Question about ANSYS' TREF command
Juan Ernesto Salazar
I'm a last year mechanical engineering student and this message has the
intention of asking your help to clarify the matter of the use of
reference temperatures (TREF) in a thermal stress analysis of a
composite body using ANSYS 5.1. Solving this matter is of great
importance to me since it is an essential part of a project that
requires to be finished in order to move on to my degree thesis. The
problem is as follows.
The thermo-mechanical stress during the assembly of a cathode bottom
block
of an aluminum reduction cell needs to be determined. The practice
involves connecting a steel bar into the slot of a carbon block by
pouring
gray cast iron in the space between them. This is usually called
cathode
rodding and in order to achieve it the following procedure must be
carried
on:
1. Preheating of the carbon cathode block to a 400 °C temperature.
2. Preheating of the steel bar to a 550 °C temperature.
3. Pouring of gray cast iron at a 1480 °C temperature.
Steps 1 and 2 must be done simultaneously and step 3 immediately
after.
I have tried to solve the problem of determining the stress developed in
the different materials at the very same moment of pouring the cast iron
by
the means of a static analysis. The model is described next,
-3D model made of 4 different volumes (different materials for e/a) all
glued together.
-Meshed with SOLID45 tetrahedral elements (3747 elements, 907 nodes).
The boundary conditions are the temperatures described before, applied
as
body loads on all nodes for each volume and own weight. The block is
simply supported and symmetry conditions were taken into account (only
1/4
of the assembly was modeled). Pictures of the model are available for
those of you who want to take a look.
An uniform temperature (TUNIF) of 30 °C was also considered and the
reference temperature (TREF) was set at 400 °C. At this point doubt
arises
on the assignment of this reference temperature since ANSYS manuals
state
that this reference temperature is the strain-free temperature for a
particular body but make no reference for the case of a composite.
Even more doubt comes along with the fact that results are extremely
higher
than expected (about 10 times). For example, the results for the carbon
cathode block show that the stress at most points of the block is
greatly
higher than either the tensile, compressive or flexural strength of the
material. This is not an actual fact, since experimental conditions
show
that stresses of this magnitude are not reached all over the block but
only
in a few critical points.
Because of all of the above, I would like to know whether there is a
need
to take any special consideration with regard to the reference
temperature
(TREF) or the approximation taken is wrong in any way.
Any comments on the subjects discussed before would be greatly
appreciated. Please reply both by e-mail and to the newsgroup. Thanks
in advance,
jesp99
Martin Liddle
<je...@viptel.com> writes
you just doing a single thermal stress solution? My approach would be
to do a thermal transient analysis to model the heating up and cooling
down following the pouring of the cast iron and then do a series of
thermal stress runs to calculate the variation of the stresses with
time. I agree that the cathode block and steel bar will start stress
free and at different temperatures. Your version of ANSYS (5.1) is
rather old. The current version 5.5.1 allows different materials to
have different reference temperatures using the MP,REFT command: I can't
remember whether this is present in 5.1.
--
Martin Liddle, Tynemouth Computer Services, 27 Garforth Close,
Cramlington, Northumberland, England, NE23 6EW.
Phone and fax: 01670-712624.
Juan Ernesto Salazar
1. Static thermo-mechanical analysis using six different load
conditions in order to get an idea of the magnitude of stress and deformation
at pouring time for these different conditions (combinations of preheating
temperatures for the carbon block and steel bar keeping the gray cast
iron temperature constant).
2. Transient thermal analysis to get the temperature distribution over
time in the assembly. Then, thermal stress analysis for selected load
steps.
The problem was divided in two stages just for academical purposes.
The first stage is intended to help me choose the initial conditions
for the transient analysis.
In fact, previous runs (transient ones) have proved that peak stresses are
reached some minutes after pouring the cast iron (on some particular
points of the block), so I guessed that I could first get a slight idea about
running time and the value of stress from a static type of analysis, and at
the same time evaluating how the assembly reacts to the changes in load
conditions.
