diff --git a/doc/reference.txt b/doc/reference.txt
new file mode 100644
index 0000000..28107ed
--- /dev/null
+++ b/doc/reference.txt
@@ -0,0 +1,553 @@
+
+General Navigation
+
+ Model View
+
+ To pan the view, center-drag with the mouse. (The center button
+ is typically actuated by pressing on the scroll wheel.)
+
+ To rotate the view, right-drag with the mouse. This will rotate
+ the part about a horizontal or vertical axis. To rotate the part
+ within the plane of the screen, Ctrl+right-drag with the mouse.
+
+ To zoom in or out, rotate the scroll wheel. It is also possible
+ to zoom in or out by using the View menu, or the associated
+ keyboard shortcuts (+ and -).
+
+ It is also possible to pan by Shift+right-dragging, or to rotate
+ by Shift+center-dragging. This makes MechSketch usable on certain
+ laptop keyboards that don't provide a center mouse button.
+
+ If a workplane is active, then choose Sketch -> In Workplane (or
+ press W) to align the view to the workplane. After doing this,
+ the plane of the screen is coincident with the workplane.
+
+ Dimension Entry and Units
+
+ Dimensions may be displayed in either millimeters or inches.
+ Millimeter dimensions are always displayed with two digits
+ after the decimal point (45.23), and inch dimensions are always
+ displayed with three (1.781).
+
+ Choose View -> Dimensions in ... to change the current display
+ units. This does not change the model; if the user changes from
+ inches to millimeters, then a dimension that was entered as 1.0
+ is now displayed as 25.40.
+
+ All dimensions are entered in the current display units. In most
+ places where a dimension is expected, it's possible to enter an
+ arithmetic expression ("4*20 + 7") instead of a single number.
+
+ Show / Hide Entities
+
+ As the sketch becomes more complex, it may be useful to hide
+ unnecessary information. MechSketch provides several different
+ controls for this.
+
+ In the second and third line of the text window, links are
+ provided to hide and show different types of entity. These are:
+
+ wrkpls -- When a new "Sketch In New Workplane" group is
+ created, an associated workplane is created
+ automatically. If wrkpls is hidden, then that
+ workplane is visible only when its associated
+ group is active. If wrkpls is shown, then the
+ workplane is always visible.
+
+ normals -- By default, normals are drawn as blue-grey arrows,
+ in the direction of the normal. These normals may
+ be hovered and selected with the mouse, for
+ example in order to constrain them. This link
+ may be used to hide them.
+
+ points -- By default, points are drawn as green squares.
+ These points may be hovered and selected with the
+ mouse, for example in order to constrain them.
+ This link may be used to hide them. If points are
+ hidden, then they will still appear when the mouse
+ hovers over them, and may still be selected.
+
+ constraints - When a constraint is created, a graphical
+ representation of that constraint is displayed
+ in purple. The constraints in a group are
+ visible only when that group is active. To hide
+ them even then, use this link.
+
+ shaded -- The 3d part is displayed as an opaque solid,
+ with lighting effects to give the impression of
+ depth. This link may be used to disable that
+ view.
+
+ faces -- Some surfaces on the 3d model may be selected.
+ For example, the user can select a plane face
+ of the part, and constrain a point to lie on
+ that plane. If faces are shown, then the faces
+ will appear highlighted when the mouse hovers
+ over them. The user can click the mouse to
+ select the face, as they would for any other
+ entity.
+
+ As a convenience, faces are automatically
+ hidden when a new sketch group is created,
+ and automatically shown when a new extrusion is
+ created. If this behavior is not what's desired,
+ then the faces can be shown or hidden manually
+ with this link.
+
+ mesh -- The 3d model of the part consists of many
+ triangles; for example, a flat polygon with
+ n sides is broken down into n - 2 triangles.
+ Use this link to show the triangles on the
+ model. In general, this is useful only for
+ debugging, or to see how fine the mesh is
+ before exporting it.
+
+ hidden-lines - With the part in a given orientation, some of
+ the lines in the part will be invisible,
+ because an opaque solid is between the line and
+ the "camera". To show those lines anyways, as
+ if the part were transparent, use this link.
+ This may be useful when creating a sketch that
+ lies within the volume of the part.
