ref.pl

#!/usr/bin/perl

use TEMPL;
TEMPL::Init();

$TEMPL::TITLE = 'SolveSpace - Reference';
$TEMPL::SHOW_VERSION = 1;

TEMPL::OutputWithHeader("REFERENCE MANUAL", <<EOT

<p>This is a reference manual for SolveSpace. It is not intended as an
introduction to the program; for that, see the
<a href="tutorial.$TEMPL::PL">tutorials</a>.</p>

<h2><a id="General" href="#General" class="anchor"></a>
General Navigation</h2>
<div class="refind">

<p>
    The user interface consists of two windows: a larger window that
    contains mostly graphics, and a smaller window that contains mostly
    text. The graphics window is used to draw the geometry, and to view
    the 3d model. The Property Browser provides information about the model,
    and may also be used to modify settings and numerical parameters.
</p>

<h3><a id="Graphics" href="#Graphics" class="anchor"></a>
Graphics Window and Model View</h3>

<p>
    To pan the view, right-drag with the mouse.

<p>
    To rotate the view, center-drag with the mouse. This turns the
    part over, so that the surfaces that used to be hidden (because
    they were facing backwards, away from the viewer) become visible.

<p>
    To rotate the view within the plane of the monitor,
    Ctrl+center-drag with the mouse.

<p>
    It is also possible to pan by Shift+center-dragging, or to rotate
    by Shift+right-dragging. If a 3Dconnexion six degree of freedom
    controller (e.g., a SpaceNavigator) is connected, then this may
    also be used to transform the view of the model.

<p>
    To zoom in or out, rotate the scroll wheel. It is also possible
    to zoom by using the View menu, or the associated keyboard
    shortcuts (+ and -). Some features, including the planes, are
    always drawn the same size on-screen, and are therefore not
    affected by zooming.

<p>
    Most commands are available in three different ways: from a menu,
    from a keyboard shortcut, or from the toolbar. The toolbar is
    displayed at the top left of the graphics window. To learn what
    an icon means, hover the mouse over it. To show or hide the
    toolbar, choose View &rarr; Show Toolbar.

<p>
    To zoom to the extent of the part, choose View &rarr; Zoom To
    Fit. This adjusts the zoom level so that the part fits exactly
    on the screen, and then pans to center the part. The rotation
    of the part is not affected.

<p>
    If a workplane is active, then choose View &rarr; Align View to Workplane (or
    press W) to align the view to the workplane. After doing this,
    the plane of the screen is coincident with the workplane, and
    the center of the workplane is at the center of the screen. The
    zoom level is not affected.

<p>
    In an orthogonal view, one of the coordinate (x, y, or z) axes is
    horizontal, and another is vertical. To orient the view to the
    nearest orthogonal view, choose View &rarr; Nearest Ortho View.
    In an isometric view, all three coordinate axes are projected to the
    same length, and one of the coordinate axes is vertical.  To orient
    the view to the nearest isometric view, choose View &rarr; Nearest
    Iso View.

<p>
    To pan the view so that a given point is at the exact center
    of the screen, select that point and then choose View &rarr; Center
    View at Point.

<p>
    The x, y, and z coordinate axes are always drawn at the bottom
    left of the graphics window, in red, green, and blue. These axes
    are live: they can be highlighted and selected with the mouse, in
    the same way as any other normals. (This means that the coordinate
    axes are always conveniently available on-screen, which is useful
    e.g. when constraining a line parallel to the x-axis.)

<h3><a id="Dimension" href="#Dimension" class="anchor"></a>
Dimension Entry and Units</h3>

<p>
    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).

<p>
    Choose View &rarr; Dimensions in Inches/Millimeters 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.

<p>
    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.

<p>
    You can use <code>sqrt</code>, <code>square</code>, <code>sin</code>,
    <code>cos</code>, <code>asin</code>, <code>acos</code>, <code>pi</code>,
    <code>+</code>, <code>-</code>, <code>*</code>, <code>/</code>,
    <code>(</code>, <code>)</code> in the expressions. For example
    "<code>7*pi/(3+cos(45))</code>". The trigonometric functions take
    degrees.

<h3><a id="Text" href="#Text" class="anchor"></a>
Text Window</h3>

<p>
    The Property Browser appears as a floating palette window. It may
    be shown or hidden by pressing Tab, or by choosing View &rarr;
    Show Text Window.

<p>
    The Property Browser works like a web browser. Any underlined text is
    a link. To activate a link, click it with the mouse. The links
    may be used to navigate to other pages in the Property Browser. For
    example, the "home" screen is a list of groups in the sketch:

<div class="forimg">
    <img src="pics/ref-text-window.png">
</div>

<p>
    To navigate to a group's page, click that group's name (e.g.,
    "g002-sketch-in-plane"). The links may also trigger actions in
    the sketch. For example, in the above screenshot, all of the
    groups are shown. To hide a group, click the box in the
    "shown" column.

<p>
    As a convenience, the Property Browser will sometimes automatically
    navigate to a page that is likely to be relevant. For example,
    when a new group is created, the Property Browser displays that new
    group's page. It's always possible to navigate to a different
    page, by clicking the "home" link at the top left corner (or
    pressing Esc), and following the links from there.

<p>
    When sketch entities are selected (e.g., the user has clicked
    on them with the mouse), information about those entities is
    displayed in the Property Browser. If a single entity is selected,
    then information about that entity is displayed. For example,
    the window display's a circle's center and radius.

