Push/Pull

01 - SKETCH REGION

Extrude a sketch

Choose Push/Pull in 3D, then hover a visible closed sketch region. Click once to grab it. Move the pointer to size the preview or type an exact signed millimetre distance. Choose New body to create a separate solid.

Click to place, press Enter, or use the task's Create/Join/Cut button. Esc cancels. After creation, Push/Pull stays active. A sketch with one closed region is hidden automatically; a sketch with several regions stays visible so you can extrude the remaining areas. Hide the sketch with its eye control to select the underlying solid faces.

Adding geometry later: an existing extrusion keeps its selected outer boundary and holes. Adding a separate circle inside its source sketch leaves that solid intact; it does not automatically create a through-hole. Edits to the original boundaries still rebuild the extrusion. Missing, open or intersecting source boundaries can block a rebuild and show an explanation in the 3D view.

02 - CURRENT SOLID

Push/Pull the same face again

A supported planar solid face highlights when you hover over it. Click to begin a direct edit, move along its normal arrow or enter a signed Distance, then choose Apply face edit, click in the viewport, or press Enter.

Each edit starts at the current face position: +5 mm followed by +3 mm adds 8 mm. Positive distances add material; negative distances remove material. Holes in the selected region remain holes. No additional sketch is needed.

03 - FACE-ATTACHED SKETCH

Draw on the edited shape

Choose Sketch, then click a supported planar face of the current Extrude body. This includes faces after direct Push/Pull, sketch Join/Cut, and supported finishing operations. Cadivari creates a face-attached sketch plane, aligns the 2D editor, and shows the face boundary as projected reference geometry.

Draw a closed profile, finish the sketch with 3D, and extrude it. A side-face rectangle can cut a cross-hole; a circle can create a round boss. The sketch plane does not need to be parallel to the body's original sketch.

For a circular pocket: choose Sketch and click the solid's top face, draw the circle, return to 3D, then choose Push/Pull and Cut. Pick the circle's region, enter the inward depth, and apply Cut body. The face sketch is a separate sketch in the tree. Clicking the original sketch's edit button, or reopening its origin plane, edits that original sketch instead.

Plane can also use the current planar face for an associative construction reference. Face identity is tied to the selected stage of the body's history: earlier edits rebuild its support, while later operations use that support without making the sketch depend on itself.

04 - MATERIAL OPERATION

Choose New body or Join or Cut

The Sketch operation controls apply when you pick a sketch region. New body creates a separate solid; Join adds material to the target; Cut subtracts the overlapping volume. Select the intended Target, especially when several bodies are present. Face-attached sketches identify their owning body.

New sketch Join/Cut features evaluate the actual preceding solid in 3D, including arbitrary sketch-plane orientation and preceding direct face edits. They can appear later in the same history. The preview and saved result use the same rebuilt boundary.

Picking an existing solid face opens the separate Push/Pull face card. Its signed distance controls addition or removal independently of the Sketch operation setting.

SKETCH REGIONS

Several selectable areas in one sketch

A rectangle crossed by straight sketch lines can form several closed regions. The lines do not need to be closed individually: each region uses the portions of lines and rectangle edges around it. Endpoints must meet an edge, or lines must actually cross. A line that stops short does not close an area.

1. In one sketch, draw a rectangle, a horizontal line from its left edge to its right edge, a vertical line from bottom to top, and a diagonal joining the left and bottom edges below the horizontal line. With the diagonal in the lower-left area, this produces five closed regions.
2. Check Closed faces in the sketch summary. Return to 3D and choose Push/Pull.
3. Hover over an enclosed area to highlight it, click, type a distance and press Enter. Use New body for separate solids, or explicitly choose Join or Cut and the intended target body.
4. A sketch with several regions remains visible after extrusion. Select the next uncovered area and give it a different height. Hide the sketch using its eye control when finished.

The rectangle and lines remain editable objects; Cadivari does not permanently trim or duplicate them. Editing a dividing line updates the selected region and its extrusion while the same boundary connections remain intact. If an edit splits, merges or opens that selected region, the feature reports the changed reference. Restore the lines or remove the dependent extrusion and select the intended region again.

Existing models: extrusions made from a complete rectangle or closed chain retain their original profile when new dividing lines are added. New selections use the smaller regions.

Supported boundaries: automatic splitting supports rectangles, straight lines, circles, circular arcs and unmirrored splines, including crossings and paths ending on a boundary. Coincident straight and circular spans are treated as one boundary. Dangling lines and arcs do not create extra regions. A fully contained circle can form a hole; intersecting circles and arcs form their own smaller selectable areas. Open or closed unmirrored splines can divide these regions too; their control points remain editable. Mirrored spline halves and text/artwork retain their existing whole-profile behavior. Choose one region for quick extrusion, or Ctrl-click several as described below.