+
+ In addition to the above options, it is possible to hide and show
+ entire groups. If a group is hidden, then all of the entities
+ (line segments, circles, arcs, points, etc.) from that group
+ are hidden.
+
+ To hide a group, go to the home screen in the text window, by
+ pressing Esc or choosing the link at the top left. A list of
+ groups is displayed, along with their visibility. If a group is
+ visible, then the "show" column contains the word "yes" in green.
+ Click the "yes"; it now appears as a greyed "no", and the group
+ is hidden.
+
+ The show / hide status of groups is saved in the part file. If
+ a part is imported into an assembly, then entities that were
+ visible in the part file will be visible in the assembly, and
+ entities that were hidden will be hidden.
+
+ Active Workplane
+
+ MechSketch represents all geometry in 3d; it's possible to draw
+ line segments anywhere, not just in some plane.
+
+ This freedom is not always useful, so MechSketch also makes it
+ possible to draw in a plane. If a workplane is active, then all
+ entities that are drawn will be constrained to lie that plane.
+
+ When MechSketch starts with a new empty file, a workplane parallel
+ to the XY plane is active.
+
+ Active Group
+
+ Any groups that go after the active group will be hidden
+
+
+
+Sketch Entities
+
+ Datum Point
+
+ Workplane
+
+ Line Segment
+
+ Rectangle
+
+ A rectangle consists of two vertical line segments, and two
+ horizontal line segments, arranged to form a closed curve.
+ Initially, the rectangle is specified with the mouse by two
+ diagonally opposite corners. The line segments (and points)
+ in the rectangle may be constrained in the same way as ordinary
+ line segments.
+
+ It would be possible to draw the same figure by hand, by drawing
+ four line segments and inserting the appropriate constraints. The
+ rectangle command is a faster way to draw the exact same thing.
+
+ A workplane must be active when the rectangle is drawn, since
+ the workplane defines the meaning of "horizontal" and "vertical".
+
+ Circle
+
+ Arc of a Circle
+
+ Tangent arcs may be created automatically. To do so, first select
+ a point where two line segments join. Then choose Sketch ->
+ Arc of a Circle; the arc will be created, and automatically
+ constrained tangent to the two line segments.
+
+ The initial line segments will become construction lines, and
+ two new lines will be created, that join up to the arc.
+
+ The arc's diameter may then be constrained in the usual way, with
+ Distance / Diameter or Equal Length / Radius constraints. This
+ is a simple way to round a sharp corner.
+
+ Bezier Cubic Segment
+
+ Text in a TrueType Font
+
+
+Constraints
+
+ General
+
+ Reference Dimensions
+
+ By default, the dimension drives the geometry. If a line segment
+ is constrained to have a length of 20.00 mm, then the line
+ segment is modified until that length is accurate.
+
+ A reference dimension is the reverse: the geometry drives the
+ dimension. If a line segment has a reference dimension on its
+ length, then it's still possibly to freely change that length,
+ and the dimension displays whatever that length happens to be. A
+ reference dimension does not constrain the geometry.
+
+ To change a dimension into a reference dimension, choose
+ Constrain -> Toggle Reference Dimension. A reference dimension
+ is drawn with "REF" appended to the displayed length or angle.
+ Double-clicking a reference dimension does nothing; the dimension
+ is specified by the geometry, not the user.
+
+ Angle
+
+ When two lines intersect, four angles are formed. The
+ opposite angles are equal; to change which opposite angle is
+ displayed, drag the label, and the arc will follow. If the wrong
+ supplementary angle is displayed, then select the constraint
+ and choose Constrain -> Other Supplementary Angle.
+
+ Comment
+
+ A comment is a single line of text that appears on the drawing.
+ When the comment is created, it appears in the center of the
+ screen. To move the comment, drag it with the mouse. To change
+ the text, double-click it.
+
+ The comment has no effect on the geometry; it is only a
+ human-readable note.
+
+
+Groups
+
+ General
+
+ All groups have a name. When the group is created, a default name
+ (e.g., "g008-extrude") is assigned. The user may change this name;
+ to do so, go to the group's page in the text window, and choose
+ [rename].