<p>
    If multiple entities are selected, then the Property Browser can
    sometimes display information about all of them. These cases
    include:

<ul>
    <li>two points: the distance between the points</li>

    <li>a point and a plane face: the distance from the point to the
    plane</li>

    <li>two points, and a vector: the distance between the points,
    projected along the vector</li>

    <li>two plane faces: the angle between the plane faces</li>
</ul>


<h3><a id="ShowHide" href="#ShowHide" class="anchor"></a>
Show / Hide Entities</h3>

<p>
    As the sketch becomes more complex, it may be useful to hide
    unnecessary information. SolveSpace provides several different
    ways to do this.
</p>

<p>
    Along the top of the Property Browser, a row of icons appears. These icons
    make it possible to hide and show different elements in the sketch:
</p>

<table class="showtab" cellspacing="0" cellpadding="0">

<td class="showleft"><p>workplanes from inactive groups</p></td>
<td class="showright"><p>
When a new "Sketch In New Workplane" group is created, an associated
workplane is created automatically. These workplanes are either
visible whenever that group is visible (item shown), or visible only
when that group is both visible and active (item hidden).
</p></td>

</tr><tr>

<td class="showleft"><p>normals</p></td>
<td class="showright"><p>
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 icon may be used to hide them.
    </p></td>

</tr><tr>

<td class="showleft"><p>points</p></td>
<td class="showright"><p>
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 icon 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.
    </p></td>

</tr><tr>

<td class="showleft"><p>constraints and dimensions</p></td>
<td class="showright"><p>
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 icon.
    </p></td>

</tr><tr>


<td class="showleft"><p>faces selectable with the mouse</p></td>
<td class="showright"><p>
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.</p>

<p>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 icon.
    </p></td>

</tr><tr>


<td class="showleft"><p>shaded view of solid model</p></td>
<td class="showright"><p>
The 3d part is displayed as an opaque solid, with lighting effects to
give the impression of depth. This icon may be used to hide that view.
    </p></td>

</tr><tr>

<td class="showleft"><p>edges of solid model</p></td>
<td class="showright"><p>
Lines are drawn wherever two different surfaces of the solid model
meet. If edges are shown but shaded is hidden, then a wireframe
display results. The display of meshes may be noticeably slower when
edges are shown. The display of NURBS surfaces will not be noticeably
slower when edges are shown. The color of the edges may be set in the
line styles.
    </p></td>
</tr><tr>


<td class="showleft"><p>triangle mesh of solid model</p></td>
<td class="showright"><p>
The 3d model of the part consists of many triangles; for example,
a rectangular face is represented by two triangles. Use this icon to
show the triangles on the model. This is a good way to see how fine or
coarse the mesh is before exporting it.
    </p></td>
</tr><tr>


<td class="showleft"><p>hidden lines</p></td>
<td class="showright"><p>
With the part in a given orientation, some of the lines in the part will
be invisible, because they are buried inside the solid part.  To show
those lines anyways, as if the part were transparent, use this icon. This
is useful when drawing a sketch that lies within the volume of the part.
    </p></td>
</tr>
</table>

<p>
        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. The solid model is not affected; if a hidden group
        contains a circle that is extruded to form a cylinder, then the
        cylinder will remain visible.

<p>
        To hide a group, go to the home screen in the Property Browser, 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 checkbox in the "shown" column is checked.
        Click the checkbox; it now appears unchecked, and the group
        is hidden.

        The show / hide status of groups is saved in the part file. If
        a part is linked 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><a id="ActiveWorkplane" href="#ActiveWorkplane" class="anchor"></a>
Active Workplane</h3>

<p>
    SolveSpace represents all geometry in 3d; it's possible to draw
    line segments anywhere, not just in some plane.

<p>
    This freedom is not always useful, so SolveSpace also makes
    it possible to draw in a plane. If a workplane is active, then
    all entities that are drawn will be forced to lie that plane.
    The active workplane ("in plane:") is indicated in the top line of
    the Property Browser, at the right.

<p>
    When SolveSpace starts with a new empty file, a workplane parallel
    to the XY plane is active. To deactivate the workplane, and draw
    in 3d, choose Sketch &rarr; Anywhere In 3d.

<p>
    To activate a workplane, select it, and then choose Sketch &rarr;
    In Workplane. When a workplane is activated, the view is aligned
    onto that workplane. (The workplane remains active until the
    user chooses Sketch &rarr; Anywhere In 3d, or a different workplane
    is activated. If the user rotates the view, so that the view
    is no longer aligned onto the workplane, then the workplane
    remains active.)

<p>
    In a "Sketch in New Workplane" group, the group's associated
    workplane may be activated by choosing Sketch &rarr; In Workplane;
    there is no need to select it first.

<h3><a id="ActiveGroup" href="#ActiveGroup" class="anchor"></a>
Active Group</h3>

<p>
    When a new line, circle, or other curve is created, it will be created
    in the active group.  Geometry from the active group is drawn in
    white; geometry from earlier groups is drawn in brown. Later groups
    are hidden.

<p>
    In the Property Browser's home screen (press Escape, or choose the link
    in the top left corner), the active group's line in the list of
    groups has a selected radio button in the "active" column. All
    other groups (except g001-#references, which cannot be activated)
    have an unselected radio button in that column.  To activate an
    inactive group, click its radio button.

<p>
    In order to reduce distraction when sketching in 2D, solid models from
    inactive groups are "dimmed" (by rendering them using the
    #def-dim-solid style) so that they blend into the background.  To
    disable this uncheck View &rarr; Darken Inactive Solids.  By modifying
    the #def-dim-solid style any color may be assigned to geometry from
    inactive groups instead of just "dimming" them.  A brighter color may
    even be assigned to this style to make geometry from inactive groups
    stand out more clearly instead if desired.

</div>

<h2><a id="Sketch" href="#Sketch" class="anchor"></a>
Sketch Entities</h2>

<div class="refind">
<h3><a id="Construction" href="#Construction" class="anchor"></a>
Construction Geometry</h3>

<p>
    In normal operation, the user draws line and curves in a
    sketch. Those curves describe the geometry to be manufactured;
    ultimately, the endmill or the laser or some other tool will
    cut along those curves.

<p>
    In some cases, it is useful to draw a line that should not
    appear on the final part. For example, the user may wish to draw
    a center line for a symmetric part; but that center line is only
    a guide, and should not actually get exported with the CAM data.
    These lines are called construction lines.

<p>
    To mark an entity as construction-only, choose Sketch &rarr; Toggle
    Construction. A construction entity will behave just like any other
    entity, except that it is drawn in green, and does not contribute to
    the geometry for export by default (or to the section that will be
    extruded or lathed or swept).  You may also toggle construction
    geometry while sketching a new entity by using the 'g' keyboard
    shortcut.

<h3><a id="Datum" href="#Datum" class="anchor"></a>
Datum Point</h3>

<p>
    This entity is defined by a single point.