At the time, I'm not able to look if ANSYS 5.1 has the MP,REFT option.
However, I do have ANSYS/ED 5.3 at home an it seems to have this option
available.
Well, it's been a real pleasure receiving your comments about this
problem. I'll check for the MP,REFT in ANSYS 5.1. For the mean time
I believe some of my doubts have been cleared.
Thaks a lot,
Juan Ernesto Salazar
Mechanical Engineering Department
"Antonio Jose de Sucre" Polytechnical University (UNEXPO)
Puerto Ordaz, Bolivar 8015
Venezuela
Tel: +5816 6870665
Daniel Richard
if I may ask a few "academic" questions :
1) are you using linear elastic properties for carbon ? If so, you have to
know that it is totally untrue for most grades of commercial cathodes
(amorphous or semi-graphitized). Even worse if your properties are
temperature independant.
Look at
Michard,L. ,"Modelling of the Sealing of Cathode Bars into Carbon Blocks",
TMS Light Metals 1986, 1986, p.699-704
who proved that he could not predict cathode failures with this kind of
model. However, they did have great qualitative success. However, this might
be exactly what you are looking for, and it is quite OK for studying sealing
parameters of a smelter.
A hint : to really be able to predict cracks in cathodes, you need a
transient mechanical run with the proper constitutive model, even if the
problem could be considered as quasi-static.
2) In the transient run, did you take in account cast iron solidification ?
Again, look at Michard's article, they did a great job on the thermal model.
3) Tetrahedral linear elements (like SOLID45) are not good in high stresses
region. If you know a little about FE, it is because the gradients of the
degree of freedom are constant over the element. You might want to use
linear bricks at least, and preferably quadratic elements...
4) You need to input thermal expansion curves that are temperature dependant
to get a good solution...
5) Use TREF as being the stress free initial temperature of each body, since
ANSYS uses (T-TREF) as the temperature difference causing expansion. ANSYS
allows that in recent versions.
6) TUNIF sets that temperature to nodes without imposed temperatures in a
mechanical run ... I would not use that command...
Hope this helps,
Daniel Richard
--
==================================================
Daniel Richard,Ing.Stag. Daniel Richard,Jr.Eng.
Candidat au M.Sc. M.Sc. Student
Génie Chimique/GIREF Chemical Engineering/GIREF
Université Laval Laval University
Pavillon Pouliot Pouliot Building
Ste-Foy, Québec Ste-Foy, Québec
Canada Canada
G1K 7P4 G1K 7P4
=================================================
Bureau: PLT-1566 Office: PLT-1566
Tel: (418)656-2131, x6224 Phone: (418) 656-2131, x6224
dric...@gch.ulaval.ca dric...@gch.ulaval.ca
=================================================
Juan Ernesto Salazar <je...@viptel.com> wrote in message
news:374855F1...@viptel.com...
> For all of you dear ANSYS gurus out there:
>
> I'm a last year mechanical engineering student and this message has the
> intention of asking your help to clarify the matter of the use of
> reference temperatures (TREF) in a thermal stress analysis of a
> composite body using ANSYS 5.1. Solving this matter is of great
> importance to me since it is an essential part of a project that
> requires to be finished in order to move on to my degree thesis. The
> jesp99
>
Juan Ernesto Salazar
my reply message to Martin Liddle in the newsgroup. Anyway, here's what
I wrote him and a little bit more.
The problem is being approached two ways:
1. Static thermo-mechanical analysis using six different load
conditions in order to get an idea of the magnitude of stress and
deformation at pouring time for these different conditions (combinations
of preheating temperatures for the carbon block and steel bar keeping
the gray cast iron temperature constant).
2. Transient thermal analysis to get the temperature distribution over
time in the assembly. Then, non-linear steady-state stress analysis for
selected load steps.
The problem was divided in two stages just for academical purposes.
The first stage is intended to help me choose the initial conditions
for the transient analysis.