+
+ Groups that create a solid (e.g. extrudes or sweeps) have a "MERGE
+ AS" option, which is displayed in the page in the text window.
+ The group can be merged as union, which adds material to the
+ model, or as difference, which cuts material away.
+
+ The group's page in the text window also includes a list of all
+ requests, and of all constraints. To identify a constraint or a
+ request, hover the mouse over its name; it will appear highlighted
+ in the graphics window. To select it, click on the link in the
+ text window. This is equivalent to hovering over and clicking
+ the actual object in the graphics window.
+
+
+ Sketch in 3d
+
+ Sketch in New Workplane
+
+ A point and two line segments
+
+ The new workplane has its origin at the specified point. The
+ workplane is parallel to the two lines. If the point and
+ two are two edges on a plane face of the part, and a vertex
+ on that plane face, then the resulting workplane will be
+ coincident with that face (i.e., the user will be drawing
+ on that face).
+
+ A point
+
+ The new workplane has its origin at the specified point. The
+ workplane is orthogonal to the base coordinate system; for
+ example, its horizontal and vertical axes might lie in the
+ +y and -z directions, or +x and -z, or any other combination.
+
+ The orientation of the workplane is inferred from the
+ position of the view when the workplane is created; the
+ view is snapped to the nearest orthographic view, and the
+ workplane is aligned to that.
+
+ If a part consists mostly of ninety degree angles, then this
+ is a quick way to create workplanes.
+
+ Step Translating
+
+ Step Rotating
+
+ Extrude
+
+ If a workplane is active when the group is created, then the
+ extrude path is automatically constrained to be normal to that
+ workplane. This means, for example, that a rectangle is extruded
+ to form a rectangular prism. The extrusion has one degree of
+ freedom, so a single distance constraint will fully constrain it.
+ This is usually the desired behaviour.
+
+ If no workplane is active when the group is created, then the
+ extrude path may be in any direction. This means that a rectangle
+ could be extruded to form a parallelepiped. The extrusion has
+ three degrees of freedom. This is not typically useful.
+
+ Lathe
+
+ Sweep
+
+ Helical Sweep
+
+ Import / Assemble
+
+ In MechSketch, there is no distinction between "part" files and
+ "assembly" files; it's always possible to import one file into
+ another. An "assembly" is just a part file that imports one or
+ more other parts.
+
+ The imported file is not editable within the assembly. It is
+ imported exactly as it appears in the source file, but with an
+ arbitrary position and orientation. This means that the imported
+ part has six degrees of freedom.
+
+ To move (translate) the part, click any point on the imported
+ part and drag it. To rotate the part, click any point and Shift+
+ or Ctrl+drag it. The position and orientation of the part may be
+ fixed with constraints, in the same way that any other geometry
+ is constrained.
+
+ The Same Orientation constraint is particularly useful when
+ importing parts. This one constraint completely determines the
+ imported part's rotation. (Select a normal on the imported part,
+ select some other normal to constrain it against, and choose
+ Constrain -> Same Orientation).
+
+ Import groups have a special "MERGE AS" option: in addition
+ to the usual "union" and "difference", they have "assemble".
+ The "assemble" option is identical to "union", except that
+ it displays a warning if the components intersect with each
+ other. This is useful when checking to see if the assembled parts
+ interfere. If the parts interfere, then a warning is displayed
+ underneath the "MERGE AS" line in the group's text window page.
+ The interfering surfaces are also highlighted in the graphics
+ window, in red with black stripes.
+
+ When an assembly file is loaded, MechSketch loads all of the
+ imported files as well. If the imported files are not available,
+ then an error occurs. When transfering an assembly file to another
+ computer, it's necessary to transfer all of the imported files
+ as well.
+
+
+Export
+
+ Bitmap Image
+
+ This option will export a bitmap image of whatever is displayed
+ on-screen. It is equivalent to taking a screenshot. This option
+ is useful for producing human-readable drawings.
+
+ Choose File -> Export Image. The file is exported as a PNG,
+ which most graphics software can open.
+
+ 2d Vector (DXF)
+
+ This option will generate a 2d vector file that represents a
+ specified plane in the part. Most 2d CAM software, including the
+ software that ships with laser or waterjet cutters, will accept
+ a DXF file.
