Many 3D solids can be created by extruding, rotating or lofting 2D profiles. Other basic solids such as cylinders, boxes, cones or pyramids can be defined by entering dimensions. Nearly all mechanical parts are comprised of basic solids, which can be joined and/or trimmed. Combining and subtracting solids are called Boolean operations, and resulting solids are called “Boolean Trees.” VariCAD provides tools to add solids and to use one solid to cut another, either keeping or deleting the cutting solid. Commonly-used Boolean operations such as drilling holes, creating grooves, and cutting by a large box are also available. Blending functions are provided for rounding and chamfering solid edges.
Using 2D profiles to create solids enables you to model a wide range of objects. The solid shape can be edited by modifying the original 2D profile.
When using a 3D function that requires a 2D profile as input, you will be optionally switched to the 2D drawing area. You can stay in 3D and create the profile using 2D drawing in 3D. In this case, you can define a drawing plane:
If you create a new profile used for extrusion, rotation or other similar method of solid creation, the created solid is pre-inserted according to the profile’s location in 3D space.
If you edit an existing profile of a solid, you will always stay in 3D and the profile will be edited with 2D drawing methods in 3D.
Profiles are created by 2D lines, arc segments or NURBS 2D curves. There are two methods of profile detection:
|Detect Profile Segments (or press E) - define the profile segment by segment|
|Detect Profile (or press F) - select one segment and the entire chained profile is detected|
Apart of automatic detection of profile’s segments, you can select objects with standard methods of 2D selection – see Selecting 2D Objects. Press Enter or right-click to finish the profile definition. When the solid is created, you return to 3D space and define the object location. See Transforming and Copying Solids.
Profiles used for 3D solids must be continuous. If multiple profiles are used, they cannot intersect; one profile must completely encompass the other profiles. Profiles used in a Revolve operation cannot intersect the revolving axis.
Lines, circles or circular arcs can be selected for all type of solid creations.
If a profile contains gaps or intersections of segments, you can optionally highlight a location of the error.
Prior to selecting a 2D profile, most solid functions require you to enter the solid height or revolving angle. Along with these parameters, you can also identify the solid insertion point and set the X axis direction. If you do not select an insertion point, the point at lower left point of profile will be used. If you do not set the X axis, the default 2D X axis will be used. The insertion point and X axis direction are used when inserting the solid into 3D space.
Example of Insertion Points
Run “CFG” command to set solid insertion point relative to its creation profile. Although this setting can be done within the profile definition, not all functions offer this. Insertion point setting during profile definition is possible only when the solid height or rotation angle is defined. You can use this function at any time, and it will set the insertion point for subsequent solids. You can also choose whether to define the insertion point and X axis direction automatically.
Full Revolve - RSO
Revolves one open or closed profile 360 degrees about a revolving axis. For an open profile, the axis is defined by the profile endpoints. For a closed profile, you must define the axis. If the insertion point is defined automatically, it is located at the first defined point of the revolving axis. When selecting closed profiles, multiple profiles are allowed inside one outer profile - this will create holes in the solid.
Example of Full Revolve using an open profile
Partial Revolve - RSOP
Similar to Full Revolve, except that you can enter a revolving angle less than 360 degrees.
Example of Partial Revolve using closed profiles
Extrude - ESO
Command extrudes a profile to a specified height, forming a solid. Profiles must be closed and multiple profiles are allowed inside the outer profile - this will create holes in the solid. Optionally, you can select a draft angle of extrusion.
Prismatic Loft - PYR
Creates a solid by lofting one closed profile, or one closed profile with one inner profile, by a specified height toward another profile or profiles. Profiles must have the same number of segments.
Loft Rectangle to Circle - PRC
Similar to Prismatic Loft, this function lofts a rectangle toward a circle or vice-versa. The rectangle can have rounded corners.
Example of Extrude, Prismatic Loft and Loft Rectangle to Circle
Coil (Rotated Profile) - PRR
Similar to Prismatic Loft, Coil creates solids by lofting one profile to another while rotating as well. The 2D profile can be open, in which case only one profile is used and the revolving axis is defined by the profile endpoints. With closed profiles, multiple profiles are allowed inside the outer profiles - this will create holes in the solid, and the revolving axis must be defined. The base and top profiles must be similar to one another, as in Prismatic Loft.
Example of solid coil, created by lofting and rotating profiles
Helix - HLX
Creates a solid by extruding and rotating a 2D closed profile. Multiple profiles are allowed inside the outer profiles - this will create holes in the solid. You can choose whether the profiles represent the radial, normal or axial section. For example, a spring uses a circle as the normal section. Using a negative rotation angle will result in a helix with left ascent.
Example of spring helix defined by a normal section
Basic solids are easy to create; you only need to specify basic dimensions. Editing involves changing the basic dimensions, or modifying any 2D profiles that are used. When entering solid dimensions, you have the option of copying any or all dimensions from another solid of the same type. Primarily, dimensions of solids are edited using spatial dimensioning. Optionally, you can select entering dimensions in panel. In panel, you can also change basic shape, like chamfering cylinders etc.
The basic solids are as follows:
Box - PRS
Cylinder - CYL
(with option of rounding or chamfering either end)
Cone - CON
Pyramid - TPY
(uses rectangular base)
Pipe Elbow - PEL
Pipe - PIP
Cone Pipe - CPI
Solid Elbow - ELW
Sphere - SPH