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Construction of a rotation 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 Rotational 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. You can, without interrupting the work of the team, to build a contour or sketch and use it as a section.
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 
.
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),
•determine the direction of building a thin wall 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...
Rotation Element Properties
If necessary, you can set the name of the rotation 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 rotation feature, click Create item 
.
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 will appear, glued or cut out the element (depending on the selected result of the operation). In the Design Tree, a revolve / cut operation will be displayed with one of the following icons:
glued element/new solid,
cut element.
To complete operation of the command, click Finish 
.
•The rotation angle and wall thickness can be set using defining points.
•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, use the Tolerance command located in the menu field of the parameter to be set.
More details on assigning tolerance...
See Also
