（已解决）请问catia画的图能找到形心和质心么？

请问CATIA画的图能找到形心和质心么？谢谢您！

可以找到重心，使用测量惯性。

多谢楼上那位朋友！请问“使用测量惯性”，能说的清楚一点么？麻烦您了！

看这里！

Measuring Inertia  
  The Measure Inertia command lets you measure:
3D inertia properties of surfaces and volumes (explained below)  
2D inertia properties of plane surfaces.  
   
  This task explains how to measure the 3D inertia properties of an object.   
  You can measure the 3D inertia properties of both surfaces and volumes, as well as retrieve the density or surface density if valuated from V4 model type documents. You can also retrieve inertia equivalents set in Knowledgeware formulas.  
The area, density, mass and volume (volumes only) of the object are also calculated.
   
  Measures are persistent: a Keep Measure option in the Measure Inertia dialog box lets you keep the current measure as a feature in the specification tree.  
Note: The Keep Measure option is not available in the Drafting workbench.
   
  For examples showing 3D inertia properties measured on surfaces. To find out more about notations used.  
  Insert the Valve.cgr document from the samples folder. It is to be found in the online documentation filetree in the common functionalities sample folder cfysa\samples.  
  1. Click the Measure Inertia  icon.  
In DMU, you can also select Analyze -> Measure Inertia from the menu bar.
   
  Note: In the No Show space, this command is not accessible.
The Measure Inertia dialog box appears. By default 3D inertia properties are measured.
   
   
  A Keep Measure option in the dialog box lets you keep current and subsequent measures as features. Some measures kept as features are associative and can be used as parameters.
Note: This option is not available in the Drafting workbench.
The 2D Inertia icon lets you measure 2D inertia properties of plane surfaces.
   
  Note: When you move the cursor over the geometry or specification tree, its appearance changes to reflect the measure command you are in.   
  2. Click to select the desired item in the specification tree, for example Valve.   
  Selecting Items
In the geometry area, you can select individual faces and edges on cgr files and in Visualization mode.  
   
  Ctrl-click in the geometry area or the specification tree to add other items to the initial selection.  
Shift-click in the specification tree to make a multiple selection.  
Drag (using the left mouse button) to select items using the bounding outline.
Items must be completely inside the bounding outline; if not, they will not be selected.  
(P2 only) Use the Group command to make your multiple selection.
  
Note: Only items of the same type can be included in a multiple selection or a bounding outline; you cannot mix volumes and surfaces.  
   
  The Dialog Box expands to display the results for the selected item.   
The measure is made on the selection, geometry, assembly or part. To measure the inertia of individual sub-products making up an assembly and see the results in the document window, you must select the desired sub-product.
In our example, the item selected has no sub-products.  
   
  
    
  The dialog box identifies the selected item and indicates whether the calculation is exact or approximate:  
In Design mode, measures access exact data and wherever possible true values are given. Note that it is possible to obtain an exact measure for most items in design mode.  
In Visualization mode, measures are made on tessellated items and approximate values are given.  
In addition to the center of gravity G, the principal moments of inertia M and the matrix of inertia calculated with respect to the center of gravity, the dialog box also gives the area, volume (volumes only), density and mass of the selected item.
  
You can also compute and display the principal axes A. To do so, you must first activate the appropriate option in the Measure Inertia Customization dialog box.
   
   The density is that of the material, if any, applied to a product, part or part body:
If no density is found, a default value is displayed. You can, if desired, edit this value. If you do so, all the other inertia values are re-calculated. The default value is 1000 kg/m3 for volumes and 10 kg/m2 for surfaces.  
If sub-products or part bodies have different densities, the wording Not uniform is displayed.  
Notes:
  
You must be in design mode to access the density of parts or part bodies to which materials have been applied.  
Unless specified otherwise, material inheritance is taken into account.  
Density is a measure of an item's mass per unit volume expressed in kg/m3; surface density is a measure of an item's mass per unit area expressed in kg/m2.  
   
  In the Geometry Area, axes of inertia are highlighted and a bounding box parallel to the axes and bounding the selected item also appears.  
Color coding of axes:
  
Red: axis corresponding to the first moment M1  
Green: axis corresponding to the second moment M2  
Blue: axis corresponding to third moment M3.  
  
  3. Click Customize...  to customize the inertia computation and define what will be exported to the text file.  
  Customizing Your Measure
You can, at any time, define what will be computed and displayed in the the dialog box. To do so, click Customize... in the Measure Inertia dialog box.  
  
Note: The inertia properties checked here are also the properties exported to a text file.  
  
Click the appropriate options to compute and display in appropriate tabs of the Measure Inertia dialog box the:
  
Inertia equivalents  
Principal axes  
Inertia matrix with respect to the origin O  
Inertia matrix with respect to a point P  
Inertia matrix with respect to an axis system  
Moment of inertia about an axis  
  
  4. Click OK in the Measure Inertia Customization dialog box when done.  
  5. Click OK in the Measure Inertia dialog box.  
  The number of decimal places, the display of trailing zeros and limits for exponential notation is controlled by the Units tab in the Options dialog box (Tools ->Options, General -&gtarameters and Measure).   
  Exporting Measure Results  
  6. Insert the Body1.cgr and the Body2.cgr documents from the common functionalities samples folder.  
  7. Select the root product and click the Measure Inertia icon.  
  8. Click Export to write the results to a text (*.txt) file.
Results shown in the Measure Inertia dialog box only are exported.  Exported results are given in current units.  
   
  9. Identify the file name and location in the Export Results dialog box that appears, then click Save.  
   
    Note:  If an assembly comprises sub-products or a part comprises part bodies, individual results for all sub-products or part bodies are also exported and written to the text file.
   
   
  If the principal axes A are exported, bounding box values are also exported.  
    
where BBOx,y,z defines the origin and BBLx,y,z the length along the corresponding axis.
  
  Note: When importing the text file into an Excel spreadsheet, do not forget to identify the pipe character (|) used as separator in the Text Import Wizard dialog box.  
  10. Click OK when done.  
   If you checked the Keep Measure option in the Measure Inertia dialog box,  your measures are kept as features and your specification tree will look something like this.
Some measures kept as features are associative and can be used as parameters.
  
  In the Drafting workbench, measures are done on-the-fly. They are not persistent. This means that they are not associative and cannot be used as parameters.  
   You can write a macro script to automate your task. See Space Analysis on the Automation Documentation Home Page.  
  Creating Geometry
A Create Geometry option lets you create the center of gravity and the axis system for principal axes in a part from inertia results.  
  

就是上面的，是CATIA帮助文件，PDF 格式

谢谢楼上的朋友！