Whet user guide, chapter 2, 2026-10-09
Modelling
Building and changing a solid: placing shapes, sketching, pushing and pulling faces, fillets and chamfers, booleans, the viewing and picking tools, and Scan to CAD. Dimensions are in millimetres and angles in degrees.
Placing a shape
Whet has five one-click shapes: Box, Cylinder, Sphere, Cone and Torus. There are three ways to place one.
- Right-click in the viewport. The menu lists the five shapes. The shape lands where the pointer was, on the face under it or on the ground. Its default size is twice the grid step.
- Drag. Pick a shape on the Tool Hub (below) and drag on the ground. The drag sets the footprint and a height. A box dragged from one corner to another gets that footprint. A sphere and a torus are lifted so they rest on the ground.
- Part > Primitives. This menu holds Box, Cylinder, Cone, Sphere, Ellipsoid, Tube, Wedge, Torus and Prism, each as a form where you type the sizes. All Kinds... lists every body kind Whet can build. Part also has Extrude, Revolve, Loft, Sweep and Helix, which make a shape from a profile.
A shape needs a part session. If there is none, the item is greyed and the tooltip says that there is nowhere to put a body yet. Open or start a part first.
Sizes are checked as you type. A box side must be between 0.01 mm and 1,000,000 mm. A tube must leave a wall. A torus tube must be smaller than its ring. A refusal names the field and the limit.
Changing a shape's numbers
Select the shape in the Model Tree. Properties shows its fields. Type a new number and press Return. The part rebuilds and the info line gives the new volume. For example, a box changed to 60 by 20 by 10 mm reads 12000 mm3.
Double-click a row in the Model Tree to open its fields with the first number ready to edit.
The Model Tree
The Model Tree shows the part as the features that made it. Each row is a noun and its main figures, for example "Pad h8 taper 5" or "Boss r6 h10". Click a row and Properties shows that feature's fields. A click also lights the faces that feature made. Edit, Cut, Copy, Paste and Delete work on a body in a live part. Delete rebuilds the part without it, and Undo brings it back.
Sketching
A sketch is a 2D profile on a plane. You make it, solve it and then pad or pocket it.
Starting a sketch
- Sketch > New Sketch on XY, XZ or YZ starts on a datum plane.
- Sketch > New Sketch on Face (On Face in the SKETCH panel) starts on the picked flat face.
- Sketch > New Sketch at Vertex starts at a picked vertex. The sketch origin is that point.
- Sketch > Open Sketch... reopens a saved sketch.
- Sketch > Reorient moves an open sketch onto XY, XZ or YZ.
- Sketch > View Sketch turns the camera to look at the sketch plane.
Drawing
Sketch > Geometry holds the tools: Select, Line, Circle, Rectangle, Arc 3 Points, Arc Centre, Tangent Arc, Polygon and Slot. The Sketch panel shows the same tools under Draw.
- A rectangle takes two clicks, corner to corner. You can also type its sizes.
- A polygon has a Sides field. Polygon Mode chooses Inscribed or Circumscribed.
- A slot has a Slot radius field. It is two lines and two arcs.
- An arc takes three clicks: start, a point on the arc, then the end. Arc Centre takes the centre, the start and the end.
Each shape is written with the ties a careful drawing would carry. A rectangle drawn corner to corner is 4 lines and 8 ties, for example. You get a constrained profile and not loose lines.
Ellipses, splines, parabolas, hyperbolas, points, polylines and external geometry are not available. Trim, Extend, Split, Sketch Fillet, Offset, Mirror, Rotate and Scale are not available inside a sketch either. They are greyed with the reason. To round a corner of a finished profile, pad it and use Fillet on the solid.
Snaps
Sketch > Snap has Endpoint, Midpoint, Center, Perpendicular, Intersection and Tangent. The sketch's SNAP panel also carries a Grid snap. The first five are on by default. Hover over a line's midpoint and a small glyph under the pointer names the snap before you click. A snap also writes the tie it means, so a click on an endpoint joins the two ends.
Constraints and dimensions
Sketch > Constrain has Horizontal, Vertical, Parallel, Perpendicular, Tangent, Equal, Symmetric, Point on Object and Fix. Sketch > Dimension has Length, Radius, Horizontal Distance, Vertical Distance, Diameter and Angle. Pick the line or circle, choose the kind, type the number in the box that opens and press Return. Escape cancels.
Solve and degrees of freedom
Press Solve. The panel says how many degrees of freedom are left and names any constraints that conflict. A number above zero means the sketch can still move or change. You can pad it anyway. A rectangle padded with 4 degrees of freedom left is a fine solid. Pin the corner to the origin when its position matters.
Pad and Pocket
Set Depth and press Pad to add material, or Pocket to cut it. The button's tooltip shows what it will do, such as "Extrudes the solved profile by 10 mm". While the solver works, the panel says "Solving sketch..." and Pad waits. Press Finish to close the sketch. Save Sketch writes it to a file you can reopen.
Push and pull
Push/Pull moves a flat face along its normal. Pick a flat face, then choose Push/Pull Face from the right-click menu or press Push/Pull on the Tool Hub.
