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Construction of a revolution element |
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To add to the model / cutout from the rotation 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.
Rotation Build Commands
To construct a rotational element, the commands Revolution Element 
and Cut by Rotation 
are used.
Operation result
The result of the operation may be the union / cutting / intersection of the rotation element with the existing solid, as well as the creation of a new solid. To select the desired option, use the group of buttons Result of the Main section of the Parameter Panel.
Options Merging and New solid allow you to add material to the model, and Subtraction and Intersection options – remove material from the model.
More about selecting an operation result...
Section
Select the section of the rotation element. To do this, in the Main section of the Parameter Panel, click in the Section field. Specify a section object in the Design Tree or in the graphic area: a sketch (sketch area), a face, a 3D curve, or an edge.
If the sketch objects are constructed in such a way that closed areas are obtained in the sketch, then a separate area can also be selected as a section.
If needed, you can create a contour or sketch and use it as a section without interrupting the command. The created contour/sketch is added to the section objects after completion.
A list of all objects selected as a section is shown in the Section field.
More details on setting a section...
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In the future, during editing a rotation element, objects selected as sections can be replaced by other objects. At the same time, the geometry of the model that is based on a rotation element may lose the link with its reference objects. To prevent this, it is necessary to establish correspondence between the initial result of the rotation operation and the one obtained after the replacement of section objects. For this, the Create with matching |
button is used in the Axis of rotation
If a sketch is used as a section, and this sketch contains a axis line (object Centerline or segment with style Axial ), then this centerline is automatically selected as the rotation axis of the operation.
To select a different rotation axis, in the Main section of the Parameter Panel, click in the Axis field. Then specify in the Design Tree or in the graphics area any straight-line object or revolution surface. In the latter case, the axis will be the axis of rotation of the surface.
If necessary, you can construct an auxiliary axis that will be used as the axis of rotation during the operation.
More details about axis selection...
Direction and angle of rotation
Rotation can be performed in one direction or in two opposite directions.
The rotation angle is set directly on the Parameter Panel or determined by the specified object. To select the desired method for determining the angle, use the group of buttons Method.
To revolve in one direction, select the method for determining the angle and set the parameters for the selected method in the Main section of the Parameter Panel.
To revolve in two directions, follow the steps described above in the Main section of the Parameter Panel for the first rotation 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 specifying direction and angle of rotation...
Design Type
The rotation element is formed by rotating the section around the axis. Depending on the shape of the section and its position relative to the axis, as a result of the construction, either a spheroid or a toroid can be obtained.
If an unclosed sketch is used as a section and the axis of rotation lies in the section plane, it is possible to construct both a spheroid and a toroid. In this case, in the Main section of the Parameter Panel there is a group of buttons Build type. To select the desired type, click Spheroid 
or Toroid 
.
In all other cases, a toroid is constructed and there is no type selection group.
For details on choosing the construction type...
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),
•position 0 (disabled) - creates a solid element.
For some section objects, only thin-walled elements can be created. If all section objects are thin-walled, the toggle is missing.
When constructing a thin-walled element, it is necessary to specify the direction of construction of the thin wall and its thickness.
More about thin-walled element...
Scope of the operation
An operation's scope is the set of objects that should be transformed as a result of the operation. Specifying a scope is required if the model contains multiple bodies or components.
The controls for the operation's scope are contained in the Scope section. This section is present in the Parameters Panel for any operation result except creating a new body.
The scope of the operation may include Solids 
, Components 
or Components and solids 
. To select the required option, use the Object groups button group.
The operation can apply to all objects in the selected group or just some of them. To select objects whose intersections will be considered during construction, use the Objects button group.
More about setting scope area...
Properties of the rotation element
If necessary, you can set the name of the rotation element and the display properties of its surface using the controls located in the Properties section of the Parameters panel.
Management of color and optical properties of objects...
Completion of the operation
To complete the construction of the rotation element, click the Create object 
button.
If the operation results in a body consisting of multiple parts, the process of changing the set of parts is initiated after the operation. Select the parts to keep. More...
After completing these steps, a new body, either a glued or cut element (depending on the selected operation result), will appear in the graphics area. The Design Tree will display the rotate/cut operation with one of the following icons:
glued element/new body,
cut out element.
To complete the command, click the Finish 
button.
•The rotation angle and wall thickness can be set using characteristic points.
•To set linear and angular parameters, you can use the commands of geometrical calculator.
•You may assign tolerances, specified in linear or angular units, to operation parameter values. To do this, use the Tolerance command located in the menu field of the parameter to be set.
More details on assigning tolerance...
See Also
