You can create sketches on various surfaces, with offset, and more:

• Relative to the base planes

• On the surface of the model

Tangent plane. Create a tangent plane

Click on a plane or a face to create a plane.

RMB: Exit.

Axial plane. Create a plane through an axis

Select a straight edge, a sketch line or a surface of revolution to create a plane.

RMB: Exit.

Middle plane. Create a middle plane.

Select two flat faces to create the middle plane.

RMB: Exit.

Plane throw two lines. Create a plane trhough two lines

Select two straight edges to create a plane.

RMB: Exit.

Create normal plane. Creates a plane normal to a curve. Used with function Spline.

Offset plane. Allows you to set a plane at a distance. Called by right clicking on a surface or plane.

1. Call the Spline command on the toolbar Choose a curve option Spline or Polyline

2. Set points with the mouse (snapping works) or set numeric coordinates in the appropriate field.

3.Use the right mouse button to complete the point assignment.

Curve type. Defines the curve type: Spline or Polyline.

Draw. Switching the mode for entering new points or editing existing ones is done by pressing/releasing the Draw button.

In the editing mode, the selected point is circled, and its coordinates are displayed in separate input fields (X, Y, Z). You can change the coordinates of the selected point either by entering the coordinates or by dragging the mouse. The coordinate input fields are inactive if no point is selected.

On Plane. You can place a spline on a plane by selecting a plane or a flat edge in the OnPlane drop-down list (highlighted when selected). The curve points will be projected onto the selected plane.

Point. Defines a point for the spline

Coordinates. Determines the coordinates of a given point. To set a series of points, you can copy a set of coordinates from MS Excel or a text file and paste them into the Coordinates input field.

An alternative way to create a spline is to select a plane or planar face in model space and select Spline from the pop-up toolbar.

1. Call the Helix command in the toolbar and set the coordinate of the helical line center (point with the mouse or enter the coordinates in the input field)

The geometry of the surface on which the helical line is located is determined by the dimensions: initial and final radii, height, cone angle. You can change the dimensions by entering values in the input fields, adjusting the corresponding visual objects, or dragging the control points with the mouse.

Surface data. Geometry of the surface on which the helical line is located.

Base Surface. To construct a helical line, it is possible to use previously constructed geometry. To do this, in the curve creation/editing mode, click the mouse on the face or surface while the Base Surface selection field is pressed.

To create a helical line on existing geometry, you can select a face or surface and select the Helix command from the pop-up toolbar.

Surface type. There are three possible variants of the helical line: Helix ByCylinder, HelixByCone, HelixByDonut. The surface type is selected in the Surface Type drop-down list.

Center point. Defines the center point of the spiral.

Begin radius. The radius from which the spiral begins (relative to the central point).

Height. Determines the height of the spiral.

Cone agle. Determines the angle of the spiral.

Edn radius. Defines the final radius of the spiral.

Rotate Angle. The angular position of the starting point is relative to the RotateAngle parameter, and can be changed by adjusting the numeric value in the input field.

Twist. The helical parameter of the curve can be set in four ways: Twist By Pitch, Twist By Angle, Twist By Count.

The method of setting is selected from the Twist drop-down list, and the parameter value is set in the Value input field.

1. It is necessary to select a closed contour of the drawing

2. On the toolbar, click the button Extrude

For quick model building, it is better to select closed contours and pull them out interactively (by pulling in the desired direction)

You can also change the dimensions of the model at any time without going over to the drawing. To do this, you can simply grab the edge and move it interactively. This will change the dimensions in the drawing.

Boolean operations.

New part. Allows you to create new parts. See more

Auto. Automatically selects what needs to be done (subtract or add).

Add. Allows you to pull out drawing elements.

Subtract. Allows you to subtract drawing elements from an existing body.

Intersect. Allows you to create new geometric objects based on the intersecting areas of existing objects.

Part. The name of the part to which this operation applies.

Profile. Defines the profile of the drawing

Distance. Determines the distance of extrusion and subtraction. Possible to change interactively.

Also, when subtracting or adding, it is possible to snap to different surfaces of already extruded elements. In this case, the Distance value will be equal to 0.

Symmetrical. Extrude symmetrically both sides from the sketch plane.

Thickness. Thickness of the extrusion relative to the top level.

Thin Wall. Allows you to create thin-walled elements.

The direction of adding thickness contains the following options (in the form of pictograms):

<> - in both directions,

-> outward,

<- inward.

Corner rounding provides sharp or rounded corners for the edges of the outer contour.

Wall thickness input field (can be zero). If the thickness is non-zero, a closed 3D body is formed to which all Boolean operations are applicable.

Twist. Twisting along the normal to the sketch. The parameters are the same as in Helix. For an extrude operation, the twist is performed around the Z axis of the sketch.

When pulling out a gear profile constructed in a sketch (See more) as a block with a given value of the helical angle of the teeth, the twisting is applied automatically, and its parameters are taken from the sketch - Helic angle.

There is no option to disable the twisting. If this is necessary, the corresponding block should be destroyed in the sketch and then the operation repeated.

Pattern. Allows you to create a template for copying elements.

Type. Defines the template type.

Linear. They represent a two-dimensional array.

Defined by. Distance definition method: Extend or Spacing.

Number. Nurmber of copies along the first axis.

Distance. Distance along the first/second axis

Direction. Copy direction.

Second direction. Number of copies along the second axis

Inherited. Allows you to use another breeding template

Circular. Allows you to create a circular array

Angle. Angular span of the pattern

Along axis. Copies along the Z axis

Mirror. Allows you to create an element relative to the selected plane.

Plane. By default, 3 base planes (XY,YZ,ZX) are available. You can also add your own plane before extrusion and use it in this functionality.

The new Boolean operation can use patterns that were used in previous Boolean operations.

1.For example, we will extrude a prism and use the symmetry reproduction scheme

2.Extrude a circle

3.Select the template of the previous extrusion

We get a similar result

Part. The name of the part to which this operation applies.

Profile. Defines the profile of the drawing

Axis. Rotation axis. Can be set interactively by binding to a curve or base axes of the SC

Thin Wall. Allows you to create thin-walled elements. The functionality is described in Extrude

Pattern. Allows you to create a template for copying elements. The functionality is described in Extrude

1.Call the Sweep command from the toolbar, then sequentially select the sweep profile with the mouse - the sketch outline (the Profile selection field is pressed) and one or more path segments (the Path selection field is pressed). As you add segments, the Path field displays the number of segments, and a preview of the 3D element is generated in the main window.

If you need to exclude a selected trajectory segment, click on it again. To complete the construction, you need to click the mouse in the empty space of the model.

An alternative way to create an operation is to select the sketch outline and choose the Sweep command from the pop-up toolbar, then select the path segments.

When you select an open contour as a profile, an open body - a surface - will be constructed.

Part. The name of the part to which this operation applies.

SweepType. Defines the profile of the drawing

Profile. Defines the profile of the drawing

Path. It’s a curve along which a 2D profile is moved to create a 3D object

Thin Wall. Similar to the Extrude function.

Twist. Similar to the Extrude function.

Pattern. Similar to the Extrude function.

1. Click on an edge of the part to add it to the list. The fillet will be propagated to the tangent edges. Double click on the edge to select similar edges.

Remove fillets : Click on an added edge to remove it from the list.

DEL: Press DEL on the keyboard to clear the edges list.

RMB, LMB: Exit.

Edges. Edge for rounding

Radius. Rounding radius

1. Click on an edge of the part to add it to the list. The chamfer will be propagated to the tangent edges. Double click on the edge to select similar edges.
   
   

Remove сhamfer : Click on an added edge to remove it from the list.

DEL: Press DEL on the keyboard to clear the edges list.

RMB, LMB: Exit.

Edges. Edge for rounding

Size. Determines the size of the chamfer

1.Select draft faces Click on a part face to add or remove it to the draft faces list.

RMB, LMB: Exit.

Faces. Click to select the faces to draft

Feature Propagation. Propagate selection to the faces of the same feature.

Taper Angle. Enter the angle of inclination of the faces

Use it with the option Convert to design. ( The option allows you to transform the model and open it in Design mode)

Faces. Defines the selected surfaces

Self-Intersect.

Workpiece. Select the part of the model used as the workpiece body

Tool. Select the part of the model used as the tool body

Keep tool. Keep the tool body in the model after merging it with the workpiece. Allows you to save the second part in the tree.