- Drag along the face's normal, or type a distance in the box that appears beside the face.
- Press Return. Escape puts the face down.
A positive distance pulls the face out of the part and adds material. A negative one pushes it into the part and cuts. Under the hood this is a sketch on the face followed by a pad or a pocket, so it appears in the Model Tree like any other feature, and Undo takes it back.
A face that is not flat is refused with a sentence such as "face 3 is a Cylinder, and a push or a pull moves a flat face". With no face picked it says to click a flat face first.
Direct editing
Direct editing changes faces of a part without going back to its sketches. Pick a face, then use the right-click menu or the Direct button on the Tool Hub.
- Move Face moves a face along a vector you type. It can also turn the face about one of its straight edges, by an angle.
- Offset Face moves a face along its own normal by a distance.
- Delete Face removes a face and closes the gap.
- Blend Faces joins two faces with a blend. It needs a part with at least two faces.
Each tool opens a small form with a preview. A report in the form shows what the edit would do. Apply stays greyed until the preview has solved. If the engine refuses, you read its sentence unchanged and nothing is changed. Apply makes one undoable step.
Fillet and chamfer
Pick the edge or edges to round. Press 2 to pick edges. Click within a few pixels of an edge and it lights. Add more with further clicks. Then press Fillet or Chamfer in the MODIFY panel, on the Tool Hub or in the Part Design menu.
A form opens over the picture.
| Field | Fillet | Chamfer |
|---|---|---|
| Method | Constant radius, or Start and end radii | Distance, or Distance and angle |
| Size | Start radius, 0.001 to 10000 mm | Distance, 0.001 to 10000 mm |
| Second size | End radius, for the second method | Angle, 0.01 to 89.99 degrees |
| Tangent edge chain | Tick to include edges that continue tangent | The same |
Each change starts a new preview, and the report box says "Building preview..." until it is ready. The Apply button stays greyed until the preview of the current values has solved. If you change a value while a preview runs, the old result is dropped. A preview that fails shows the engine's sentence and Apply stays off.
Part Design > Variable Fillet... is a separate form for a radius that changes along an edge.
As a check, rounding the four 10 mm vertical edges of an 80 by 40 by 10 mm plate at r 3 removes 77.26 mm3. Type the same edges and radius and compare the volume.
Booleans
A boolean combines two bodies. You need two bodies in the part. If you have one, the Boolean button says "Add two bodies to combine them."
Choose Part > Booleans or the Boolean button on the Tool Hub.
| Kind | What you get |
|---|---|
| Fuse | One solid from both |
| Cut | The first body less the tool body |
| Common | Only the volume they share |
| Compound | Both bodies kept, grouped together |
| XOR | Everything that is in one body and not the other |
| Slice | The first body cut into pieces by the tool |
On the Tool Hub form, you choose Keep body and Tool body from lists, and the Method. The form previews the result and Apply waits for it, as for fillets. The form's method list has Fuse, Cut, Common, Xor and Slice. Compound is on the Part > Booleans menu and in the MODIFY panel's list.
For example, an XOR of two 20 mm cubes placed 10 mm apart gives 8000 mm3 in 2 solids.
A slice whose tool misses the body is refused with a sentence that says there are no pieces. Nothing is built and the part stays as it was.
Tolerance and retry
Additional tolerance (0 to 1 mm) lets the boolean merge geometry that is nearly touching. Booleans on parts that almost touch can leave small slivers. When the preview reports a small result solid, Retry Fuzzy Boolean raises the tolerance and previews again. The form warns that tolerance may merge nearby geometry, so inspect the preview. The limit is 1 mm.
Boolean Fragments, Slice Apart, Connect, Embed and Cutout are on the menu, greyed.
The feature group
Part Design holds features that act on a face or on the whole part. Each opens a form for its kind. In the command row, Hole is in CREATE, Thickness in MODIFY and the patterns in PATTERN; Body Pattern, Edit Spec, Recompute and Build Part are in their panels' lists.
- Hole has the ISO table, with counterbore and countersink.
- Boss adds a cylinder on a face. Dome adds a spherical cap.
- Groove cuts a groove around a round shaft.
- Thickness hollows a part and leaves a wall. Tick the faces to leave open. With no face ticked it is refused.
- Draft tilts faces by an angle.
- Mirror, Scale, Offset (a 3D offset of the whole part), Linear Pattern, Polar Pattern and Pattern... repeat or reshape. Offset, Thickness, Mirror and Scale are also in the Part menu.
- All Features... lists every feature kind.
You name a face by its role (top, bottom, +x and so on) or pick it in the viewport. The picked face comes first in the list.
Examples you can reproduce on an 80 by 40 by 10 mm box: Hole M6 tap, 8 deep, leaves 31842.92 mm3. Boss r6 h10 on top gives 33130.97 mm3. Dome r6 h3 on top gives 32183.78 mm3.
Pocket with Taper, MultiTransform, Involute Gear and Sprocket are on the menu and greyed, with the reason in the tooltip.
