Design in 3D mode

Application area:

This mode allows you to create 3D model. Sketches must be used to build the model. Details

Toolbar/Element properties.

Undo. Reverses the last action.

Redo. Reapplies the last undone action.

Play. Animate the model history step by step to get a better understanding of the design intent (The model must contain several elements in the build tree.)

Plane. Allows you to set a plane for a drawing.

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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.

Spline. A spatial curve, represented by a spline, a polyline, and a helical line.

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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.

Spline.

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.

Closed. Allows closing the spline.

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. This function is not supported on cylindrical surfaces or circular geometries

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.

Helix. A spatial curve.

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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.

Base element. 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 element selection field is pressed.

Change the helix direction by clicking the arrow button.

Helix type. There are three possible variants of the helical line.

Cylindrical.

Conical.

Flat (Archimedes).

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

When using the By Pitch option, the step is controlled by the Pitch parameter.

With the By Angle option, the length is controlled by the Total Angle parameter.

For the By Count option, the step is controlled by the Number of Threads (NB of Threads) parameter.

Below are all remaining parameters available depending on the Helix type.

Height. Determines the height of the spiral.

Start Runout. Radius Exit for the Start diameter. A positive value increases the diameter outward from the base diameter, while a negative value subtracts twice the exit radius value from the base diameter.

End Runout. Radius Exit for the End diameters. A positive value increases the diameter outward from the base diameter, while a negative value subtracts twice the exit radius value from the base diameter.

Diameter. This option allows you to change the diameter of the helix.

Start Angle. This option allows you to change the angle of the starting point relative to the center of the helix.

Start diameter. This option allows you to change the lower diameter of the helix.

Cone agle. Determines the angle of the spiral.

End diameters. This option allows you to change the upper diameter of the helix.

Sketch. Allows you to create a sketch in the selected plane

Extrude. Extrude areas of the sketch to create a prismatic shape.

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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. Details

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 using the By Pitch option, the step is controlled by the Pitch parameter.

With the By Angle option, the length is controlled by the Total Angle parameter.

For the By Count option, the step is controlled by the Number of Threads (NB of Threads) parameter.

When pulling out a gear profile constructed in a sketch (Details) 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

Revolve. Revolve areas of the sketch around an axis.

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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

Sweep. Stretching the profile along the trajectory. The profile can be a closed or open outline sketch ( Profile ). The contours of a sketch, spatial curves, and edges of bodies can act as a Path

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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 Helix function.

Pattern. Similar to the Extrude function.

Coil. Generation of a 3D solid by extruding a sketch along a helical trajectory (unlike the Sweep operation, explicit creation of a helical guide curve is not required).

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1. Call the Coil command from the toolbar, then select the profile (sketch outline) to extrude with the mouse.

By default, the coil axis is aligned with the sketch's X‑axis; its position can be later adjusted (restriction: the axis must lie within the sketch plane).

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

Profile. Defines the profile of the drawing.

Change the Coil direction by clicking the arrow button.

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.

Input method. Similar to the Helix function.

Height. Allows you to change the element height.

End Runout. Similar to the Helix function.

Pattern. Similar to the Extrude function.

Filet. Round sharp corners of the model.

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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

Chamfer. Chamfer sharp corners of the model.

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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

Draft faces. Tilt the selected surfaces relative to a given plane.

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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

Offset. This functionality allows you to offset a selected surface by a specified distance. It can be used for creating a blank. Details

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Delete face. R emove elements of a part (holes, grooves, chamfers, etc.) It can be used for creating a blank. Details

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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.

Pattern a part. Mirror or create a linear or circular pattern of the given part. In the window, select the model and specify the type of reproduction. The reproduction patterns are described in the Extrude.

Combine parts. Combine two parts together with boolean addition, subtraction or intersection. The result is one body out of two. Works similar to the Extrude function, only with details.

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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.

Scale the whole model. Scale the whole model by specifying the scale factor or entering a new dimension of the model.

Load. Allows you to download internal format (*.gsm) and sample projects. There is a New Model button that allows you to clear the 3D mode.

Save. Allows you to save in internal format (.gsm) and export to format (.stp).