tool reference

Model tools

Reference for every visible solid creation, modification, construction, pattern, and inspection tool.

Operations and confirmation#

Model tools show the selections they require and preview the result before commit. New Body creates a separate body. Join adds material to a target, Cut subtracts material, and Intersect keeps common volume. Automatic operation and target choices are starting suggestions; review the preview and set them explicitly when needed. Apply commits the feature to History; Cancel discards the staged operation.

Create solid features#

• Box and Cylinder create dimensioned primitive bodies. Gear creates a parametric involute spur gear using its gear type and dimensional settings.
• Coil creates a spring or coiled solid. The command bar shows Diameter and the two active definition values: Turns + Pitch, Turns + Height, or Height + Pitch. Details provides section size and shape, taper by end diameter, cone angle, or radial growth per turn, reference-derived diameter, angle or picked-point starts, calculated or picked-point ends, clockwise direction, axis reversal, variable-pitch stations, a flat spiral, inside/centered/outside section placement, and New Body/Join/Cut/Intersect results. Circular helical coils can use plain, closed, or closed-and-ground ends.
• Helix creates the same parametric helical, tapered, variable-pitch, or flat-spiral centerline as a reusable wire. Its command bar also shows Diameter and the two active definition values; axis and advanced path controls are in Details. Its axis and start radius can follow a circular edge or cylindrical/conical face. Select the generated edge as the path for Sweep when you need a custom sketch profile instead of a Coil section preset. After Sweep succeeds, MakerSolid hides the Helix wire while retaining it in History for associative editing; applying a Helix History edit rebuilds the linked Sweep. Use the visibility control under Wire Bodies to show the wire again.
• Extrude gives depth to selected closed sketch profiles or planar faces. Set distance, direction, symmetric behavior, operation, and target where shown.
• Revolve rotates a closed profile around a selected axis. Sweep carries a profile along a connected, tangent-chain, or explicitly selected path. Turn on Composite Path in Sweep Details to append separately selected sketch curves, model edges such as a Helix, or straight path pieces into one continuous unbranched path. Loft transitions through ordered profiles.
• Hole cuts a configured blind or through hole from a selected target location or face. Thread adds cosmetic or modeled standard threads to a supported cylindrical face. Newly created matching ISO Metric or Unified internal/external sizes use complementary 60° modeled profiles; the named size is the shared nominal major diameter, while the internal bore is resized to its catalog tap/minor diameter. Set Starts from 1 through 4 for equally phased multi-start threads; Lead is Pitch multiplied by Starts. Use the same standard, size, handedness, and starts on both parts, then add modeled Allowance for manufacturing or printing clearance. This geometry is intended to mate but is not a certified tolerance-class inspection model.

Thread also offers **Size from selected face** in Standard. The selected cylinder diameter sets the **Nominal diameter** for both external and internal threads, including after upstream diameter edits. Enter Pitch for complementary 60° metric-style profiles; this is not a catalog or tolerance-class specification. Internal threads extend inward: the entire selected bore is reduced to the derived minor diameter before grooves are cut, even at zero Allowance. Resize to Standard is hidden because sizing is automatic. For mating parts, use the same nominal diameter, pitch, handedness, and starts. Positive modeled Allowance adds radial clearance (smaller external threads, larger internal threads); allowance on both parts adds together and excessive clearance can remove engagement. New ISO Metric, Unified, and face-sized Modeled, External, Full Length threads default End to Chamfer to provide a usable entrance; choose None explicitly when an untreated end is required. Print a short mating test before a full container and lid. The preview wire shows placement and the derived internal opening, not the complete solid. Custom remains available for independent diameters and an included Angle. New 60° Custom threads use complementary truncated profiles on Internal and External sides when Modeled; enter the same major diameter, minor/tap diameter, pitch, handedness, and starts on both parts. Other Custom angles use their specified V groove. If the angle, diameters, pitch, and selected cylinder cannot form the requested profile, Apply reports an error instead of substituting another shape. End > Chamfer cuts a conical lead-in around each end of a Modeled thread and eases each groove into it, opening an internal bore entrance or reducing an external nose while leaving the middle of the groove at full depth. Older saved Custom threads retain their saved profile until you enable Matching 60° in History. New face-sized threads require project format 18; new Custom and complementary catalog threads require format 19. Previously saved catalog and **Use selected surface** threads keep their original profile and sizing modes; reopening or rebuilding a Modeled thread recalculates its groove angle and End Chamfer with the corrected geometry. Recreate both mating catalog threads to opt into the complementary catalog profile.