<p>
    If a workplane is active when the datum point is created,
    then that datum point will always lie in the workplane. If no
    workplane is active, then the datum point will be free in 3d.
    (This is the same behaviour as for all points, including e.g. the
    endpoints of a line segment.)

<p>
    Datum points are typically used as construction geometry. The user
    might place datum points in order to simplify the dimensioning
    of line segments or other entities.

<h3><a id="Workplane" href="#Workplane" class="anchor"></a>
Workplane</h3>

<p>
    This entity is specified by a point and a normal. The point
    defines its origin, and the normal defines its orientation.

<p>
    A workplane makes it possible to draw a section in 2d. If a
    workplane is active, then any entities that are drawn must lie
    in that workplane.

<p>
    It's almost never necessary to create workplanes explicitly.
    Instead, create a new Sketch in New Workplane group.

<h3><a id="Line" href="#Line" class="anchor"></a>
Line Segment</h3>

<p>
    This entity is specified by its two endpoints. If a workplane is
    active, then the two endpoints will always lie in that workplane.

<p>
    To create the line segment, choose Sketch &rarr; Line Segment, and
    then left-click one endpoint of the line. Then release the mouse
    button; the other endpoint is now being dragged.

<p>
    To create another line segment, that shares an endpoint with
    the line segment that was just created, left-click again. This
    is a fast way to draw closed polygons.

<p>
    To stop drawing line segments, press Escape, or right- or
    center-click the mouse. SolveSpace will also stop drawing new
    line segments if an automatic constraint is inserted. (For
    example, draw a closed polygon by left-clicking repeatedly, and
    then hovering over the starting point before left-clicking the
    last time. The endpoint of the polyline will be constrained to
    lie on the starting point, and since a constraint was inserted,
    SolveSpace will stop drawing.)

<h3><a id="Rectangle" href="#Rectangle" class="anchor"></a>
Rectangle</h3>

<p>
    This entity 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.

<p>
    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.

<p>
    A workplane must be active when the rectangle is drawn, since
    the workplane defines the meaning of "horizontal" and "vertical".

<h3><a id="Circle" href="#Circle" class="anchor"></a>
Circle</h3>

<p>
    This entity is specified by its center point, by its diameter,
    and by its normal.

<p>
    To create the circle, choose Sketch &rarr; Circle, and then left-click
    the center. Then release the mouse button; the diameter of
    the circle is now being dragged. Left-click again to place
    the diameter.

<p>
    If a workplane is active, then the center point must lie in
    that workplane, and the circle's normal is parallel to the
    workplane's normal (which means that the circle lies in the
    plane of the workplane).

<p>
    If no workplane is active, then the center point is free in space,
    and the normal may be dragged (or constrained) to determine the
    circle's orientation.

<h3><a id="Arc" href="#Arc" class="anchor"></a>
Arc of a Circle</h3>

<p>
    This entity is specified by its center point, the two endpoints,
    and its normal.

<p>
    To create the arc, choose Sketch &rarr; Arc of a Circle, and then
    left-click one of its endpoints. Then release the mouse button;
    the other endpoint is now being dragged. The center is also being
    dragged, in such a way as to form an exact semi-circle.

<p>
    Left-click again to place the other endpoint, and then drag the
    center to the desired position. The arc is drawn counter-clockwise
    from the first point to the second.

<p>
    The arc must be drawn in a workplane; it cannot be drawn in
    free space.

<h3><a id="TangentArc" href="#TangentArc" class="anchor"></a>
Tangent Arc at Point</h3>

<p>
    To round off a sharp corner (for example, between two lines),
    we often wish to create an arc at the corner, that is tangent to
    both of the lines. This will create a smooth appearance where
    the line and arc join. It would be possible to draw these arcs
    by hand, using Sketch &rarr; Arc of a Circle and Constrain &rarr;
    Tangent, but it's easier to create them automatically.

<p>
    To do so, first select a point where two line segments or circles
    join. Then choose Sketch &rarr; Tangent Arc at Point; the arc
    will be created, and automatically constrained tangent to the two
    adjoining curves.

<p>
    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.

<p>
    By default, the radius of the tangent arc is chosen automatically.
    To change that, choose Sketch &rarr; Tangent Arc at Point with nothing
    selected. A screen will appear in the Property Browser, where the radius
    may be specified. It is also possible to specify whether the original
    lines and curves should be kept, but changed to construction lines
    (which may be useful if you want to place constraints on them),
    or whether they should be deleted.

<h3><a id="Bezier" href="#Bezier" class="anchor"></a>
Bezier Cubic Spline</h3>

<p>
    This entity is specified by at least two on-curve points, and
    an off-curve control point at each end (so two off-curve points
    total). If only two on-curve points are present, then this is a
    Bezier cubic section, and the four points are exactly the Bezier
    control points.

<p>
    If more on-curve points are present, then it is a second derivative
    continuous (C2) interpolating spline, composed of multiple Bezier
    cubic segments. This is a useful type of curve, because it has a smooth
    appearance everywhere, even where the sections join.

<p>
    To create the Bezier cubic spline, choose Sketch &rarr; Bezier
    Cubic Spline. Then left-click one endpoint of the cubic segment.
    Release the mouse button; the other endpoint of the cubic segment
    is now being dragged. To add more on-curve points, left click with
    the mouse. To finish the curve, right-click, or press Esc.

<p>
    The two control points are intially placed on the straight line
    between the endpoints; this means that the cubic originally
    appears as a straight line. Drag the control points to produce
    the desired curve.

<p>
    To create a closed curve (technically, a "periodic spline"), start
    by creating the curve as usual, left-clicking to create additional
    on-curve points. Then hover the mouse over the first point in the
    curve, and left-click. The curve will be converted to a periodic
    spline, which will be C2 continuous everywhere, including at that
    first point.

<h3><a id="TextTT" href="#TextTT" class="anchor"></a>
Text in a TrueType Font</h3>

<p>
    This entity is defined by four points, at each corner of the text.  The
    distance between the points determines the height and width of the
    text; the angle of the line between them determines the orientation of
    the text, and their position determines the text's position.

<p>
    To create the text, choose Sketch &rarr; Text in TrueType Font. Then
    left-click the top left point of the text. The bottom right point
    of the text is now being dragged; left-click again to place it.