+
+ Before exporting a DXF, it is necessary to specify which plane of
+ the part should be exported. This may be specified by:
+
+ a face:
+
+ Any surfaces coplanar with that plane face will appear in the
+ file. The faces must be shown before they can be selected;
+ click the link in the third line of the text window.
+
+ a point, and two lines or vectors:
+
+ The export plane is through the point, and parallel to
+ the two lines or vectors. If the two lines or vectors are
+ perpendicular, then they will become the x and y axis in the
+ DXF file. Whichever line is more horizontal in the current
+ view becomes the x axis, and the other one becomes the y.
+
+ This means that it's possible to rotate the exported DXF
+ through ninety degrees by rotating the view through ninety
+ degrees (in the plane of that face). Similarly, by rotating
+ the part around to look at the face from behind instead of
+ in front, the exported DXF is mirrored.
+
+ the active workplane
+
+ If a workplane is active, and nothing is selected when the
+ export command is chosen, then MechSketch will export any
+ surfaces that are coplanar with the active workplane. The
+ workplane's horizontal and vertical axes become the x and
+ y axis in the DXF file.
+
+ The units of the DXF file are determined by the export scale
+ factor, which may be specified in the configuration screen.
+
+ 3d Mesh (STL)
+
+ This option will generate a 3d triangle mesh that represents
+ the entire part. Most 3d CAM software, including the software
+ for most 3d printers, will accept an STL file.
+
+ The mesh from the active group will be exported; this is the
+ same mesh that is displayed on screen. The coordinate system
+ for the STL file is the same coordinate system in which the part
+ is drawn. To use a different coordinate system (e.g., to rotate
+ or translate the part), create an assembly with the part in the
+ desired position, and then export an STL file of the assembly.
+
+ The units of the STL file are determined by the export scale
+ factor, which may be specified in the configuration screen.
+
+Configuration
+
+ Material Colors
+
+ In the text window screen for certain groups (extrude, lathe,
+ sweep), a palette of eight colors is displayed. This palette
+ allows the user to choose the color of any surfaces generated
+ by that group.
+
+ These eight colors are specified here, by their components.
+ The components go from 0 to 1.0. The color "0, 0, 0" is black,
+ and "1, 1, 1" is white. The components are specified in the order
+ "red, green, blue".
+
+ A change to the palette colors does not change the color of any
+ existing surfaces in the sketch, even if the color of an existing
+ surface no longer appears in the palette.
+
+ Light Directions
+
+ The 3d part is displayed with simulated lighting, to produce
+ the impression of depth. The directions and intensities of these
+ lights may be modified according to user preference.
+
+ The lights do not have a position; they have only a direction,
+ as if they were coming from very far away. This direction is
+ specified in 3 components, "right, top, front". The light with
+ direction "1, 0, 0" is coming from the right of the screen.
+ The light with direction "-1, 0, 0" is coming from the left of
+ the screen. The light with direction "0, 0, 1" is coming from
+ in front of the screen.
+
+ The intensity must lie between 0 and 1. A light with intensity
+ 0 has no effect, and 1 is full brightness.
+
+ Two lights are available. If only one is desired, then the second
+ may be disabled by setting its intensity to zero. When the part
+ is rotated or translated, the lights do not move.
+
+ Chord Tolerance
+
+ MechSketch does not represent curved edges or surfaces exactly.
+ Any curves are broken down into piecewise linear segments,
+ and surfaces are represented as triangles.
+
+ This introduces some error. The chord tolerance determines how
+ much error is introduced; it is the maximum distance between
+ the exact curve and the line segments that approximate it. If
+ the chord tolerance is decreased, then more line segments will
+ be generated, to produce a better approximation.
+
+ The chord tolerance is specified in units of screen pixels. This
+ means that when the user zooms in on the model, a better
+ approximation is produced.
+
+ The same tolerance is used for the mesh that's displayed on
+ screen, and for the mesh that is used to export to a file. It
+ may be helpful to use a large chord tolerance (2-5 pixels) while
+ drawing, for fast response, and then temporarily specify a small
+ chord tolerance (~0.5 pixels) before exporting an STL or DXF file.