In fact, previous runs (by J. Bos et. al. and Michard) have proved that
peak stresses are reached some minutes after pouring the cast iron (on
some particular points of the block), so I guessed that I could first
get a slight idea about running time and the value of stress from a
static type of analysis, and at the same time evaluating how the
assembly reacts to the changes in load conditions for that very same
moment. This is a qualitative approach, since the non-linear behavior
of the materials was not taken into account and besides, values obtained
are way too high (What do you have to say about this?)
That first stage was indeed a linear approach. The
temperature-dependant
properties of the semi-graphitic cathode block being analyzed are
available from previous measurements and they're used for the transient
run.
I'm using ANSYS 5.1 and I was forced to use SOLID45 tetrahedra because
the program wouldn't aloud the brick or quad shape of the element for
meshing the assembly's geometry. This has happened to me before when
modeling the anode-stub contact of a pre-baked anode using ANSYS 5.3. I
let it go that time because of the irregular shape of this contact, but
I'm not really sure how much of an error it introduces to the results
this time (I'm not very familiar with FE Theory, I'm just a beginning
user).
The latent heat of cast iron was neglected, I know this modifies the
heat capacity of the material but then again I don't know how great the
error might be. I'm aware Michard used it and so did J. Bos et. al.
("Numerical Simulation, Tools to Design and Optimize Smelting
Technology" TMS Light Metals 1998, pp 393-401), but as long as the
results show the tendency on the answer of the system to the change of
the different variables involved (operating parameters) I think I would
be able to come up with some partial conclusions and recommendations,
which is my main objective.
As Michard did I also neglected friction between cast iron and carbon.
When I get to conclusions I have to be careful to remember that the
effect of increasing friction is an increased shear fracture probability
while the highest tensile stress would be slightly reduced (Larsen and
Sorlie. "Stress Analysis of Cathode Bottom Blocks". TMS Light Metals
1989. pp 641-646). So the answer is using collector bars with smooth
surface and I wouldn't worry that much about that.
My original question about TREF came up with the reading of a rather old
(ANSYS 5.0) manual that didn't say anything about using this parameter
in composite bodies. When I made the first static runs I didn't use any
reference temperature at all and then I made a run using only one TREF,
which was obviously wrong. Now I think this is one of the reasons I got
such high results.
Well, it's been a real pleasure receiving your comments about this
problem, they have been very useful. I think I have pretty much
described the work I'm trying to perform. If you see anything wrong,
feel free to send me your comments, they will be much appreciated since
this project needs to be finished if I want to go on to my degree
thesis. Thanks a lot for your time.
Regards,
Juan Ernesto Salazar
Undergraduate Student
Mechanical Engineering Department
"Antonio Jose de Sucre" Polytechnical University (UNEXPO)
Puerto Ordaz, Bolivar 8015
Venezuela
Tel: +5816 6870665
e-mail: je...@viptel.com jua...@hotmail.com
Daniel Richard
nice to discuss with you. I guess you are working with Venalum isn't ?
I did take a look at your reply to the others, and my comments are still
valid I think.
I am sending you a picture of a mesh of a stubhole I did as a mech eng
undergrad last year in ANSYS 5.3. It is all in bricks. I know it is not easy
to do, but it is possible. The thing with linear tets is that the gradient
of the degrees of freedom (displacements) is CONSTANT over the element, i.e.
your stresses are constant over the element (mechanical) and thermal flux is
constant over the element (thermal) ! In regions of high stresses, it gives
a very bad picture of the true stress distribution, especially with
shear-dominated problems (such as thermal stress) ; for thermal problems, in
regions of high thermal gradients, it also gives a bad picture of the
temperature distribution, especially if you are imposing thermal flux as a
boundary condition. I would recommend you work on your mesh to get bricks at
least (linear gradients!), or use quadratic tetrahedron (linear gradient!)
(mechanical SOLID92, thermal SOLID87). If you can't, refine A LOT the mesh
in the regions where you think stresses/thermal gradients are high. You
could do a mesh-sensitivity analysis (refine until solution does not change
significantly).