<p>
    To change the font, select the text entity. A list of installed
    fonts appears in the Property Browser; click the font name to select
    it. To change the displayed text, select the text entity and
    click the [change] link in the Property Browser.

<h3><a id="Image" href="#Image" class="anchor"></a>
Image</h3>

<p>
    This entity may be used to place a bitmap reference image in a sketch.
    The entity is defined by four control points that may be used to
    position, constrain and orient the image similar to those for TrueType
    Text entities.  Image entities are typically used as a reference for
    sketching or tracing other entities and removed later.  As such, Image
    entities are not exportable.

<h3><a id="Splitting" href="#Splitting" class="anchor"></a>
Splitting and Trimming Entities</h3>

<p>
    In some cases, it is desirable to draw by creating overlapping
    figures, and then removing the extra lines. For example, in this
    case, a circle and a rectangle are drawn; the two short lines and
    the short arc are then deleted, to form a single closed shape.

<div class="forimg">
    <img src="pics/ref-split.png">
</div>

<p>
    In order to trim the extra lines, it is necessary to split the
    entities where they intersect. SolveSpace can split lines, circles,
    arcs, and Bezier curves against each other.
    To do so, select the two
    entities to be split, and then choose Sketch &rarr; Split Curves
    at Intersection. This deletes each original entity, and replaces it
    with two new entities that share an endpoint at the intersection.
    The excess lines may then be deleted as usual.

<p>
    Because the original entities are deleted, any constraints on the
    original entities are deleted as well. This means that the sketch
    may no longer be constrained as desired after splitting. If an
    entity is marked as construction before splitting, then it will
    not be deleted, so the constraints will persist.

</div>

<h2><a id="Constraints" href="#Constraints" class="anchor"></a>
Constraints</h2>

<div class="refind">
<h3><a id="GeneralConstraints" href="#GeneralConstraints" class="anchor"></a>
General</h3>

<p>
    To create a constraint, first select the geometry to be
    constrained. For example, when constraining the distance between
    two points, first select those two points. Then choose the
    appropriate constraint from the Constrain menu.

<p>
    Depending on what is selected, the same menu item may generate
    different constraints. For example, the Distance / Diameter menu
    item will generate a diameter constraint if a circle is selected,
    but a length constraint if a line segment is selected. If the
    selected items do not correspond to an available constraint,
    then SolveSpace will display an error message, and a list of
    available constraints.

<p>
    Most constraints are available in both 3d and projected versions.
    If a workplane is active, then the constraint applies on the
    projection of the geometry into that workplane. If no workplane
    is active, then the constraint applies to the actual geometry
    in free space.

<p>
    For example, consider the line shown below:

<div class="forimg">
    <img src="pics/ref-projd-constraint.png">
</div>

<p>
    The line's length is constrained in two different ways. The upper
    constraint, for 50 mm, applies to its actual length. The lower
    constraint, for 40 mm, applies to the length of its projection
    into the XY plane. (The XY plane is highlighted in yellow.) The
    dotted purple lines are drawn to indicate the locations of the
    line segment's projected endpoints.

<p>
    In normal operation, the user activates a workplane (or a
    workplane is activated automatically, for example by creating a
    "Sketch in New Workplane" group). The user then draws an entity,
    for example a line. Since a workplane is active, the line is
    created in that workplane. The user then constrains that line,
    for example by specifying its length. Since the workplane is
    still active, the constraint actually applies to the projection
    of the line segment into the workplane.

<p>
    In this case, the projected distance is equivalent to the
    3d distance. If the line segment lies in the workplane, then
    the projection of that line segment into the workplane is just
    that line segment. This means that when drawing in a workplane,
    most of this can be ignored.

<p>
    It's possible to use projected constraints in more complex ways,
    though. For example, the user might create a line segment in
    workplane A, and constrain its projection into workplane B.

<p>
    Constraints are drawn in purple on the sketch. If a constraint
    has a label associated with it (e.g. a distance or an angle), then
    that label may be repositioned by dragging it with the mouse. To
    modify the dimension, double-click the label; a text box will
    appear on the screen, where the new value can be entered. Press
    enter to commit the change, or Esc to cancel.

<h3><a id="Automatic" href="#Automatic" class="anchor"></a>
Automatic Constraints</h3>

<p>
    There is an option in the configuration screen labled "enable
    automatic line constraints". If this option is checked and a line
    being drawn is nearly horizontal, a horizontal contraint will
    appear over the middle of the line and will be applied when the
    second point of the line is clicked in place. Similarly when a
    nearly vertical line is being drawn a "V" constraint will appear
    automatically. If the line is not close enough to horizontal or
    vertical, no constraint will be added.  Holding Ctrl while sketching
    will also disable this feature.
    
<p>
    If an automatic constraint is redundant or would result in the
    sketch being over-constrained, it will not be created even if
    it is shown during line placement. Similarly if a distance or
    diameter constraint is added that would over-constrain the
    sketch, it will be created as a reference (REF).

<p>
    Another option in the configuration screen is "edit newly added
    dimensions". With this option enabled, when a new Distance, Lenght
    Ratio, or Length Difference constraint is added the input box will
    automatically appear so a specific value can be entered. With the
    option off the user would have to create the constraint and then
    double-click on it to edit the value, which is almost always what
    we want to do.
 
<h3><a id="Failure" href="#Failure" class="anchor"></a>
Failure to Solve</h3>

<p>
    In some cases, the solver will fail. This is usually because the
    specified constraints are inconsistent or redundant. For example,
    a triangle with internal angles of 30, 50, and 90 degrees is
    inconsistent--the angles don't sum to 180, so the triangle could
    never be assembled. This is an error.

<p>
    A triangle with internal angles constrained to 30, 50, and 100
    degrees is also an error. This is not inconsistent, because the
    angles do sum to 180 degrees; but it's redundant, because only
    two of those angles need to be specified.

