Transient thermal analysis using ANSYS???

[poloniner]

Using ANSYS, I am trying to do an transient thermal analysis of a steel mold and molten alloy. The molten alloy(1800 F) is poured into the steel mold(1200 F) and is left to cool under natural convection at an ambient temp of 75 F. I need to determine how long it takes for the alloy to cool to the ambient temp. Please help.............

 

[corus]

I'd read up on heat transfer before attempting this. ANSYS, like most software companies, provide many manuals with examples in. You still need to know the theory though.

corus

 

[poloniner]

it's not that i don't know the theory behind it, well i don't(enough anyway), but i'm also a novice at using ansys.
let me be more specific on the problem.....
the steel molds o.d.=5", i.d.=3.5", and l=36", and the ingot resulting is a solid 3" diam, 36" long rod. i just need to find out how long it takes to cool to the ambient temp of 75F. i have found some similar tutorials but nothing that to do with finding the time to cool. i have even set the time-step to see if it cools down........nothing.
if anyone can help that would be great.......

 

[poloniner]

i meant the resulting ingot is a solid 3.5" diam.......

 

[corus]

You need to know the material properties of all the materials, including the latent heat. The problem appears to be predominantly axi-symmetric so a 2D model would do. Set the tinital temperatures to be 1800 and 1200 respectively and allow natural convection on the outer surface, then run the analysis for however long you want. Theoretically it would take an infinite amount of time to reach the ambient temperature. You need to define how close to ambient it takes to cool.

corus

 

[poloniner]

I understand what your saying, and I've done that already. Well, actually, I've tried to do it.
These are the steps that I used to input the data into ansys.

1. created the area(2D)
2. glue areas
3. input mat props
4. add element
5. mesh with mat props
6. loads on nodes - 1800F inner area
1200F outer area
.3 convection on outer line
7. create new analysis - transient
8. apply time step
9. solve

i've run the time step at different values and the temps are the same on the model

 

[Thane]

It sounds like you applied a temperature as a load instead of setting it as an initial condition.

If the temperatures are applied to the nodes as a load, then ANSYS will continuously apply the temperatures as a heat source instead of allowing the nodes to decrease in temperature.

Step 10 in the Thermal Tutorial gives a good description of how to apply the initial temperatures to a transient problem.

Hope this helps.

Thane

 

[poloniner]

Taking the advice from "thane" i have tried setting the temps as intitial conditions and ran the program. What the analysis it gives is confusing. The contour plot shows a uniform temp of 75....What the?? Seems as though the temperature entered using the intial conditions weren't even recognized. The solution went straight to ambient temp. I don't even see the existence of the 1800 and 1200 initial condition i applied.

 

[magicme]

hi there
without studying your ansys script, its really hard to know whats not working right.
but.....possibly this will help....below is a much-reduced version of a file i used to do something similar. it was a while ago, but i do remember an early issue similar to what you're seeing....after much hassle, this file worked fine....it had to do with how the BC's are applied after the TUNIF command.
the listing below is doing a transient on a component defined in ansys.....you need not have such a component defined....that part is not important to your issue.

i know its a pain reading other people's files, but...hey maybe its worth it.

regards,

daveleo

! ...............................................

! this will create the *thermal* step results that will
! later have to be read onto the structural database in steps
!
! in ANSYS, resume from the thermal database file
! then read in this file

/prep7

antype,trans,new

! delete existing loads

lsclear,all
ddele,all,all
sfedele,all,1,all
sfedele,all,2,all
bfdele,all,all

tref,75
tunif,130

! initial conditions on specific areas
! must come *after* the TUNIF command

! these IC's are the initial operating temperatures
! on the component uhexh (or whatever)

cmsel,s,uhexh
nsle
ic,all,temp,220.

allsel

! write IC's to a load step file
lswrite

/Title, Initial to final transient
/soln !Thermal transient solution
timint,on !Turn on transient effects
trnopt,full
time,3600 !Time at end of load step (seconds)
NSUBST,30 !Number of time substeps
KBC,1 !KBC=1 is step change
AUTOTS,OFF
outres,all,all
!
!...... temp and HTC variables..............

uhexhhtc=20
uhexhtemp=125

! select whatever components of the model and apply BC's
cmsel,s,uhexhcase1
cmsel,u,uhstrips
nsle
sf,all,conv,uhexhhtc/518400,uhexhtemp
! .............................................
allsel
lswrite

! then solve from load step files 1 and 2

 

[poloniner]

i have finally got it done. thank you all for your help.....i really appreciate it.