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Building an extrusion element |
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To add to the model / cutout from the extrusion element model, call the appropriate command, set the construction parameters, check the correctness of the specified values with the help of a phantom and complete the operation.
Extrusion Build Commands
For constructing an extrusion element, the commands Extrusion Element 
and Cut Extrusion 
are used.
Section
Select the section of the extrusion element. For this purpose, in the Main section of the Parameters Panel, click Section field and specify in the Design Tree or in the graphic area one or more objects. Sketches, faces, 3D curves and edges can be specified.
If the sketch objects are built in the way that the sketch contains closed areas, then you can also select one or several areas as a section.
Without interrupting the command, you can build a contour or sketch and use it as a section. The created contour/sketch is added to the section objects after building is completed.
The list of all objects selected as sections is displayed in the Section.
More details on setting a section...
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In the future, during editing the extrusion element, objects selected as a section can be replaced by other objects. In this case, the model geometry based on extrusion elements may lose the link with its reference objects. To prevent this, it is necessary to establish a correspondence between the initial result of the extrusion operation and the result obtained after replacing the section objects. For this purpose, Create with matching |
in the section Guiding Object
If the section is a sketch (a sketch area) or a flat face, then this sketch/flat face is automatically selected as a guiding object.
If the section comprises several objects including sketches (sketch areas) and/or flat faces, then the first specified sketch or flat face is automatically selected as the guiding object.
Extrusion is perpendicular to the sketch / face plane.
To set another guiding object, in the Main section of the Parameter Panel, click in the Guiding Object. Then specify in the Design Tree or in the graphics area any flat or straight-line object. If necessary, you can build a vector that sets the direction of extrusion.
For more details on the selection of the guiding object...
Extrusion direction and depth
The element can be extruded in one direction and in two opposite directions.
The extrusion depth can be determined in various ways. To select the desired method use the group of buttons labeled Method.
To extrude in one direction, select the method for determining the depth and set the parameters for the selected method in the Main section of the Parameter Panel.
If you want to extrude an element in two directions, follow the steps described above in the Main section of the Parameter Panel for the first extrusion direction, then set the Second direction toggle switch in position I (on) and set the desired parameters for the second direction.
It is also possible to build symmetrically, the parameters of which are configured in the Main section of the Parameter Panel. In this case, the Second direction toggle switch is not available.
More details on setting the extrusion direction and depth...
Extrusion slope angle
If sketches and/or flat faces lying in parallel planes are used as section objects, and the extrusion direction is perpendicular to the section, it is possible to perform a taper of the side faces of the extrusion element. To do this, set the value and direction of the slope using the Angle field and Change direction buttons to the right of this field.
More details on setting the inclination...
Creating a thin-walled element
If you want to form a thin-walled element, set its parameters in the Thin-walled element section:
•set the Thin-walled element toggle switch in position I (enabled),
•determine the direction of the thin wall construction and its thickness.
More details on building a thin wall...
Operation Application Area
The operation application area is a set of objects which should be transformed as a result of the operation. Specifying the area is required if the model contains several solids or components.
The controls for the operation application area are contained in the Application area section. This section is present on the Parameter Panel for any result of the operation, except for the creation of a new solid.
The operation application area can include solids 
, components 
or components and solids 
. To select the desired option use a group of buttons Groups of objects.
The operation can extend to all objects of a selected group or to some of them. To select objects, the intersection with which will be taken into account when building, use a group of buttons Objects.
More details on defining the operation application area...
Extrusion Element Properties
If necessary, you can set the name of the extrusion element and the properties of its surface display using the controls located in the Properties Parameter Panel.
Management of the color and optical properties of objects...
Completing the operation
To complete the extrusion feature, click Create item 
button.
If the operation results in a solid consisting of multiple parts, then after completing the operation, the program starts the process of modifying this set of parts. Select the parts that should be left. Details...
After performing the specified actions in the graphics area, a new solid, a glued or cut element appears (depending on the selected result of the operation). In the Design Tree, an extrusion/cutting operation is displayed with one of the following icons:
glued element/new solid,
deleted element.
To complete operation of the command, click Finish 
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•The depth, slope and wall thickness values can be changed in the graphical area of the model – using defining points. If the section of an extrusion element includes multiple objects, defining points are displayed on the phantom of the first object.
•You can set linear and angular parameters using the geometrical calculator.
•You may assign tolerances, specified in linear or angular units, to operation parameter values. To do this, invoke the Tolerance command located in the required parameter menu, or click the icon 
displayed in the parameter field (the icon is displayed if a tolerance is assigned to the parameter value). More details on assigning tolerance...
See Also