<p>
    If the sketch is inconsistent or redundant, then the background
    of the graphics window is drawn in red (instead of the usual
    black), and an error is displayed in the Property Browser:

<div class="forimg">
    <img src="pics/ref-inconsistent.png">
</div>

<p>
    As a convenience, SolveSpace calculates a list of constraints
    that could be removed to make the sketch consistent again. To
    see which constraints those are, hover the mouse over the links
    in the Property Browser; the constraint will appear highlighted in
    the graphics window. By deleting one or more of the constraints
    in that list, the user can make the sketch consistent again.

<p>
    A different type of error occurs when the solver fails to
    converge. This may be a defect in the solver, or it may occur
    because impossible geometry was specified (for example, a
    triangle with side lengths 3, 4, and 10; 3 + 4 = 7 < 10). In
    that case, a similar error message is displayed, but without a
    list of constraints to remove to fix things. The problem can be
    resolved by removing or editing the constraints, or by choosing
    Edit &rarr; Undo.


<h3><a id="Reference" href="#Reference" class="anchor"></a>
Reference Dimensions</h3>

<p>
    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.

<p>
    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 possible to freely change that length,
    and the dimension displays whatever that length happens to be. A
    reference dimension does not constrain the geometry.

<p>
    To convert a dimension into a reference dimension, choose
    Constrain &rarr; 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, so it is
    not meaningful to type in a new value for the reference dimension.

<h3><a id="Specific" href="#Specific" class="anchor"></a>
Specific Constraints</h3>

<p>
    To get help on a specific constraint, choose its menu item without
    first selecting any entities. An error message will be displayed,
    listing all of the possibilities.

<p>
    In general, the order in which the entities are selected doesn't
    matter. For example, if the user is constraining point-line
    distance, then they might select the point and then the line, or
    the line and then the point, and the result would be identical.
    Some exceptions exist, and are noted below.

<h3><a id="Distance" href="#Distance" class="anchor"></a>
Distance / Diameter</h3>

<p>
    This constraint sets the diameter of an arc or a circle, or the
    length of a line segment, or the distance between a point and
    some other entity.

<p>
    When constraining the distance between a point and a plane, or
    a point and a plane face, or a point and a line in a workplane,
    the distance is signed. The distance may be positive or negative,
    depending on whether the point is above or below the plane. The
    distance is always shown positive on the sketch; to flip to the
    other side, enter a negative value.

<h3><a id="Angle" href="#Angle" class="anchor"></a>
Angle</h3>

<p>
    This constraint sets the angle between two vectors. A vector
    is anything with a direction; in SolveSpace, line segments and
    normals are both vectors. (So the constraint could apply to
    two line segments, or to a line segment and a normal, or to two
    normals.) The angle constraint is available in both projected
    and 3d versions.

<p>
    The angle must always lie between 0 and 180 degrees. Larger or
    smaller angles may be entered, but they will be taken modulo
    180 degrees. The sign of the angle is ignored.

<p>
    When two lines intersect, four angles are formed. These angles
    form two equal pairs. For example, the pictured lines interesect
    at 30 degrees and 150 degrees. These two angles (30 and 150) are
    known as supplementary angles, and they always sum to 180 degrees.

<div class="forimg">
    <img src="pics/ref-line-cross-angles.png">
</div>

<p>
    (Notice that in the sketch, three of the angle constraints are
    reference dimensions. Given any one of the angles, we could
    calculate the other three; so a sketch that specified more than
    one of those angles would be overconstrained, and fail to solve.)

<p>
    When a new angle constraint is created, SolveSpace chooses
    arbitrarily which supplementary angle to constrain. An arc is
    drawn on the sketch, to indicate which angle was chosen. As the
    constraint label is dragged, the arc will follow.

<p>
    If the wrong supplementary angle is constrained, then select the
    constraint and choose Constrain &rarr; Other Supplementary Angle. A
    constraint of 30 degrees on one supplementary angle is exactly
    equivalent to a constraint of 150 degrees on the other.

<h3><a id="Horizontal" href="#Horizontal" class="anchor"></a>
Horizontal / Vertical</h3>

<p>
    This constraint forces a line segment to be horizontal or
    vertical. It may also be applied to two points, in which case
    it applies to the line segment connecting those points.

<p>
    A workplane must be active, because the meaning of "horizontal"
    or "vertical" is defined by the workplane.

<p>
    It's good to use horizontal and vertical constraints whenever
    possible. These constraints are very simple to solve, and will
    not lead to convergence problems. Whenever possible, define
    the workplanes so that lines are horizontal and vertical within
    those workplanes.

<h3><a id="On" href="#On" class="anchor"></a>
On Point / Curve / Plane</h3>

<p>
    This constraint forces two points to be coincident, or a point
    to lie on a curve, or a point to lie on a plane.

<p>
    The point-coincident constraint is available in both 3d and
    projected versions. The 3d point-coincident constraint restricts
    three degrees of freedom; the projected version restricts only
    two. If two points are drawn in a workplane, and then constrained
    coincident in 3d, then an error will result--they are already
    coincident in one dimension (the dimension normal to the plane),
    so the third constraint equation is redundant.

<p>
    When a point is constrained to lie on a circle (or an arc of
    a circle), the actual constraint forces the point to lie on
    the cylindrical surface through that circle. If the point and
    the circle are already coplanar (e.g., if they are both drawn
    in the same workplane), then the point will lie on the curve,
    but otherwise it will not.

<h3><a id="Equal" href="#Equal" class="anchor"></a>
Equal Length / Radius / Angle</h3>

<p>
    This constraint forces two lengths, angles, or radiuses to
    be equal.

<p>
    The equal-angle constraint requires four vectors as input:
    the two equal angles are the angle between each pair of inputs.
    For example, select line segments A, B, C, and D. The constraint
    forces the angle between lines A and B to be equal to the angle
    between lines C and D. If the wrong supplementary angle is chosen,
    then choose Constrain &rarr; Other Supplementary Angle, as for the
    angle constraint.

<p>
    If a line and an arc of a circle are selected, then the length of
    the line is forced equal to the length (not the radius) of the
    arc.

<h3><a id="LengthRatio" href="#LengthRatio" class="anchor"></a>
Length Ratio</h3>

<p>
    This constraint sets the ratio between the lengths of two line
    segments. For example, if line A and line B have length ratio
    2:1, then the constraint is satisfied if A is 50 mm long and B
    is 25 mm long.

<p>
    The order in which the lines are selected matters; if line A is
    selected before line B, then the ratio is length of A:length of B.

<h3><a id="LengthDifference" href="#LengthDifference" class="anchor"></a>
Length Difference</h3>

<p>
    This constraint sets the difference between the lengths of two line
    segments. For example, if line A and line B have length difference
    5 mm, then the constraint is satisfied if A is 50 mm long and B
    is 55 mm long or 45mm long.

<p>
    Note that a negative difference can be entered when editing the
    constraint to change which is the shorter segment. At the same time
    the value is always displayed as a positive number (the absolute
    difference) and entering positive numbers does not change the
    "direction".

<h3><a id="At" href="#At" class="anchor"></a>
At Midpoint</h3>

<p>
    This constraint forces a point to lie on the midpoint of a line.

<p>
    The at-midpoint constraint can also force the midpoint of a line
    to lie on a plane; this is equivalent to creating a datum point,
    constraining it at the midpoint of the line, and then constraining
    that midpoint to lie on the plane.

<h3><a id="Symmetric" href="#Symmetric" class="anchor"></a>
Symmetric</h3>

<p>
    This constraint forces two points to be symmetric about some
    plane. Conceptually, this means that if we placed a mirror at
    the symmetry plane, and looked at the reflection of point A,
    then it would appear to lie on top of point B.

<p>
    The symmetry plane may be specified explicitly, by selecting a
    workplane. Or, the symmetry plane may be specified as a line in
    a workplane; the symmetry plane is then through that line, and
    normal to the workplane. Or, the symmetry plane may be omitted;
    in that case, it is inferred to be parallel to either the active
    workplane's vertical axis or its horizontal axis. The horizontal
    or vertical axis is chosen, depending which is closer to the
    configuration in which the points were initially drawn.

<h3><a id="Perpendicular" href="#Perpendicular" class="anchor"></a>
Perpendicular</h3>

<p>
    This constraint is exactly equivalent to an angle constraint
    for ninety degrees.

<h3><a id="Parallel" href="#Parallel" class="anchor"></a>
Parallel / Tangent</h3>

<p>
    This constraint forces two vectors to be parallel.

<p>
    In 2d (i.e., when a workplane is active), a zero-degree angle
    constraint is equivalent to a parallel constraint. In 3d, it
    is not.

<p>
    Given a unit vector A, and some angle theta, there are in general
    infinitely many unit vectors that make an angle theta with A. (For
    example, if we are given the vector (1, 0, 0), then (0, 1, 0),
    (0, 0, 1), and many other unit vectors all make a ninety-degree
    angle with A.) But this is not true for theta = 0; in that case,
    there are only two, A and -A.

<p>
    This means that while a normal 3d angle constraint will restrict
    only one degree of freedom, a 3d parallel constraint restricts
    two degrees of freedom.

<p>
    This constraint can also force a line to be tangent to a curve, or
    force two curves (for example, a circle and a cubic) to be tangent to
    each other. In order to do this, the two curves must already share
    an endpoint; this would usually be achieved with a point-coincident
    constraint. The constraint will force them to also be tangent at
    that point.

<h3><a id="Same" href="#Same" class="anchor"></a>
Same Orientation</h3>

<p>
    This constraint forces two normals to have the same orientation.

<p>
    A normal has a direction; it is drawn as an arrow in that
    direction. The direction of that arrow could be specified by
    two angles. The normal specifies those two angles, plus one
    additional angle that corresponds to the twist about that arrow.

<p>
    (Technically, a normal represents a rotation matrix from one
    coordinate system to another. It is represented internally as
    a unit quaternion.)

<p>
    For example, the picture below shows two workplanes, whose
    normals are constrained to be parallel:

<div class="forimg">
    <img src="pics/ref-parallel-normals.png">
</div>

<p>
    Because the normals are parallel, the planes are parallel. But one
    plane is twisted with respect to the other, so the planes are not
    identical. The line on the left is constrained to be horizontal
    in the leftmost plane, and the line on the right is constrained
    to be horizontal in the rightmost. These lines are not parallel,
    even though the normals of the workplanes are parallel.

<p>
    If we replace the "parallel" constraint with a "same orientation"
    constraint, then the two workplanes become identical, and the
    two horizontal lines become parallel.

<p>
    This is a useful constraint when building an assemblies; a single
    "same orientation" constraint will fix all three of a linked
    part's rotational degrees of freedom.

<h3><a id="Lock" href="#Lock" class="anchor"></a>
Lock Point Where Dragged</h3>

<p>
    Constrain a point such that the solver will not alter its location.
    This does not prevent direct manipulation by dragging the entity
    that owns the point or the point itself.  It simply instructs the
    solver to consider the point fully constrained.  This can be easily
    demonstrated by drawing an equilateral triangle with sides
    constrained equal and one point locked.  Dragging the side opposite
    this locked point will not alter its position but will resize the
    triangle instead.

<h3><a id="Comment" href="#Comment" class="anchor"></a>
Comment</h3>

<p>
    A comment is a single line of text that appears on the drawing.
    To create a comment, select Constrain &rarr; Comment, and then
    left-click the center of the new comment. To move the comment,
    drag it with the mouse. To change the text, double-click it.

<p>
    The comment has no effect on the geometry; it is only a
    human-readable note. By default, the comment is shown in the same
    color as the constraints; but a comment may be assigned to a
    custom line style, in order to specify the line width and color,
    text height, text origin (left, right, top, bottom, center), and
    text rotation.

<p>
    If a comment is created within a workplane, then the text will
    be drawn within the plane of that workplane. Otherwise, the text
    will always be drawn facing forward, in the plane of the screen.

<p>
    By default, comments are hidden when their group is inactive, the
    same as for all other constraints. If a comment is assigned to a
    custom style, then that comment will be shown even when its group
    is inactive, as long as the style (and the group, and constraints
    overall) is shown.

</div>

<h2><a id="Groups" href="#Groups" class="anchor"></a>
Groups</h2>

<div class="refind">
<p>
    To view a list of groups, go to the home page of the Property Browser.
    This is accessible from the link at the top left of the text
    window, or by pressing Esc. To view a group's page, click
    its name in the list.