• Wrap maps a live sketch profile or connected path onto a planar, cylindrical, or conical face. Solid changes volume; Split imprints/splits the target face. The source and target remain associative history references.

For a matching 60° Custom pair, start with an outside cylinder for External and a cylindrical bore for Internal. Use the same Major Dia, Minor/Tap Dia, Pitch, Direction, and Starts on both Thread features. Keep **Resize to Standard** on when the cylinder needs to be brought to the specified diameter; turn it off for an internal bore already sized to Minor/Tap Dia. Modeled Allowance can be applied to either part or both, and the clearances add together. Choose End > Chamfer where the parts need a lead-in.

To adjust an existing thread's fit, open **History**, tap its pencil, set **Representation** to **Modeled**, edit **Allowance**, and select **Update Feature**. For an older 60° Custom thread, turn on **Matching 60°** to convert its saved V groove to the complementary shape; convert both parts of a matching pair. Previously saved shapes do not change just by opening a project. Allowance accepts nonnegative lengths or expressions in the document units. Cosmetic hides the field but keeps its saved value. Invalid values or failed geometry rebuilds leave the saved feature unchanged.

Selections must define valid geometry. Closed profiles cannot be self-intersecting. Sweep paths must form one unbranched ordered wire, and revolve, Coil, and Helix axes must be resolvable references. Picked start and end points must lie away from the axis, and the end must be ahead of the start along the selected direction. A solid Coil pitch must be at least its section height; reduce the section or increase pitch if the turns overlap. Variable pitch requires Turns + Pitch with a calculated end, a station at turn 0, and another at the total turn count.

Modify bodies#

• Transform moves, rotates, scales, or copies selected bodies. It can also reposition whole sketches or supported construction references.
• Fillet rounds selected body edges. Chamfer bevels selected edges. Values that consume or invalidate nearby geometry fail rather than committing an approximate result.
• Shell hollows a solid and opens selected faces. Press Pull offsets a selected planar or cylindrical face; on traceable modeled thread faces it edits thread allowance.
• Draft tapers planar side faces relative to a selected neutral plane. Split divides a body with a supported plane or face.
• Combine uses a target body and one or more tool bodies for Join, Cut, or Intersect. Review which bodies remain after the operation.

Position bodies#

Choose Model → Modify → Position to place or copy exact CAD bodies. Open Details, choose **Moving Bodies**, then choose a method from the command bar. Multiple moving bodies keep their relative arrangement; destination bodies stay fixed. **Selection Center** is the midpoint of the combined world-aligned body bounds, not the center of mass.

• **Coordinates** shows the current selection center in world X/Y/Z coordinates. Enter its destination or choose **Origin** for 0/0/0.
• **Point to Point** moves a source anchor to a destination without rotating. Anchors include selection/body centers, planar-face area centers, circular-edge centers, straight-edge midpoints, and the destination Origin. **World Offset** adds X/Y/Z distances after matching the anchors.
• **Align Centers** matches one reference body's center along enabled X/Y/Z axes. Disable X to keep two side-by-side bodies separated while lining up their Y and Z centers.
• **Between Bodies** positions the selection center halfway between two distinct reference body centers along enabled axes. This uses center spacing, not equal gaps between surfaces.
• **Align Faces** matches two planar-face area centers and rotates their outward normals to oppose. **Flip** makes the normals point in the same direction. Positive **Offset** separates the centers along the destination face's outward normal. **Rotation** turns the moving selection around that normal.

Use **Pick Moving Bodies** to toggle the moving selection in the viewport. For **Point to Point**, choose an **Anchor** type for Source and Destination. Selection Center and Origin need no geometry pick; Body Center offers a named body menu. Planar Face Center, Circle Center, and Edge Midpoint highlight eligible geometry for direct viewport selection. **Align Faces** uses **Source Face** and **Destination Face** picks. The pane explains what can be selected: sources on Moving Bodies, destinations on stationary bodies. Tap a highlighted reference to finish, or choose **Done Picking** to exit the picker. Selected references stay highlighted and show their body name. Rotate the view to expose hidden geometry; nearby taps are accepted for edges. Curved faces, arbitrary points, sketches, construction objects, and STL display references are not positioning inputs. A trimmed face's area center can lie outside its boundary.

