不同网格之间节温度场分析结果如何传递？
我想实现这样的功能：首先在一个实体上划分一个网格，进行温度场计算后，保存结果，然后再在相同的实体上划分另外一个不同的网格，并将前一个网格的温度计算值传递到这个网格上。是不是只需要传递单元节点的温度值就可以了？积分点的温度值还需要传递吗？[ 本帖最后由 后起之秀 于 2007-3-13 09:29 编辑 ] ANSYS has the function *MOPER to achieve such purpose. Here is an example:
Suppose first you calculate the temperature rise using free mesh, then you want to covert the temperature into a mapped mesh.
*MOPER,TINTRPC,TC,MAP,TDIST,NODLOCS,2,,1
NODLOCS saves the node coordinates of free mesh.
TDIST saves the node temperature of free mesh.
TC is the node coordinates of new mapped mesh.
After MOPER operation, TINTRPC will interpret the temperature from free mesh to mapped mesh.
原帖由 后起之秀 于 2007-3-13 09:27 发表
我想实现这样的功能：首先在一个实体上划分一个网格，进行温度场计算后，保存结果，然后再在相同的实体上划分另外一个不同的网格，并将前一个网格的温度计算值传递到这个网格上。是不是只需要传递单元节点的温度值 ... I am confused. You want to compute one model with two meshes. Let us assume Mesh I and Mesh II. You want to save the solution (degrees of freedom) from Mesh I. But when you use Mesh II, you don't compute anything, you just want to assign the nodal values of Mesh I to those ofMesh II. Am I right?
My question is: Do Mesh I and Mesh II have the same number of elements and the same order of the elements?
If Mesh I and Mesh II have the same type of elements and the same number of nodes, you are okay to save the nodal values only.
You don't need to save the values at the integration points. The values at the integration points are always calcuated by plugging the coordinate of integration points into the linear combination of degrees of freedom with the corresponding shape functions.
Could you tell us why you want to do this way? I just don't see your point. 原帖由 tonnyw 于 2007-3-13 13:16 发表
II am confused. You want to compute one model with two meshes. Let us assume Mesh I and Mesh II. You want to save the solution (degrees of freedom) from Mesh I. But when you use Mesh II, you don't compute anything, you just want to assign the nodal values of Mesh I to those ofMesh II. Am I right?
Yes, this is in case the second step calculation need Mesh II instead of Mesh I for further simulation. That's my guess from above question.
My question is: Do Mesh I and Mesh II have the same number of elements and the same order of the elements?
No, Mesh I and Mesh II don't need to have same amount of elements and order.
If Mesh I and Mesh II have the same type of elements and the same number of nodes, you are okay to save the nodal values only.
Mesh I and Mesh II could have different type of element and node numbers.*MOPER will take care of it - in real case it might be time consuming, since ANSYS need to do interpolation between two mesh sets.
You don't need to save the values at the integration points. The values at the integration points are always calcuated by plugging the coordinate of integration points into the linear combination of degrees of freedom with the corresponding shape functions.
Could you tell us why you want to do this way? I just don't see your point. 谢谢iomega版主和tonnyw:
我把我的课题背景和想法说一下：我研究的是焊接残余应力的模拟，焊缝区的网格比较细密，目前网格尺寸为1mm，焊件采用实体尺寸建模，以便于考察约束对残余应力的影响。所以，单元数和节点数较多。而且由于焊接时间和随后的冷却时间较长，时间步长又不能取得太大，导致求解时间过长，计算一个参数组合需要四五天，而且存储规模也较大。因此，我想实现移动网格划分功能。初始网格较粗，而只在热源附近划分较细的网格，该细网格可随着热源移动，网格的单元类型当然是一样的。因此存在将前一时间步的计算结果传递为后一时间步网格节点初始值的问题。目前网格的移动以及粗细网格节点之间的约束已经实现。由于粗网格在整个计算过程中不变，其计算结果可根据节点直接传递，而细网格节点的初始值须进行插值计算。我没有采用*MOPER,TINTRPC,TC,MAP,TDIST,NODLOCS,2,,1命令，因为当时没有弄懂TDIST,NODLOCS的组成格式，我想NODLOCS的每一行应是按节点编号的节点坐标值，TDIST应是对应节点相应的自由度值和导出量。对于我的方案采用*MOPER可能运算量较大。后来的计算结果较原始细网格网格偏高，而且计算时间反而长得多，我估计应是初始化时，由于热冲击使得计算不易于收敛，目前这个问题还没有得到解决，希望版主能否给点建议。若ansys支持非线性分析的自适应网格划分的话，我就没有必要费这样大的精力了。
[ 本帖最后由 后起之秀 于 2007-3-15 12:24 编辑 ] 厉害，值得学习
回复 #4 iomega 的帖子
看了一下帮助:*MOPER, ParR, Par1, Oper, Par2, Par3, kDim, --, kOutFor MAP,Par2 will be an {N(in) x M} array of values to be interpolated, where N(in) is the number of points to interpolate from, and M is the number of values at each point.
问一下:M是对应节点相应的自由度值和导出量吗?如果单元类型不一样,自由度值和导出量也会不一样,Par2 格式需要匹配吗?
斑竹能不能给一个简单例子说明一下,大家学习学习!
页:
[1]