
Yes, changing to KEYOPT(11) = 1 or 2 and applying only a single SURF152 works absolutely fine, no problems.  

It's only when I try to make two SURF152's (one for the top and one for the bottom) that I encounter the problem described in my post on the 10th of August.

I have still not found a method in which I can successfully apply SURF152 to the top layer and a separate SURF152 to the bottom layer without seeing the error.

Thanks for any ideas you may have!
HVSmith

RE: Radiosity Solver and RSURF

(OP)
Apologies - the above is incorrect...

KEYOPT(11) = 2   ---->  and apply a single SURF152 works OK

KEYOPT(11) = 1   ---->  and apply a single SURF152 does not work...
Errors are present for radiation elements 421 and 401 (error as described in post from 10th August)

And the errors are still present when I try to apply SURF152 to both sides.

I'm really confused.  

I must be doing something really wrong.  I think it might be to do with the way I'm defining the amount of layers now?

I used to make a SHELL131 act as a SHELL57, but now to get the TTOP and TBOT as you suggest I must change they KEYOPTS to allow temperature variation through the layer.

CODE

ET,1,SHELL131                        !THERMAL SHELL
KEYOPT,1,3,1                        !LINEAR TEMPERATURE VARIATION THROUGH LAYER

I used to define KEYOPT(4) to be equal to the amount of layers, which is equal to those in SECDATA, this is what I used to have:
 

CODE

KEYOPT,1,4,1                        !NUMBER OF LAYERS (EQUAL TO SECDATA)    
R,1                             !REAL CONSTANT
SECTYPE,1,SHELL
SECDATA,1E-6,1

So now, because I don't just want one layer, I'd have to change these keyopts to reflect this, in some way?  I have tried KEYOPT,1,4,2 to try and give me a top and a bottom layer?  But then I'm not sure what to put in SECDATA, do I have to define the thickness of the further sections?

I've tried very many things over the past days, but nothing is working.

Any further insight appreciated, many thanks, most recent macro file attached (with many lines commented out) if it's more useful to view this way...
HVSmith

RE: Radiosity Solver and RSURF

It seems like it's having trouble attaching to the TTOP DOF. I wish I could help more, but I haven't really used the layered shell feature before. I think that you're looking at the SECDATA is the right direction.

Worst case, you can always put in a ticket with ANSYS.

RE: Radiosity Solver and RSURF

Post back with your results when you get it figured out; I'd be interested in knowing where the trouble stems from.

RE: Radiosity Solver and RSURF

(OP)
OK, so I have spent some time talking to ANSYS about this - their advice is to revert to using SFE RAD command on both load keys rather than SURF152s at all - how confusing!
I'll give this another go and see if anything different happens this time...

Thanks again for all of your input - hope these discussions may shed some light for others out there too...!
 

RE: Radiosity Solver and RSURF

(OP)
OK, so I convinced the guys at ANSYS that SFE,RAD wasn't working at all, they agree and apparently this is being fixed fo v14.0.  

Instead of applying SURF152 to TTOP and TBOT, the same result can be obtained by using 2xSURF152's on the TEMP DOF - I'm not sure if this is just because I have such a thin thickness or also true in the general case.  But they assure me this is fine for the above purpose, and is effectively radiation twice, so once from each surface.  The answer it gives is also reasonable.  

The other point I should make is that TOFFST should always be > 0.  I guess this depends on how you define 0 as being +ve/-ve etc.  I was under the impression TOFFST,0 would allow me to work in absolute temperature units (K).  Apparently not.  A value > 0 is required.  I could have changed all my values to work with TOFFST,273 and work in degC, but instead I chose to use TOFFST,0.00001 so it is > 0 but only slightly (!), so the effect on the results is negligible...

Hopefully these tips will help someone else out there in the future!

RE: Radiosity Solver and RSURF

Thanks for posting back. I'd imagine that a thin sheet or foil would work fine by tying both sets of SURF152 elements to the TEMP DOF, which is simply the temperature at the midplane. If you were dealing with something thicker, you may be stuck using solid elements to achieve an accurate result.

That's an interesting limitation on the TOFFST command (must be greater than zero); I'll file that away in my brain.

Glad to hear that your model seems to be working for you. Best of luck.

//signed//
Christopher K. Hubley
Mechanical Engineer
Sunpower Incorporated
Athens, Ohio

RE: Radiosity Solver and RSURF

Hello everybody,

I am quite new to the this radiation method(s) in Ansys and hence have some question to you guys...

1) In one of the post earlier, HVSmith mentioned that results of surf152 and different from Radiosity solver method. I could not understand what is the different in these methods.
Please correct me if I am wrong in my understanding about these methods-
Surf152 method: Here you solve radiation between surf152 element (pasted over other surface of a component) and an ambient nodal point such that the view-factor is always 1. Hence no separate calculation is required to calculate view-factor. Here do we need to assign RAD or RDSF tag on these surf152 elements using SFE command?


Radiosiy Method: Used to compute radiation between two surfaces. Here again, I think we need to create surf152 (or surf252? What is the difference?) over these surfaces, specify RDSF tag using SFE, specify TOFFSET, HEMIOPT setting. Now Ansys computes the viewfactor between these surfaces. Also, if the total viewfactor from a surface is less than 1, the remaining viewfactor is assigned to ambient with the ambient temperature specified (Thats why Ansys Mechanical - R13 GUI panel requires ambient temperature in the radiation command even if surface to surface radiation is selected).

Please confirm if my understanding is correct.
Also some additional queries -

1) When we can create surf152 using ESURF and use RAD or RDSF flage on Surf152 using SFE, why do we also have RSURF to create SURF252?
2) What is different between RAD and RDSF? I believe former is only for ambient radiation (Viewfactor always = 1), while latter is for surface-to-surface ( and ambient if Viewfactor < 1)
3) When surf-to-surf radiation for closed chamber is modeled through APDL commands, do we need to use SPCNOD and SPCTEMP? Also are surf152 enough to model this radiation using SFE,..RDSF flag?
And is this how the Radiation object (inserted in GUI panel of Ansys MEchanical 13 for surface-to-surface radiation) works?

Excuse me for sooo many questions, but I am stuck in radiation and any help will be highly appreciated.

Regards,
Shreesh

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources