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Don't emphasize edges between coincident plane faces, and check in 

beginnings of reference manual.

[git-p4: depot-paths = "//depot/solvespace/": change = 1841]
solver
Jonathan Westhues 2008-07-15 21:45:11 -08:00
parent bc2a9c11b3
commit 3765175ec3
2 changed files with 575 additions and 1 deletions
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<h2>General Navigation</h2>
<h3>Model View</h3>
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.
<h3>Dimension Entry and Units</h3>
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.
<h3>Show / Hide Entities</h3>
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.
<h3>Active Workplane</h3>
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.
<h3>Active Group</h3>
Any groups that go after the active group will be hidden
<h2>Sketch Entities</h2>
<h3>Datum Point</h3>
<h3>Workplane</h3>
<h3>Line Segment</h3>
<h3>Rectangle</h3>
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".
<h3>Circle</h3>
<h3>Arc of a Circle</h3>
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.
<h3>Bezier Cubic Segment</h3>
<h3>Text in a TrueType Font</h3>
<h2>Constraints</h2>
<h3>General</h3>
<h3>Reference Dimensions</h3>
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.
<h3>Angle</h3>
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.
<h3>Comment</h3>
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.
<h2>Groups</h2>
<h3>General</h3>
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.
<h3>Sketch in 3d</h3>
<h3>Sketch in New Workplane</h3>
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.
<h3>Step Translating</h3>
<h3>Step Rotating</h3>
<h3>Extrude</h3>
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.
<h3>Lathe</h3>
<h3>Sweep</h3>
<h3>Helical Sweep</h3>
<h3>Import / Assemble</h3>
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.
<h2>Export</h2>
<h3>Bitmap Image</h3>
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.
<h3>2d Vector (DXF)</h3>
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.
<h3>3d Mesh (STL)</h3>
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.
<h2>Configuration</h2>
<h3>Material Colors</h3>
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.
<h3>Light Directions</h3>
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.
<h3>Chord Tolerance</h3>
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.
<h3>Perspective Factor</h3>
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.
<h3>Edge Color</h3>
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.
<h3>Export Scale Factor</h3>
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).
<h2>Licensing</h2>
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.

23
mesh.cpp
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@ -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;