CIRCLES AND ARCS

Extrude part of a circle or a curved intersection

Circle and circular Arc now participate in the same region detection as Rectangle and Line. A line through a circle divides its disk into two profiles. Two crossing lines can produce four quadrants. Two overlapping circles produce three profiles: the shared lens and a crescent on either side. An arc and connected lines can enclose a profile even though the arc itself is open.

1. In one sketch, draw a circle and two crossing lines through its centre. Extend each line past both sides of the circle so it clearly intersects the outline.
2. Return to 3D > Push/Pull. Confirm that hovering highlights one quadrant at a time.
3. Click a quadrant, enter 10 mm, and create a New body. Select another uncovered quadrant and give it a different height.
4. For one combined extrusion, Ctrl-click two adjacent quadrants, choose Extrude selected, and enter a shared distance. Adjacent selected areas merge; disconnected areas produce separate New body outputs.
5. On a solid face, choose Sketch and select that face before drawing. Return to Push/Pull and use the same region selection for Join or Cut, with the intended target body.
6. Save and reopen, then edit the circle radius or a dividing line. The extrusion follows its stored region while the same boundary connections remain intact.

The original circle, arc and lines remain editable. Intersections are calculated from their geometry; no permanent trimming is applied. A previously stored whole-circle extrusion remains whole when a dividing line is added. Newly selected portions store their own region references. An edit that removes, splits or merges such a region reports a changed reference instead of choosing a nearby area.

SPLINE REGIONS

Divide profiles with an editable spline

An open spline crossing a circle or rectangle can divide it into enclosed regions. Unmirrored splines also intersect lines, circular arcs and other splines. A closed spline can be divided in the same way, and a spline joined to ordinary lines can enclose a profile.

1. Draw a circle. In the same sketch, draw a simple S-shaped spline starting outside the circle and ending beyond the opposite side. Its actual curve must cross the circle twice; the control polygon alone does not count.
2. Return to 3D > Push/Pull. Hover over either side of the spline to highlight that enclosed region.
3. Extrude one side to 20 mm, then give the other side 10 mm. The shared wall follows the spline.
4. Alternatively, Ctrl-click both areas, choose Extrude selected, and use one distance. Adjacent regions combine into one body. The same selection works for Join and Cut on a suitable target body.
5. Edit a spline control point, then return to 3D. The extrusion rebuilds while the selected region keeps the same boundary connections. Save and reopen to retain both the spline and its linked extrusions.

Cadivari computes intersections on the spline geometry and uses bounded curve samples for the resulting solid. It does not convert the editable spline into line objects. If an edit changes which regions exist, the affected extrusion reports a changed reference so you can restore the boundaries or select the intended region again.

MULTIPLE REGIONS

One preview for several sketch regions

1. In 3D, choose Push/Pull. Hold Ctrl (Cmd on Mac) and click the first region to start a selection.
2. Click more regions in the same sketch. Selected areas are highlighted and numbered, and the task card shows the total. Click a selected region again to remove it. Once selection has started, ordinary clicks also add or remove regions.
3. Choose New body, Join or Cut, and choose the target body for Join/Cut.
4. Click Extrude selected or press Enter to start one shared preview. Type a distance, choose the direction and extent, then confirm. All selected regions use those settings.

New body: regions sharing an edge merge into one solid without internal dividing walls. Disconnected regions, including regions that only touch at a corner, create separate bodies. The task card reports how many bodies will be created. Each resulting body has its own editable extrusion after creation.

Join and Cut: the entire selection is stored as one feature on the target body. Joined areas must connect to that body or another area in the same Join. A floating result is rejected. A Cut can remove material in several separated areas at once. The complete result is checked before anything is committed.

Unselected holes remain holes; selecting the enclosed inner region as well fills that opening in the combined extrusion. Distance, negative or symmetric directions, Through all for Cut, and Up to face share the normal extrusion controls. Orbit and pan remain available during selection and preview.

Use Change selected regions during the preview to return to the selection. Clear selection or Esc clears a pending selection. A plain click with no pending selection retains the original single-region workflow.

One Undo reverses the entire creation, including all bodies in a disconnected New body result. Save/open retains every selected region reference. Editing a dividing line rebuilds the combined result while its references remain valid; missing, split or merged source regions report a rebuild issue. Select up to 128 regions from one sketch per operation; selections across multiple sketches are not supported.