Picking: keys 1 to 4
The viewport has four pick modes.
| Key | Picks |
|---|---|
| 1 | Vertices |
| 2 | Edges |
| 3 | Faces |
| 4 | Bodies |
The keys change what a click selects. They do not move the camera. View > Pick Filter offers the same choices with Any. The filter you set stays on until you change it.
A picked vertex shows its coordinates in Properties. Two picked vertices give the distance between them. A picked face or edge shows its size and kind.
Other keys in the viewport:
- V, then F fits everything in view.
- Frame Selection is F in the Whet and Unreal navigation styles, and V, then S in the FreeCAD and Gesture styles.
- Delete or Backspace removes selected sketch entities.
- Save, Open, Undo and Redo use the usual keys: Command on macOS, Control on Windows and Linux.
- A field that has the keyboard owns its editing keys, so typing a number never fires a viewport key.
The Tool Hub
The Tool Hub is a small floating panel of the modelling tools over the picture. View > Tool Hub shows or hides it. Drag its grip to move it. It stays inside the picture and comes back where you left it.
It holds the five shapes, Push/Pull, Direct, Fillet, Chamfer, Boolean, Colour and Sketch. Each button runs the same action as the menu item of the same name. A greyed button has the reason in its tooltip: no face picked, no edge picked, fewer than two bodies.
The Colour button paints the selection. The Sketch button starts a sketch on a plane or on the picked face.
Looking at the part
- View > Standard Views has Home, Isometric, Front, Back, Top, Bottom, Right and Left. Projection switches between Orthographic and Perspective.
- View > Draw Style has Points, Wireframe, Hidden Line, No Shading, Shaded and Flat Lines.
- The navigation cube in the corner names each face. Click a face and the camera turns to it. The mouse and touch schemes (Whet, FreeCAD, Gesture and Unreal) are in Settings > Whet > Viewport > Navigation.
A clipping plane for sectioning the live view is not available. A section as a drawing is in Drawings and measuring.
Scan to CAD
A scan is a mesh of triangles. You cannot fillet it or use it as a solid. Scan to CAD builds B-spline curves and NURBS surfaces over it and sews them into a STEP file. The kernel makes every curve and surface.
Where the commands are
Surface > Import Scan... reads a scan from a .stl, .obj or .ply file. The scan opens as a reference you cannot edit, and a Scan panel appears at the left of the viewport. While a scan is open the ribbon shows five panels, in the order you work:
| Panel | Commands |
|---|---|
| SCAN | Import Scan, Close Scan |
| CURVE | Curve on Scan, Section Curve |
| SURFACE | Fit Surface, Loft, Sew |
| EDIT | Control Points, Increase Control Points, Decrease Control Points |
| ANALYZE | Deviation, Zebra, Curvature |
The Surface menu holds the same commands. A greyed command gives the reason in its tooltip, for example that no surface is current.
The Scan panel also sets the Tolerance (0.1 mm to start), the scan's Opacity, and the Section axis and offset. Its CURVES and SURFACES lists show what you made. Tick a row to use it in the next command. Hover over a row to see its size and control points.
Curves
- Curve on Scan. Press it, click points on the scan, then press it again. Whet fits a curve through the points within the tolerance.
- Section Curve. Cuts the scan with the plane set in the panel, for example Z at 12 mm, and fits a curve to the cut. If the plane misses the scan, it says so.
Each new curve reports its length, its control points, the largest distance from your points, and whether the tolerance was met.
Surfaces
- Fit Surface. With three or more curves ticked, it fits a surface through them. Otherwise drag a rectangle over the scan; the rectangle must hold at least 16 scan points. Whet adds control points until the surface is within the tolerance or the limit is reached. A fit that misses the tolerance says "not met" and keeps the closest surface.
- Loft. A surface through two or more ticked curves.
- Sew. Joins the ticked surfaces into one shell. If the shell closes, it becomes a solid. Sew writes a .sewn.step file and a record beside it, and reports faces, free edges and, for a solid, the volume.
Editing and checking
- Control Points shows the control net of the current surface. Drag a point to reshape the surface; the kernel checks that the face is still valid.
- Increase Control Points adds one point in each direction without changing the shape. Decrease Control Points refits with one fewer and says how far the surface moved.
- Deviation colours the surface by its distance from the scan. Zebra shows stripes for checking smoothness. Curvature colours by curvature. Only one of the three is on at a time, with its legend in the panel.
What Scan to CAD does not do yet
- There is no cap command. An open end of a surface cannot be closed with a flat or filled face here.
- Surfaces fitted one by one do not sew into a closed shell unless they share curves. Build neighbouring surfaces from the same curves, with Loft or Fit Surface. Otherwise Sew leaves free edges and writes an open shell, not a solid.
Limits
- Datum planes, lines and points, a coordinate system, Refine Shape, Defeaturing and Shape from Mesh are not available.
- The sketcher draws lines, circles, arcs, rectangles, polygons and slots. It does not trim or offset.
- A push or a pull works on flat faces only.
- Parts export as STEP and STL. See Import and export.
More are listed in Known limits.