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Subtraction of components |
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Subtraction allows you to create a cavity that has the shape of the subtracted part. Both parts should be inserted into one assembly. The part subtraction operation is available in the in-place editing mode of the part in which a cavity should be made.
Subtraction is performed using the Subtract components 
command.
Step-by-step instructions
1.Specify the part to be subtracted from the edited one, in the graphic area or in the Design Tree.
The name of the subtracted part is displayed in the Components field on the Parameters toolbar. In the graphic area, the part is highlighted.
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Subtraction is possible if the edited part and the parts subtracted from it each contain one solid. For multisolid parts, subtraction is not possible. |
2.If you want the dimensions of the cavity being created to differ from the size of the subtracted part, enter the linear expansion ratio in percent for the cavity in the Coefficient Coefficient field on the Parameter Panel. Details...
3.If necessary, specify the operation name in the Properties section.
4.To complete creating the cavity, click Create object 
.
5.If the operation results in a solid consisting of multiple parts, then after specifying the operation parameters the program starts the process of changing this set of parts. Keep the desired parts of the model (see Selecting the parts to keep).
6.To complete operation of the command, click Finish 
.
In the current part a cavity is formed, having the given shape and size. On the Design Tree branch corresponding to the current part, the icon for the component subtraction operation and its name will appear.
Having completed the creation of the cavity, exit the "in place" editing mode.
You can hide or exclude from calculation the parts used to form the cavity.
See Also
Boolean operations on parts: overview
Managing dimensions of a cavity formed in a part
If necessary, you can increase or decrease the dimensions of the cavity obtained by subtracting parts. To do this, set the appropriate coefficient in the Coefficient Coefficient field on the Parameter Panel. To increase the dimensions of the cavity, the coefficient value should be positive, to decrease them it should be negative.
The cavity will increase in comparison with the subtracted part by (1 + k/100) times, where k is the specified coefficient. By default, the cavity scaling center is the center of the dimensional parallelepiped of the subtracted part. You can change the position of the scaling center by specifying the desired point object in the graphic area.
