What it will not do

This page is worth a read before you start something you have a deadline on. Each entry says what happens, and the way round it where there is one.

None of it is a bug report. This is the shape of the tool as it stands.

Modelling

The last body cannot be deleted. A document is always at least one sketch, so the × on the only body is greyed. Press Clear to start the document over.

An export takes the whole visible model. There is no per-body export, so hide the bodies you do not want and then export.

Exclusive-or does not exist. Join, cut and keep-shared are the three booleans offered, between bodies and (as add, cut, intersect) on a feature. Compose the fourth from a join and a cut.

Cut is only offered on a sketch drawn on a face. A base sketch on the world plane always adds, and the toggle is hidden. Pick a face, press Sketch on face, and draw the cut there.

Midplane is ignored for cuts. The checkbox has no effect on a cut, because a cut is positioned by the face it is drawn on.

Features cannot be reordered. The build order is creation order. Rolling the marker back sets how much of that order is built; it does not change it.

A new feature always lands at the end. Making one while the marker is rolled back returns the marker to the end of the list instead of inserting there.

Blends always apply after every extrude, wherever their row sits.

A turn that folds into a body is narrower than one standing alone. A revolve joining or cutting into existing material must stand clear of its own axis, stop short of half a turn, and have no hole in its profile. Each is a refusal with a sentence rather than a wrong solid. Turning the shape as a New body and combining it afterwards has none of those limits.

A revolve has no taper and no second side. A turn is one angle about one line. There is no midplane, no start offset and no two-sided sweep, because none of them is measured in degrees.

A circular pattern turns about a world axis through the origin. Repeating something round a picked edge is not here. Move the body so the origin sits where the centre belongs.

A pattern makes at most 256 instances, and a mirror of a patterned body is not built. Mirror first, then pattern.

No sheet metal, no surfacing, no simulation, no drawings. All four are absent, and none of them is half finished.

Assemblies go as far as joints and no further. One body can be held against another, and moving the holder carries what it holds, but a body takes one joint only, nothing stops parts passing through each other, and there is no constraint solver looking for a position that satisfies several requirements at once.

Blends

A rim blend takes the outer boundary only. A hole through the face keeps its sharp rim. To round the hole as well, pick one of its own edges and ask for the Loop reach.

A rim that turns a corner into a round wall cannot be rounded, for instance the cap of a sector. Chamfering the same rim works, and so does rounding those edges one at a time.

A chain cannot cross between faces. You cannot ask for one blend that runs around a boss instead of along a single face's boundary. Blend each face's boundary separately.

A cylinder whose axis crosses the edge is refused. There is no workaround.

A taper only works on a single edge. Ticking Taper along the edge pins the reach to Edge, because a run of several edges has no one parameter to run the size along. Taper each edge of the run separately and match the ends by hand.

Blends that fall back are not exactly tangent. Most blends are exact. Where the precise route cannot be taken, a fallback runs whose result starts about 4.5% of the radius early, leaving up to 0.09 mm of discrepancy and a crease of roughly 2.6 degrees. Two such chamfers meeting at a corner leave a spike of about 1.1 mm³. Prefer a rim blend over two edge blends wherever both would do, since one pass mitres the corner properly.

Blends cannot be positioned in the timeline. An edge does not exist until both its faces do, so blends are always last.

See blends.

Faces and references

A re-attach loses any projected reference geometry. Repairing a stale reference from the flagged row moves the sketch and everything you drew on it, but the projection is dropped: it named curves on the old host, which say nothing about the new one. Project again once the sketch has landed. See face references.

Curved faces cannot host a sketch. The cylindrical wall of a boss is one curved face and refuses.

In the perspective view, a sketch overlay can look offset from the solid. The overlay is drawn on the sketch plane, and the face you are looking at is one extrude away from it, so the two drift apart the further they sit from the centre of the view. Switching the projection back to orthographic, which is the default, has no parallax and draws them registered; so does working in the 2D sketch view.

Interface

Undo resets when you switch sketches. Clicking another timeline row, pressing New body, pressing Sketch on face, or importing all clear both undo and redo, so finish what you are doing before switching.

Undo does not cover everything. Extrudes, blends, part colours, and dimension annotation positions are outside the history. Removing a feature or a blend cannot be undone.

Clear asks for no confirmation and cannot be fully undone.

Dragging in the 3D view moves points only. Whole entities have to be moved in the sketch view.

A sketch drawn in the 3D view is drawn OVER the solid, never behind it. It belongs to the plane you are working on, so it shows through whatever is in front of it.

Dimensions are not displayed on a sketch plane in 3D.

Projecting reference geometry covers points and lines only. Circles and arcs from the parent sketch are not projected.

The theme is light or dark and nothing else. It starts at whichever your machine asks for, the half-moon in the top bar swaps it, and the choice is remembered from then on. There is no third theme and no way to set your own colours.

A phone is too small for it. A tablet works: the document panel starts put away, one finger draws and two pan and zoom. Below about ten inches the drawing area left over is too small to place anything accurately, and nothing in the interface is laid out for a column that narrow.

Parameters drive dimensions, extrudes and blends, and nothing else.Named values reach every field that stores a number of its own. Point X and Y are solver output and take arithmetic without keeping it, and a tapered blend's far end has no field to drive.

A parameter edit is not undoable. Undo works on sketch geometry; the parameter table sits outside it, so typing the old value back is the way out.