I suggest you ask for your ASD or a teacher or somebody competent for some
FE theory background ... it helps believe me ! You have to realise FE always
give you an APPROXIMATE solution, whose accuracy will strongly depend on the
mesh discretisation ...( An ANSYS advice : it should be really easy to brick
mesh a cathode geometry ... Do a 2D plane, mesh it with quad area elements,
then extrude in 3D with VDRAG or VEXT. )
> 2. Transient thermal analysis to get the temperature distribution over
> time in the assembly. Then, non-linear steady-state stress analysis for
> selected load steps.
> In fact, previous runs (by J. Bos et. al. and Michard) have proved that
> peak stresses are reached some minutes after pouring the cast iron (on
> some particular points of the block), so I guessed that I could first
> get a slight idea about running time and the value of stress from a
> static type of analysis, and at the same time evaluating how the
> assembly reacts to the changes in load conditions for that very same
> moment.
This is a good approach if you assume that the mechanical problem is
quasi-static ... which is NOT the case. Michard concluded that they could
not predict failure with this approach (1986 article). This is why I
suggested you do a transient thermo-mechanical run with suitable
constitutive equations....
> This is a qualitative approach, since the non-linear behavior
> of the materials was not taken into account and besides, values obtained
> are way too high (What do you have to say about this?)
This is absolutely right. Unless you consider that carbon is NOT linear
elastic, you won't get true stress values. Even worse with temperature
independant properties... It is indeed a qualitative approach, and for
comparison purposes, or for coupling with an extensive experimental campain
(like Michard & al. did), it is a good approach. However, if you want to
*predict* cathode failure at casting, you need to take in account these
nonlinear properties. Believe me, I gave that a lot of thought, since my
senior undergrad project was the modelling of the stub-to-carbon contact,
which is not at all that obvious, and has finally become my master's thesis.
The whole problem is to model the mechanical behaviour of carbon ! If you
have done a little litterature review, you should have come to the
conclusion that nobody was ever able to predict thermal shocks in anodes or
cathodes... take a look at Markus Meier "Cracking Behaviour of Anodes"
published by R&D Carbon, and take a close look at the apparatus he
developped for bending strength measurement - short span, high load rate -
and ask yourself why is is designed that way...
I think I gave you enough clues to figure out how carbon is really behaving
...
> The latent heat of cast iron was neglected, I know this modifies the
> heat capacity of the material but then again I don't know how great the
> error might be. I'm aware Michard used it and so did J. Bos et. al.
> ("Numerical Simulation, Tools to Design and Optimize Smelting
> Technology" TMS Light Metals 1998, pp 393-401), but as long as the
> results show the tendency on the answer of the system to the change of
> the different variables involved (operating parameters) I think I would
> be able to come up with some partial conclusions and recommendations,
> which is my main objective.
It influences a lot the temperature distribution in the transient run !
Remember that a cooling liquid entering the solidification phase reaches a
temperature "plateau" until solification is completed : this is the latent
heat of solidification effect. An ice cube in a glass of water melts slowly
because it needs to absorb the heat in the liquid to change from solid to
liquid phase. It is quite important to take that in account.
> As Michard did I also neglected friction between cast iron and carbon.
> When I get to conclusions I have to be careful to remember that the
> effect of increasing friction is an increased shear fracture probability
> while the highest tensile stress would be slightly reduced (Larsen and
> Sorlie. "Stress Analysis of Cathode Bottom Blocks". TMS Light Metals
> 1989. pp 641-646). So the answer is using collector bars with smooth
> surface and I wouldn't worry that much about that.
Good assumption, since graphite is "self-lubricating" (if you touched the
surface of a cathode you know what I mean !). It is not related to the
smoothness of the surfaces however.
Did you figure out with whom I am working with yet? :)
I am glad to see you are interested in aluminum-industry related
problems....
Hope this helps,
Daniel Richard
PS: By the way, would you speak French by any luck?