05 - EXTRUSION EXTENT

Choose Distance or Through all or Up to face

• Distance: use a fixed numeric length. Move the pointer or type a signed value.
• Through all: available for Cut. The depth is recalculated from the target's preceding solid, with a small clearance beyond its far boundary. Positive or Negative cuts from the sketch in that direction; the two-sided direction covers both sides. Changing earlier dimensions updates the required depth.
• Up to face: choose the mode, then click a planar end face parallel to the sketch plane. Orbit or use view buttons to reach the intended face. The direction is set toward the selected face, and the extrusion ends at its supporting plane. Changing the referenced earlier geometry updates the length.

The displayed length for an adaptive extent is calculated, not a second editable distance. Up to face uses the face's plane; it does not trim the extrusion sideways to the end face's outline.

In the saved feature's inspector, use Extent to return to Distance or Through all. The Up to face selector lists eligible parallel end faces and their signed distances. Missing, coincident, nonparallel or circularly dependent references cannot produce a valid preview.

06 - EXACT ENTRY

Direction and distance

For a fixed sketch extrusion, Positive and Negative use one side of the sketch plane. Symmetric divides the fixed length across both sides. Up to face uses one direction only.

For a direct solid-face edit, positive means outward and negative means inward. Its normal follows a moved or rotated body. Dragging follows the face normal as it appears in the current view, including side and bottom faces. If you look directly along that normal, upward dragging increases the signed distance; orbit slightly to see the direction in space. Pointer movement uses 0.5 mm increments; hold Shift for 0.1 mm. Exact entry accepts a decimal point or comma, with nonzero face-edit distances from 0.001 to 100,000 mm.

Navigate during a preview: middle-drag to orbit, hold Shift while middle-dragging to pan, right-drag to pan, or use the wheel to zoom. These gestures work during both sketch extrusion and direct face Push/Pull. They hold the current distance and do not place the feature. Release the camera gesture and continue sizing from the same distance in the new view. Shift without a mouse navigation gesture still provides fine sizing.

Typing stops pointer sizing, so moving to the controls does not change the entered value. Adaptive sketch extents disable manual pointer sizing while retaining their calculated length.

07 - FINISHING

Keep modeling after Chamfer or Fillet or Shell

On an edited Extrude body, choose Chamfer or Fillet and select one straight convex edge between planar faces. Enter the bevel Distance or rounding Radius and choose Apply. Choose Shell and select a planar opening on a convex planar body; enter the inward wall Thickness.

These features rebuild from the current solid. Later face edits and face-attached sketch Join/Cut operations remain available. Their numeric sizes are editable in the object tree.

A useful order is: resize the block, add a bevel if wanted, shell the convex body, then add holes, pockets and compatible rounded edges. Rounding that breaks into an unrelated wall or cavity is rejected. See Chamfer, 3D Fillet and Shell for their specific limits and the separate controls retained for clean prismatic bodies.

08 - ASSOCIATIVE HISTORY

Editing and restoring your work

Sketch extrusions retain their profile, operation, direction and extent definition. Direct edits retain their referenced surfaces and signed distances. Finishing features retain their selected boundary references and size. The saved model contains definitions; display and export meshes are rebuilt.

Changing an earlier sketch or extrusion rebuilds downstream operations when their referenced faces still exist. For example, increasing the original 20 mm extrusion to 30 mm retains later +5 mm and +3 mm face edits, giving 38 mm overall.

Undo and Redo step through committed operations. Save/open preserves the history, and 3MF export uses the evaluated solid. Remove later dependent features and attached references before deleting their source.

CURRENT SCOPE

Supported combinations

• Planar face editing and face-attached sketch selection focus on Extrude-based bodies, including existing sketch Join/Cut and supported finishing histories
• Supported caps may contain holes; straight Rectangle/Line walls and uniquely identified planar result faces are selectable
• New sketch Join/Cut features support any sketch-plane orientation and can follow direct edits and finishing operations
• Through all is a Cut extent; Up to face currently requires a parallel planar target and uses its supporting plane
• Finishing on edited boundaries selects one continuous straight convex edge per Chamfer/Fillet feature; multiple features can be stored
• Shell on an edited boundary requires one convex body entirely bounded by planar faces and one planar opening; use it before concave pockets, holes or Fillets
• General curved-face offsets, curved-edge finishing, ambiguous disconnected patches, and general Loft/Revolve/Split-result face editing are not included
• Legacy specialized finishing features retain their original definitions and controls; newly selected features on edited boundaries use the current-solid workflow
• No-change cuts, missing or cyclic references, complete body removal, invalid boundaries and detected finishing collisions block Apply