Files and export

STL, OBJ and STEP are the exports. No IGES, DXF, SVG, or 3MF. STEP is the one that carries the solid, so it is what to hand another CAD tool or a shop.

Sketch geometry cannot be exported on its own. Only the solid.

Exports carry no colour or materials. OBJ writes a normal per vertex, so a curved face keeps the smooth shading it has on screen. STL has one normal per facet and cannot. Neither carries the colours you paint bodies with.

Curves are approximated as polygons in a mesh export. A hole leaves in STL or OBJ as a many-sided prism. STEP carries the true curved surface, though a bore goes out as an exact rational B-spline rather than as STEP's own cylinder entity, so a reader that recognizes holes by looking for cylinders will not fire on it.

A body imported as a mesh cannot be exported to STEP. There is no real geometry behind it. The export says which bodies it left out and writes the rest.

Work is kept by saving it. Save writes the whole document to a file you keep, and that file is the only copy that outlives this browser. The browser holds the open document as well and offers it back after a closed tab or a crash, but it holds exactly one, only on this machine, Clear drops it, and a document carrying a large imported file can be too big for it to hold at all. It says so when that happens.

There is no document list and no revision history. Opening an earlier version of a part means having saved it as its own file.

See export formats and saved files.

Import

Imports arrive under-constrained on purpose. Check the flagged dimensions and finish the constraining yourself. This is about the three doors that produce a sketch; a solid arrives finished and is not constrained at all.

From a STEP file

An imported solid cannot be edited. The file is the shape, so there is no dimension to change and no Timeline row to change it from. A boolean can be aimed at it, provided the report says can be cut into.

An imported face hosts a sketch by where it LIES, not by what made it. Nothing swept it and no sketch curve is behind it, so the reference is its plane. Two flat faces in the same plane pointing the same way (the far side of a slot) cannot be told apart, and the first is taken.

An assembly's parts arrive placed, and holding them together is up to you. Each part arrives where the file says and can be hidden, painted, renamed, cut into or deleted on its own. Nothing in the file says which parts are fastened to which, so a joint between two of them is something you make rather than something that is read. Hierarchy is flattened, and colours and materials are not read.

Foreign solids are often not watertight, and the report says when one is not. Such a part displays and measures correctly, but its volume is an estimate and an exported mesh of it will not print without repair first.

Wireframe and surface-only files are refused, since they declare no shells.

The unit is read out of the file and can be got wrong. If a part arrives a thousand times too small it was written in metres; set the units by hand and read it again.

From a 2D file

Only 2D formats are read: DXF, Gerber, Excellon drill files, and IDF board files.

An IDF board reads as profiles. Component outlines come from the paired library file (.emp); pads, copper, keepouts and component heights are left out. Without the library the board still reads as its blank, and the report counts the placements that were left out.

A DXF's splines are approximated. There is no spline in the sketcher, so one arrives as straight segments through the curve. Everything else about a DXF is read exactly. If the shape to the eye is enough, that is the end of it; redraw the curve as arcs if it is not.

Text, hatching and ellipses are left out of a DXF, counted in the report. An ellipse has no sketch entity, and neither does a circle squashed by a block placed at different scales in x and y.

Binary DXF is refused. Re-export it as ASCII.

A Gerber is read along the centre line of its traces. That is the right reading for an outline layer and the wrong one for a copper layer.

Two things about a file can be ambiguous, and both are reported rather than guessed at quietly: a DXF that declares no units is read as millimetres, and a drill file with no decimal points and no stated zero suppression is read one particular way. Each note names the assumption it made.

From a mesh file

A mesh never comes back as the part. STL and OBJ hold triangles and nothing else: the surfaces the part was made of were thrown away when the file was written. What is recovered is the flat regions and their outlines, one of which becomes a sketch, and the triangles themselves, which stand in the model as a body. Neither is editable geometry. STEP is the format for a file that still knows what it is.

A mesh body cannot be cut into. It shows, it measures, and it hosts a sketch on any flat face, and no feature or combine can be aimed at it. Turning triangles back into a solid is not something this does.

A mesh file is one body however many pieces it draws. Nothing in the file says where one part ends and the next begins, so six loose pieces arrive as one body holding six loose pieces.

Only one region at a time. Read the file again to trace a second face.

Nothing traced is dimensioned. The numbers in a mesh are a tessellation away from the ones the part was designed to, so a bore that measures 6.998 was a 7. The geometry is placed and left free, since dimensioning it would put numbers nobody chose into the sketch.

A coarse mesh is read as the polygon it has become. A ring of facets turning more than about 22 degrees at a time is no longer evidence of a circle, so a hexagonal hole stays a hexagon. Above sixteen facets to a turn a bore comes back as one circle of the right radius.

A mesh file states no unit, so millimetres is assumed and the reported size is how you check it. An inch file read as millimetres arrives 25 times too small.

From an image

There is no image import. A photograph or a scanned drawing cannot be turned into a sketch. Bring the part in as a geometry file, a mesh or a STEP file, or describe it directly in the importer's text area.

See the import dialog.

Speed

Curved cuts are far slower than straight ones, by roughly a hundred times. A round hole through a part can take seconds where a square one is instant.

Opening a saved document is as slow as building it, because the solid is rebuilt from the features instead of being stored.

A stack of features with curved cuts occasionally fails the modelling kernel outright. It is restarted automatically, with a message naming the stage; after three restarts it asks you to reload. Simplifying the offending feature clears it, such as a slot in place of a round hole.

See rebuilds and speed.