急啊，帮帮忙呀

::y::y请问各位朋友，有没有办法把CAD里的三视图调入PRO/E里，并一一对应，也就是说CAD里面的主视图在PRO里是主视图，CAD的左视图在PRO里对应的也是左视图，仰视图也一样。我现在要利用CAD里面的二D图档调到PRO里画三D.但用一般的方法把二D图插入PRO里只能利用上（主视图，左视图，仰视图中的其中一个视图。我现在就是想看有没有办法把三个视图都利用起来。请各位朋友帮帮忙。::y::y::y::y::y::y::y::y::y::?::?:-P:-P::y

不用了，自己顶出来了，谢谢:-P大家。:-P:-P::y::y::y

帮你顶

Creating Solids from DXF's  
由DXF文件创建实体  
If you've ever dealt with importing geometry from another CAD source, you've also dealt with the headaches of finding the right translation medium.  
如果你曾处理从别的CAD系统输入的几何，你也会碰到找一个正确的转化媒介的问题。  
Pro/E does handle several Import/Export types. In our February 1999 Tip we addressed issues with 3D surface geometry like IGES.  
PROE确实能处理一些输入输出。在1999年二月我们发布的tip中描述了处理IGES等3D的曲面几何。  
But, What if the information is only available in 2D? like DXF? How do you get that into a Pro/E solid model?  
但是，如果只有2D的信息呢，如DXF？怎样将这些导入proe的实体模型中？  
To start, notice that Pro/E will not import 2D formats directly into a 3D model, so we have to use a work around. The work around follows these steps (more detail in the example below):  
首先，请注意proe不会将2D格式直接导入3D模型中，所以我们要使用一个work around. 这work around是以下几步组成：（细节见后面的例子）  
1. Import the DXF file into a blank Pro/E drawing.  
将DXF文件导入空的proe图纸文件  
2. Align the respective views for export.  
对齐相关的视图以供输出  
3. Export views as IGES (so they can be read in 3D).  
以IGES格式输出视图（这样可以在3D中被读入）  
4. Import the views into the Pro/E model.  
在proe模型中输入视图  
5. Build the part geometry in 3D based on the 2D info.  
以2D信息在3D中建立实体几何  
  
The above steps are illustrated in the following step by step example showing how a DXF file was used as reference to create a Pro/Engineer solid.  
以下将以一个一步一步的实例来描述怎样以一个DXF文件为参考，建立一个PROE的实体  
1. Start a blank Pro/Engineer drawing. File > New > Drawing > give it a name > OK > make sure the "Optional Default Model" field is blank > OK.  
开始一个空的PROE图纸文件。File > New > Drawing > “文件名称“ > OK >确信 "Optional Default Model" 这个框是空的。  
2. Import the DXF file. File > Import > Append to Model > choose DXF or All Files from the "Type" pull down menu > select the correct DXF file > OK.  
输入DXF文件，File > Import > Append to Model > 在type的下拉式菜单中选择DXF或则是All files > 选择你所需要的DXF文件 > OK.  
  
Figure 1 - Views of DXF file  
图1-DXF文件的视图  
Note: If Pro/E complains about the scale, it is possible that the DXF was created in a different units scheme (Metric vs. English) or the format you chose is too large or small. Usually, you want to preserve the original scale. That may make the new drawing entities either very large or very small with respect to the Pro/E drawing border, but this blank drawing will eventually be discarded anyway, so zoom as needed to see it.  
注意：如果proe警告比例不对，可能是DXF的单位不对（公制或英制），或者是proe的图纸格式太大（小）。通常，你想保留原始的比例，这使得相对于proe的图纸边界，新导入的对象太大（小）。但最后这个图纸格式会被抛弃，所以放大（缩小）就解决问题了。  
  
Figure 2  
  
3. Locate the 0,0 point on each view. Once the drawing appears, use the >Sketch and >Tools menus to sketch a line with one vertex at the point in each view where you would like the coordinate system (0,0,0) to be in the new (yet to be created) Pro/E part.  
在每个视图上定位0,0点。一旦图纸出现，在每个视图用Sketch或则Tools菜单来画一条线在这个点上  
  
Note: For many models step 3 will not be necessary, but if you need the coordinate system to be at a certain spot in the final model, you must identify that point here. Figure 2 shows a white diagonal line sketched with one vertex at the center of the circle. The line was created by first sketching a line horizontal using the vertex (end point) of the imported horizontal line then picking the vertex of the vertical imported crossing line. The first line was deleted after the diagonal line was sketched.  
4. Move the drawing view (or a copy of it) to the lower left corner of the drawing to prepare to export to the Pro/E part model. When the drawing is exported, Pro/E uses the lower left corner of the drawing as the X0Y0, so the drawing view to be exported must be set-up for this (0,0).  
Note: Either Tools > Copy or Tools > Translate will work with slightly different prompts. I like Copy because it makes steps 5 & 12 easier.  
To copy the view, use Detail > Tools > Copy > Translate > Pick Many > select all the desired entities of the view > Done Sel > From - To > Vertex > select the vertex at the (0,0) point for the view (this may be the end of the sketched entity of step 3). Next select Abs Coords > Enter 0 (zero) for the X Coordinate > Enter 0 (zero) for the Y Coordinate > Enter 1 (one) for the number of copies. The view is then copied to the lower left corner of the drawing. Portions of the view may be outside the Pro/E border -- that's OK.  
5. Use Layers to show only the desired entities of the single view to be exported.  
6. Export the drawing entities in a compatible-for-3D format by using File > Export > Model > IGES > define a name.  
7. Switch windows to your Pro/E part (or start a new part).  
8. Create a new coordinate system at the same location of the default coordinate system (or some offset) using Feature > Create > Datum > Coord Sys > Offset. The new one is created to give flexibility in rotating or moving the imported view.  
9. Import the 2D drawing view using File > Import > Append to Model > select the file created in step 6 above, then place it using the coordinate system of step 8.  
10. If the orientation of the new import feature is not correct, move it by redefining the coordinate system of step 8. The coordinate system may be rotated and/or translated as required.  
  
Figure 3  
  
11. To remove entities from the imported feature (like the drawing border), use Feature > Redefine > select the import feature > Heal Geometry > Delete. Use the appropriate menu options there to remove unnecessary pieces of the imported geometry.  
Warning - these actions cannot be undone so be careful. Figure 3 show the first section imported, drawing border removed.  
12. Repeat steps 4 through 11 to import and position all the desired views. Move the views as appropriate to begin modeling.  
13. Figure 4 shows the completed model for our example. In the picture, the model is shown transparent with the sections and end views all imported and located as applicable for model. The imported views were used as reference and as visual location as the model was created.  
  
Figure 4 - Completed part with Imported geometry shown.  
Note: There are times when the imported geometry does not make sense in 3D. Be prepared to create things (like rounds especially) in a manner consistent with good modeling practices.  
Note: The green dim lines shown could also be deleted from the imported views, but were left as an easy reference to the dimensioning scheme of the original.  
   
  
Special Thanks to those who asked the question. We hope this gives you a good start. Remember, things are not as easy as they seem ... sometimes you have to be creative.

把视图放到rhino里，根据三视图的对应关系用3d旋转来实现，再转成iges格式，插入pro/e里即可！