+
+ Perspective Factor
+
+ To display a 3d part on-screen, it must be projected into 2d. One
+ common choice is a parallel projection. In a parallel projection,
+ any two lines that are parallel in real life are also parallel
+ in the drawing. A parallel projection is also known as an
+ axonometric projection. Isometric and orthographic views are
+ examples of parallel projections.
+
+ Another way to transform the image into 2d is with a perspective
+ projection. In a perspective projection, objects closer to the
+ "camera" appear larger than objects that are farther away. This
+ means that some lines that are parallel in real life will not be
+ parallel in the drawing; they will converge at a vanishing point.
+
+ A perspective projection will often look more realistic, and
+ gives a better impression of depth. The disadvantage is that
+ the perspective distorts the image, and may cause confusion.
+
+ By default, MechSketch displays a parallel projection. To display
+ a perspective projection, set the perspective factor to something
+ other than zero. The distance from the "camera" to the model is
+ equal to one thousand pixels divided by the perspective factor.
+
+ Edge Color
+
+ The surfaces of the 3d part are shaded according to the specified
+ lighting. Different faces will catch the light at slightly
+ different angles, and will therefore appear slightly brighter
+ or darker. This permits the viewer to distinguish the boundary
+ between the faces.
+
+ Depending on the lighting, this may not provided very much
+ constrast. To make the edges of the part more visible, it's
+ possible to emphasize them with a solid-color line.
+
+ If the edge color is specified as "0,0,0", then no emphasized
+ edges will be drawn. If any other color is specified, then the
+ edges will be drawn in that color. The edge color is specified
+ in the same format as for the material color.
+
+ Export Scale Factor
+
+ Internally, MechSketch represents lengths in millimeters. Before
+ exporting geometry to an STL or DXF file, these lengths are
+ divided by the export scale factor. This scale factor determines
+ the units for the exported file.
+
+ If the scale factor is set equal to 1, then exported files are
+ in millimeter units. If the scale factor is set equal to 25.4,
+ then the exported files are in inch units, since 1 inch = 25.4 mm.
+
+ MechSketch works in a right-handed coordinate system. If the
+ scale factor is negative, then the exported file will appear in
+ a left-handed coordinate system (so that a right-handed screw
+ thread will become left-handed).
+
+Licensing
+
+ As downloaded, MechSketch does not include a license file. This means
+ that it cannot create files with more than seven groups. Larger files
+ may be opened, but not modified. This light version of MechSketch
+ is intended for evaluation, but non-commercial / personal use is
+ also permitted.
+
+ The licensed version of MechSketch can create files with an unlimited
+ number of groups.
+
+ When a license is purchased, a license file ("mechsketch.license")
+ will be sent via email. To activate the license, save this file
+ somewhere on your computer. In MechSketch, choose Help -> Load
+ License... A file dialog box will appear; select the license file.
+
+ No license server or dongle is required, and licenses do not expire.
+
+
diff --git a/mesh.cpp b/mesh.cpp
index 68b7632..e72482e 100644
--- a/mesh.cpp
+++ b/mesh.cpp
@@ -593,7 +593,28 @@ void SKdNode::FindEdgeOn(Vector a, Vector b, int *n, int *nOther,
(a.EqualsExactly(tr->a) && b.EqualsExactly(tr->c)))
{
(*n)++;
- if(tr->meta.face != m.face) (*nOther)++;
+ if(tr->meta.face != m.face) {
+ if(tr->meta.face != 0 && m.face != 0) {
+ hEntity hf0 = { tr->meta.face },
+ hf1 = { m.face };
+ Entity *f0 = SS.GetEntity(hf0),
+ *f1 = SS.GetEntity(hf1);
+
+ Vector n0 = f0->FaceGetNormalNum().WithMagnitude(1),
+ n1 = f1->FaceGetNormalNum().WithMagnitude(1);
+
+ if(n0.Equals(n1) || n0.Equals(n1.ScaledBy(-1))) {
+ // faces are coincident, skip
+ // (If the planes are parallel, and the edge
+ // lies in both planes, then they're also
+ // coincident.)
+ } else {
+ (*nOther)++;
+ }
+ } else {
+ (*nOther)++;
+ }
+ }
}
tr->tag = cnt;