**Copy Originals** keeps the originals and creates positioned bodies. Numeric fields accept expressions and explicit units. X/Y/Z are world axes in MakerSolid's Z-up system. Preview markers identify source and destination. **Apply** adds one Position History feature; **Cancel** discards the draft. Apply is disabled when the references are invalid or placement would not change.

Position remains linked to its references: upstream size and placement edits recompute the result. In History choose Edit to reopen the same controls using geometry before the Position feature. Missing or ambiguous references produce an error; reselect them or suppress/remove the Position feature. Failed updates leave the saved project unchanged. Projects containing Position require a MakerSolid version supporting project format 22.

Patterns#

Linear Pattern repeats selected bodies or features along a direction. Circular Pattern repeats them around an axis. Mirror reflects bodies or features across a plane. Set count, spacing or angle, direction, result operation, and target where the command presents those controls.

Construction and inspection#

Plane creates reference planes from the available placement method and selected references. Axis creates reference axes from supported geometry. Construction references can be used for sketches, patterns, mirrors, revolves, splits, directions, and other reference pickers.

Measure reports supported edge and face measurements without adding a modeling feature. Keep the measurement tool active while selecting the geometry you want to inspect.

Extrusion start and end conditions#

Distance remains the default in the Extrude command bar. Open **Details** to choose an end condition and use the grouped Start, Direction, Sides, End, Shape, and Result controls. Select the source profile first. The dedicated start, end, body, and direction pickers preserve that source selection; **Cancel Selection** exits the active picker. When there is only one eligible termination body, Up to Body selects it automatically. Choosing a face, plane, or body from a menu closes the active reference picker.

**Up to Face/Plane** stops on the selected trimmed face, including a curved loft face. The face must cover the whole swept profile. Use **Up to Body** when the end crosses a loft seam or several faces. Construction and world planes are infinite. **Up to Next** uses the first boundary, or the first exit when starting inside a candidate body. Next and **Through All** start with the currently visible bodies as candidates and save that set; hiding a body later does not change the result. Through All is available for Cut and Intersect. The boolean Target is separate from the termination reference. End Body and candidate-body choices use the same names shown in the Bodies browser, including renamed bodies.

**Start** offers Profile Plane, Offset, and Selected Face/Plane. An offset moves the source along the extrusion direction. A referenced start trims the sweep without wrapping the profile. **Direction** supports Profile Normal, Reverse Direction, world or construction axes, straight edges, and Explicit Vector. The direction must be nonzero and cross the profile plane. **Two Sides** has separate end and shape settings. **Symmetric** labels its distance per side.

**Clearance** can be measured Along Extrusion or Normal to Surface. Positive end clearance stops short; negative clearance extends beyond. Positive start clearance moves the start into the interval. Normal clearance uses an offset surface and rejects invalid or singular geometry.

For referenced ends, **Shape Reference Length** sets the axial station where End Scale and Twist reach their entered values. The deformation continues until the target trims it, and scale must remain positive throughout. A numeric start offset moves the deformation origin; a referenced start does not reset it. Distance mode retains its end-section interpretation. Numeric fields accept expressions.

Numeric parameters, including Distance, End Scale, Twist, and Clearance, show their labels above their inputs in the details pane and full Extrude History editor. A reversed extrusion uses **Reverse Direction** with a positive Distance. In **Your First Solid**, the History pane scrolls to the highlighted Distance input; change it, then select **Update Feature** to advance.

Apply and History's Update Feature require a successful current exact preview. Invalid inputs remain editable and do not change the committed project. Repair missing upstream references explicitly; History rejects construction planes and axes derived from the edited feature or later history. Use a larger face or body when coverage is incomplete, and reduce offsets or deformation when the exact geometry is invalid. Existing projects retain their legacy geometry; converting a legacy symmetric deformed extrusion uses an equivalent offset sweep to preserve its shape.