急求帮助！！怎样进行交变生热率作用下的温度场分析！！
各位版上的牛人们，我主要是想分析一下图中的金线(模型为工字型为金线，下面为硅基)，在交流电作用下的温度分布，及温度随时间的变化。不知道这个交变的生热率应该如何同时间相关的添加到金线上。希望大家能够给我提供帮助。不胜感激。http://home.simwe.com/attachment/201009/7/465478_1283827207p4DI.jpg 自己先帮自己顶一下！！！！ Hehe, correct me if I am wrong - your model is for 3-omega thermal conductivity measurement, where you want to look at the averaged harmonic temperature over the heater to extract the thermal conductivity of the under-earth thin film or substrate.
There are three ways to do get the solution:
(1) 2D or 3D analytical solution - Just to solve the 2/3D heat conduction heat conduction problem subjected to surface heat flux conditions in frequency-domain, where the temperature is a complex number.
(2) Write you own finite volume model where you substitute real temperature to the complex temperature which convert the problem from transient to quasi-steady state problem.
(3) In Ansys you can use the harmonic thermal analysis where you only need to input the amplitude and frequency of the heat flux, the temperature will be complex number too, which represent the amplitude and phase (ANSYS help doesn't list the harmonic thermal analysis capability but it does work).
I have done all three approaches before and I would recommend (1)>(3)>(2) 谢谢您，麻烦您可不可以帮我把添加生热率的这个部分写几句命令呀？我是新手，不大会用ansys做热分析，麻烦您了！！！ 3# iomega 4# bulabula iomega的英语是牛了一点。。。感觉是不是可以采用第三种方法会比较好点，只要给出振幅和频率，ansys就会生成谐振的热生成率。听起来蛮符合楼主的要求的，只是该如何施加。。。。只能楼主查资料了。。。 也看了几本书，就是没找到有这种加载方式的，版上的兄弟姐们能不能推荐两本书呀？ 5# webcam 本帖最后由 iomega 于 2010-9-7 20:54 编辑
I raised this question long time ago in below post but nobody answered it so I have to figured it out by myself.
http://forum.simwe.com/viewthread.php?tid=257772&highlight=%2Biomega
For method (1), you can look at my previous post on Mathcad board, where I already gave the source code of analytical solution in mathcad file:
http://forum.simwe.com/viewthread.php?tid=819280&highlight=%2Biomega
For method (2), just refer to Patankar's famous book of numerical heat transfer simulation, assuming the T(x,y,z,t) is in the form of T(x,y,z,omega)*exp(i*omega*t+ phase), then the transient problem becomes steady-state problem.
For method (3), below is an example of a suspended metal bridge with two-sides kept at T0, subjected to a heat generation of Q*sin(omega*t), where omega is the heating frequency and Q is the amplitude. The heating frequency is 100 Hz in this example.
FINISH! Make sure we are at BEGIN level
/Clear
/PREP7
/PNUM,VOLU,1
/NUMBER,1
/PNUM,MAT,1
/REPLOT
k=90
DEN=3900
Cp=420
/PREP7
um=1e-6
L=20*um
W=2*um
T=2*um
T0=0
Size=0.25*um
ET,1,SOLID70
UIMP,1,DENS, , ,DEN,
UIMP,1,KXX,KYY,KZZ,k,k,k,
UIMP,1,C, , ,Cp,
BLC4, 0, 0, W, L, T
aesize,all,Size,
TYPE,1
MAT,1
mshkey,1
mshape,0,3d
vmesh,1
/SOLU
ANTYPE,HARMIC
HROPT,FULL
OUTRES,ALL,ALL
tunif,T0
TREF,T0
asel,s,LOC,y,0,0
asel,a,LOC,y,L,L
DA,all,TEMP,T0
allsel,all
nsel,all
BF,ALL,HGEN,1e14
allsel,all
HARFRQ,100,
SOLVE
After the solution is done, you have to read the results: set 1 is the real part and set 2 is imaginary part. They together form the complex temperature rise from which you can easily obtain the amplitude and phase delay.
BTW, bulabula,you are coming from engineering mechanics department, right? Is your boss Liang? Just curious... 非常感谢，我是学工程力学的，呵呵，不过老板不是姓liang。 engineering mechanics department has three majors:
solid mechanics, fluid mechanics and thermophysics. Are you from thermophysics?
8# bulabula 我是学习固体力学的，只是我的文章中有一小部分要进行热的计算，你是哪里呀？怎么都用英文呀？ 9# iomega So you are from 力xx. I have lots of friends from solid mechanics area in your department.
10# bulabula ANSYS不是再带载荷编辑器吗，可以生成热载荷函数，再调用就行了。 Think twice before you post something...
If you want to run it in time-domain, you have to use small enough time steps in order to capture the exact response of the system.You have to use the time step at least twice of the bandwidth of the thermal transfer function of the system.
One prerequisite of harmonic analysis is that it should be a linear system.
12# xiaohutu186
页:
[1]