<p>
    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 Property Browser, and choose
    [rename].

<p>
    Groups that create a solid (e.g. extrudes or lathes) have a "solid
    model as" option, which is displayed in the page in the Property Browser.
    The group can be merged as union, which adds material to the
    model, or as difference, which cuts material away. A third option is
    intersection, which preserves only the material that falls within
    both solids.

<p>
    The union, difference and intersection operations may be performed either as
    triangle meshes, or as exact NURBS surfaces. Triangle meshes are
    fast to compute and robust, but they require any smooth curves
    to be approximated as piecewise linear segments. The NURBS surface
    operations are not as robust, and will fail for some types of geometry;
    but they represent smooth curves exactly, which makes it possible
    for example to export a DXF in which a circular arc appears as an
    exact circle, instead of many piecewise linear edges.

<p>
    These groups also have a color, which determines the color of
    the surfaces they produce. To change the color, click one of
    the swatches in the group's page in the Property Browser.

<p>
    The group's page in the Property Browser 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 the link in the
    Property Browser. This is equivalent to hovering over and clicking
    the actual object in the graphics window.

<h3><a id="SketchIn3d" href="#SketchIn3d" class="anchor"></a>
Sketch in 3d</h3>

<p>
    This creates a new empty group, in which the user may draw lines,
    circles, arcs, and other curves.

<p>
    The ultimate goal is usually to draw closed sections (like
    a triangle, or a square with a circular cutout, or some more
    complicated shape). These sections are the input for later groups.
    For example, an extrude group takes a flat section, and uses it
    to form a solid.

<p>
    If all of the entities in the group can be assembled into closed
    loops, then the area that the loops enclose is shaded in very
    dark blue. This is the area that would be swept or extruded or
    lathed by a subsequent group.

<h3><a id="SketchInWorkplane" href="#SketchInWorkplane" class="anchor"></a>
Sketch in New Workplane</h3>

<p>
    This creates a new empty group, similar to a new "Sketch in 3d".
    The difference is that a "Sketch in New Workplane" also creates
    a workplane. The workplane is created based on the entities that
    are selected when the sketch is created. These may be:

    <table class="showtab">
    <tr>
    <td class="showleft"><p>a point and two line segments</p></td>
    <td class="showright"><p>
        The new workplane has its origin at the specified point. The
        workplane is parallel to the two lines. If the point is a
        vertex on a face of the part, and the two lines are two edges
        of that face, then the resulting workplane will be coincident
        with that face (i.e., the user will be drawing on that face).
    </p></td>

    </tr><tr>

    <td class="showleft"><p>a point</p></td>
    <td class="showright"><p>
        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.</p>

        <p>
        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.</p>

        <p>If a part consists mostly of ninety degree angles, then this
        is a quick way to create workplanes.</p>
    </p></td>

    </tr></table>

<p>
    The new group's associated workplane is automatically set to be
    the active workplane.

<p>
    If the entities in this group do not form closed curves, then
    an error message is displayed on the screen, and a red line is
    drawn across the gap. An error is also displayed if the curves
    are not all coplanar.

<h3><a id="StepTranslating" href="#StepTranslating" class="anchor"></a>
Step Translating</h3>

<p>
    This group takes geometry in the active group, and copies it
    multiple times along a straight line.

<p>
    If a workplane is active when the step translating group is
    created, then the translation vector must lie parallel to that
    workplane. Otherwise, the translation vector may go anywhere in
    free space.

<p>
    The number of copies to create is specified by the user. To
    change this value, click the [change] link in the group's page
    in the Property Browser.

<p>
    The copies may be translated on one side, or on two sides. If
    the copies are translated on one side, then the original will
    appear to the left of (or above, below, etc.) all the copies. If
    the copies are translated on two sides, then the original will
    appear in the center of the copies.

<p>
    The copies may be translated starting from the original,
    or starting from copy #1. If the translation starts from the
    original, then the translation will contain the original. (So
    a 1-element step will always produce the input geometry in its
    original location.) If the translation starts from copy #1, then
    the original is not included in the output. (So a 1-element step
    makes a single copy of the input geometry, and allows the user
    to translate it anywhere in space.)

<p>
    If the active group is a sketch (sketch in 3d, sketch in new
    workplane), the the sketch is stepped and repeated. In that case
    the user would typically draw a section, step and repeat that
    section, and then extrude the step and repeat.

<p>
    If the active group is a solid (extrude, helix, lathe, revolve), then
    the solid is stepped and repeated. In this case, the user would
    draw a section, extrude the section, and then step and repeat
    the extrusion.

<p>
    In some cases, these two possibilities (extrude the step, vs.
    step the extrusion) are equivalent. If the translation vector
    isn't parallel to the section plane, then only the second option
    will work.

<h3><a id="StepRotating" href="#StepRotating" class="anchor"></a>
Step Rotating</h3>

<p>
    This group takes the geometry in the active group, and copies
    it mutiple times along a circle.

<p>
    Before creating the group, the user must select its axis of
    rotation. One way to do this is to select a point, plus either
    a line segment or a normal; the axis of rotation goes through
    the point, and is parallel to the line segment or normal.

<p>
    If a workplane is active, then it's also possible to select
    just a point; in that case, the axis of rotation goes through
    that point, and is normal to the workplane. This means that the
    rotation remains within the plane of the workplane.

<p>
    The step and repeat options (one side / two sides, with original /
    with copy #1) are the same as for step translating groups.

<p>
    The numer of copies is specified in the same way as for step
    translating. If the rotated geometry has not yet been constrained,
    then the copies will be spaced evenly around a circle; for
    example, if 5 copies are requested, then the spacing will be
    360/5 = 72 degrees.

<p>
    To place the copies along less than (or more than) a complete
    circle, drag a point on one of the copies with the mouse; all
    of the rest will follow, as the step rotation angle is modified.
    Constraints (for example an angle constraint, or a point-on-lie
    constraint) may be used to specify the angle of rotation exactly.

<h3><a id="Extrude" href="#Extrude" class="anchor"></a>
Extrude</h3>

<p>
    This group takes a flat section, and extrudes it to form a solid.
    The flat section is taken from the section of the group that
    is active when the extrude group is created. (This is usually
    a sketch in workplane, or a sketch in 3d, but could also be a
    step and repeat.)

