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Cone |
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To build cones in KOMPAS-3D, the following commands are used:
•Cone by center of base, diameters and height,
•Cone by center of base, diameters and angle,
See also
Cone by center of base, diameters and height
To build a cone based on the center of the base, two diameters and the height, use the command Cone by center of base, diameters and height 
.
Procedure
1.Select operation result, clicking the required button in group Result on Parameter panel:
Merging,
New solid,
Subtraction,
Intersection.
For variants Merging, Subtraction and Intersection you can set operation application area in section Application area.
2.The graphic area displays a phantom cone with a basing element 
. Set the position of the cone anchor point in the group Position and the orientation of the axes of its coordinate system in the group Orientation. These actions are similar to setting the position of the LSC in the model and are described in detail in the sections LCS position and LCS orientation.
You can change object position in graphic area using the basing element.
The cone position can also be specified by specifying a flat face/plane or a circle/circular arc in the Design tree or graphic area. The name of the object will appear in the Snap point.
•If a flat face or plane is specified, the base point of the cone is built at the location where the object is specified. The snap point field displays the method for building the point — On surface. The Z axis is directed perpendicular to the specified face/plane.
•If an edge, sketch curve, or circular/arc-shaped spatial curve is specified, the base point is created at the center of the circle. In the field Snap point the way In center displays.The Z axis is directed perpendicular to the plane of the circle/arc. In this case, the diameter of the cone base is set equal to the diameter of the circle/arc.
An associative link is formed between the selected object and the cone, due to which the cone will follow the object when its position changes.
3.Specify the diameter of the cone base. The value will be displayed in the field Diameter of base. Details about diameter assigning...
The diameter of the second base of the cone is zero by default. If you want to draw a truncated cone, set the diameter of the second base similar to the diameter of the first base. The value will be displayed in the Diameter field. The diameters of the bases do not have to be equal.
4.Set the direction of building and the height of the cone in the Height group of elements. This is done in much the same way as when building an extrusion element.
•the cone can be built in one direction or in two opposite directions, including the creation of a body symmetrical relative to the supporting plane; for more details, see the section Direction and depth of extrusion;
•the method for determining the height for each direction is set using a group of buttons Method:
• To distance,
• Through all,
• To object (for a cone, unlike an extrusion element, only point objects can be used in this method).
5.Press button Create object 
to complete the building.
6.To complete the command, click the button Finish 
.
Once the building is complete, a cone will appear in the model and its icon will appear in the Design tree.
Additional parameters of elementary solids
Cone by center of base, diameters and angle
To build a cone based on the center of the base, two diameters and angle, use the command Cone by center base, diameters and angle 
.
Procedure
1.Select operation result, by clicking the required button in the Result group on the Parameter panel:
Merging,
New solid,
Subtraction,
Intersection.
For variants Merging, Subtraction и Intersection you can set operation application area in section Application area.
2.The graphic area displays a phantom cone with a base element . Set the position of the cone's base point in the Position group and the orientation of its coordinate system axes in the Orientation group. These actions are similar to setting the LCS position in the model and are described in detail in the LCS Position and LCS Orientation sections.
It is available to change object position in the graphic area using the base element.
The cone position can also be specified by specifying a flat face/plane or a circle/circular arc in the Design tree or graphic area. The name of the object will appear in the Snap point.
•If a flat face or plane is specified, the cone's reference point is built at the location where the object is specified. The Snap point field displays the point building method — On surface. The Z axis is directed perpendicular to the specified face/plane.
•If an edge, sketch curve or 3D curve in the form of a circle/arc is specified, the snap point is created at the center of the circle. The Snap point field displays the In center method. The Z axis is directed perpendicular to the plane of the circle/arc. In this case, the diameter of the cone base is set equal to the diameter of the circle/arc. An associative link is formed between the selected object and the cone, due to which the cone will follow the object when its position changes.
3.Specify the diameter of the cone base. The value will be displayed in Diameter of base field. Details about assigning diameter of base...
The diameter of the second base of the cone is zero by default. If you want to construct a truncated cone, set the diameter of the second base similar to the diameter of the first base. The value will be displayed in the Diameter field. The diameters of the bases do not have to be equal. The diameter of the second base can be larger than the diameter of the first base. In this case, you will need to change the slope of the cone generator (see item 4).
4.In the Angle field, specify the inclination of the generatrix to the cone axis.
To change the slope of the generatrix, enter a negative value in the Angle field or click the Change direction button 
to the right of this field.
5.The cone can be built in one direction or in two opposite directions.
To construct in two directions, set the Second direction switch to position I (on) and set the parameters for the second direction of the cone: the angle of inclination of the generatrix and the diameter of the second base.
To perform a symmetrical building in both directions from the base of the cone, set the Symmetrical switch to position I (on). The diameter of the second base and the angle of inclination of the generator will be the same in both directions. The Second direction switch becomes unavailable.
6.Press the button Create object , to complete the building.
7.To complete the command, click the button Finish .
Once the building is complete, a cone will appear in the model and its icon will appear in the Design tree. .
Additional parameters of elementary bodies
To build a truncated cone using two arcs, use the command Cone by wo acrs 
.
Procedure
1.Select operation result, by clicking the desired button in the Result group on the Parameter panel:
Merging,
New solid,
Subtraction,
Intersection.
For variants Merging, Subtraction and Intersection it is available to assign operation application area in section Application area.
2.Specify two arcs in the Design tree or in the graphic area. An arc can be an edge, a curve in a sketch, or a 3D curve in the form of a circle/circular arc..
After selecting objects, a cone phantom appears in the graphic area. The names of the specified objects are displayed in the fields Arc 1 и Arc 2 on Parameter panel.
3.If necessary, specify the name of the cone and the display properties of its surface using the controls located in the Properties section.
Details about color and optical properties management...
4.Click the button Create object to complete the building.
5.To complete the command, click the button Finish .
Once the building is complete, a truncated cone will appear in the model and its icon will appear in the Design tree. .
•The values of the base diameters and the angle of inclination of the cone generator can be changed in the graphic area of the model - using defining points.
•To set the linear parameters of the operation, you can use the commands geometrical calculator.
•You can assign tolerances to the values of operation parameters expressed in linear quantities. To do this, call the Tolerance command located in the menu of the required parameter. Details about tolerance assigning...
