gmsh是个好东西，开源免费跨平台，容易上手同时功能强大。所有操作都能通过脚本完成，故易于自动化——脚本化到了GUI上某些功能不全的程度。

gmsh自带了一个不算简陋的造型系统，不过我还是习惯用Creo这类软件画图，导出成*.step格式（*igs格式在网格软件中的兼容性相当捉鸡），然后用gmsh的Open CASCADE模块导入之，再继续在gmsh中操作。这样做在做单个零件网格划分的时候是没问题的，但做多物理体仿真的时候，这么搞有可能出现零件界面上网格点不对齐的问题，尤其是在具有复杂形状的零件界面上。

两周之前我就遇到了这个问题，纠结了一整天。开始时以为gmsh不过是在界面上用了两个位置重合的网格点来分别表示两个零件，还试图自己写网格导入器去重复来着。后来去重复功能写成了，但是只在部分区域有用，因为其他位置的网格点实在是完全没有对齐。

无奈之下，只好去官方的邮件列表里面提问，运气很好，当试有高手很闲，直接就给详细回复了，解决了问题。昨晚发现又有人在提问同样的问题，看来这个问题对于新手实在不是很友好，有必要把这个贴子专门记录一下。

我当时以为官方邮件列表是不能贴图的，所以邮件列表提问的同时在`stackoverflow`贴图提问了。下面直接把[`stackoverflow`的帖子](https://stackoverflow.com/questions/47095493/any-way-to-make-gmsh-to-use-the-same-vertex-set-on-both-sides-of-a-material-boun)贴下来。

# Any way to make gmsh to use the same vertex set on both sides of a material boundary?

I am trying to mesh a complex geometry composed of 3 kinds of materials, like below:

The geometry is imported from a *.stp file.

I defined several physical surfaces and 3 physical domains in the geo file:

Physical Surface("air-case", 1) = {50, 42, 41, 40, 48};
Physical Surface("case-thermal", 2) = {32, 15, 22, 21, 25};
Physical Surface("thermal-grain", 3) = {2, 7, 6};
Physical Surface("thermal-fluid", 4) = {30, 27};
Physical Surface("burning", 5) = {3, 4, 5, 10, 13, 9, 11, 12};

Physical Surface("case-sym", 11) = {49, 51, 34, 43, 44, 47};
Physical Surface("thermal-sym", 12) = {24, 28, 14, 23, 29, 33};
Physical Surface("grain-sym", 13) = {8, 1};

Physical Volume("case", 1) = {6, 5, 7};
Physical Volume("thermal", 2) = {2, 3, 4};
Physical Volume("grain",3)={1};

The picture looks ok at first glance. The vertices near material boundaries are well aligned, see enlarged views below:

However, inside the geometry (actually, near the middle of the cylinder part), you can find the vertice are not aligned:

It is weird because, on the boundary of the green and yellow material, all the vertice are aligned. Even though the output mesh contains duplicated points, I can easily remove duplicated ones according to the coordinate. I think this means gmsh does have the ability to ensure this.

However, near the yellow/blue interface, vertice just randomly distributes on two sides, it is then impossible to connect the vertices without modifying the coordinates.

I think there must be some way to ensure gmsh to use the same vertex on both sides of the interface, but I didn't find relevant information in the document. Any suggestions?

OK, I've got the solution somewhere else. I am posting it here to help others who encountered the same issue.

The problem is resulted by my modelling procedure. I modelled the geometry using Creo in separated parts and then exported the assembly. As a result, the *.stp file contains several geometries which are not topologically connected.

To solve this, we need to merge the duplicated surfaces. There are two options:

You can use the new CAD features in Gmsh to remove these duplicate internal surfaces. With the stable release, you can do

SetFactory("OpenCASCADE"); v() = ShapeFromFile("file.step"); BooleanFragments{ Volume{v()}; Delete; }{}

With the latest development snapshots, you can use the "Coherence" shortcut (which does exactly the same thing):

SetFactory("OpenCASCADE"); Merge "file.step"; Coherence;

The Coherence didn't work for my model, but BooleanFragments worked perfectly. Thank professor Geuzaine for offering help.

问题的原因出在Creo导出的装配体上（我相信其他CAD软件也是一样的，没时间测）。虽然画图的时候，几个零件的接触面是在一起的，但由于他们是不同的零件，所以导出时Creo并不会把这些贴在一起的面做合并——奇怪的是，gmsh的交互式选择GUI界面中并未区分这两个贴在一起的面，所以开始时我以为Creo或者gmsh做了自动合并。

所以，非常合乎逻辑地，gmsh把他俩当成了毫无关联的两个零件，给你对齐是情分，不给你对齐也完全合理。

希望官方赶紧把Coherence开发好吧，现在（2017年11月24日）这玩意儿还标着实验性功能呢，无效的话就只能先拿老办法顶着。

PS：最近还发现了一个小问题：如果要使用`gmsh`中的`netgen`功能，系统`PATH`必须是可以访问到你安装的`netgen`可执行文件了，否则可能使得（起码在windows下是）`gmsh`会不报错直接崩溃。