<p>
    The sketch may be extruded on one side, or on two sides. If the
    sketch is extruded on one side, then the new solid is either
    entirely above or entirely below the original sketch. Drag a
    point on the new surface to determine the extrude direction,
    and also to determine the extrude depth. Once the extrusion
    depth looks approximately correct, it may be specified exactly
    by using constraints. For example, the user might constrain the
    length of one of the newly extruded edges.

<p>
    If the sketch is extruded on two sides, then the original sketch
    lies at the exact midpoint of the new solid. This means that
    the solid is symmetric about the original sketch plane. Later
    dimensioning often becomes simpler when the part has symmetry,
    so it's useful to extrude on two sides whenever possible.

<p>
    A workplane must be active when the group is created, and 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.
    It is possible to extrude perpendicular to a workplane other
    than the one the sketch is drawn in by selecting the other
    workplane prior to creating the extrusion. This can be used to
    create skewed extrusions.

<p>
    By default, no workplane is active in a new extrude group. This
    means that constraints will apply in 3d; for example, a length
    constraint is a constraint on the actual length, and not on the
    length projected into some plane. This is typically the desired
    behaviour, but it's possible to activate a workplane in the usual
    way (by selecting it, then choosing Sketch &rarr; In Workplane).

<h3><a id="Lathe" href="#Lathe" class="anchor"></a>
Lathe</h3>

<p>
    This group takes a flat sketch, and sweeps it around a
    specified axis, to form a solid of revolution. The section
    is taken from the group that is active when the lathe group
    is created.

<p>
    To create a lathe group, first select a line segment. Then choose
    New Group &rarr; Lathe. The line segment is the axis of revolution.

<p>
    The section must not intersect itself as it is swept along the
    curve. If the section crosses the axis of rotation, then it is
    certain to intersect itself and fail.

<h3><a id="Revolve" href="#Revolve" class="anchor"></a>
Revolve</h3>

<p>
    This group takes a flat sketch, and sweeps it around a
    specified axis, to form a solid of revolution. The difference
    between this and a Lathe group is that Revolve does not sweep
    a full 360 degrees. The resulting solid can be dragged or constrained
    to a specific angle. If dragged beyond 360 degrees this will
    produce the exact same solid as a Lathe group.

<h3><a id="Helix" href="#Helix" class="anchor"></a>
Helix</h3>

<p>
    This group takes a flat sketch, and sweeps it around a specified
    axis while also translating along that axis. The result is a
    helical surface which can be used to model threads or other
    twisted surfaces. The two most common approaches are to use an
    axis in the sketch plane to create a spiral shape, or an axis
    perpendicular to the sketch plane to create what behaves like a
    twisted version of the standard extrusion.

<p>
    When a Helix group is created, a construction line will also be
    created along the axis of the helix. Dragging the ends of that
    line or any other points on the axis will change the length of
    the helical extrusion. Dragging points that are not on the axis
    will change the angle of the helix similar to a Revolve group.
    The angle of a helix can be much more than 360 degrees to allow
    creation of very long spiral shapes, or all of the threads on a
    bolt in a single group.

<h3><a id="Link" href="#Link" class="anchor"></a>
Link / Assemble</h3>

<p>
    In SolveSpace, there is no distinction between "part" files and
    "assembly" files; it's always possible to link one file into
    another. An "assembly" is just a part file that links one or
    more other parts.

<p>
    The linked file is not editable within the assembly. It is
    included exactly as it appears in the source file, but with an
    arbitrary position and orientation. This means that the linked
    part has six degrees of freedom.

<p>
    To move (translate) the part, click any point on it
    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.

<p>
    The part may also be transformed with a 3Dconnexion six degree of
    freedom controller. To manipulate a part in an assembly, select any
    entity within that part (for example, a point, a line segment, or
    a normal). The 3Dconnexion controller will move that part, instead
    of transforming the view. Be careful not to produce an undesired
    translation into or out of the screen, since that motion may not
    be readily perceptible.

<p>
    To rotate the part by exactly ninety degrees about the coordinate
    axis (x, y, or z axis) closest to perpendicular to the screen, choose
    Edit &rarr; Rotate Imported 90&deg;. If an entity in a linked group
    is selected, then the part from that group will be rotated. If an
    import group is active, then the part from the active group will be
    rotated.

<p>
    The Same Orientation constraint is particularly useful when
    linking parts. This one constraint completely determines the
    linked part's rotation. (Select a normal on the linked part,
    select some other normal to constrain it against, and choose
    Constrain &rarr; Same Orientation).

<p>
    The linked part also has an associated scale factor. This makes
    it possible to link a smaller or larger version of the part. If
    the scale factor is negative, then the part is scaled by the absolute
    value of the scale factor and mirrored.

<p>
    SolveSpace also has the ability to import IDF (.emn) files defining
    printed circuit boards from electronic design tools.
    This is useful for designing enclosures and checking fit within
    an assembly. Sketch entities and an extrusion of the board will
    be created and can be used for taking measurements.
    
<p>
    Import groups have a special "solid model as" option: in addition
    to the usual "union", "difference" and "intersection", they have "assemble".
    The "assemble" option should be used when combining parts that
    should not interfere with each other into an assembly. To
    verify that the assembly does not interfere, choose Analyze
    &rarr; Show Interfering Parts.

<p>
    If an import group contains a sketch that forms a closed contour,
    then that group may be extruded in the same way as if the contour
    had been drawn within the same file. This means that it is possible
    to draw a section in file A, import that section into file B (with
    some arbitrary translation and rotation), and then extrude it to
    form a feature of the part in file B. Any changes to file A will
    propagate into file B when the part is regenerated.

<p>
    Similarly, it's possible to draw an open section in file A, link
    that section into file B, and then draw additional lines or curves
    (in the same group or another group) within file B to close that
    section. If file C links in file B, then the closed section may be
    extruded. This allows the user to reuse sections, or portions of a
    section, in multiple files, in such a way that a change in the
    original will propagate to all the parts that use that geometry.

<p>
    When an assembly file is loaded, SolveSpace loads all of the
    linked files as well. If the linked files are not available,
    then an error occurs. When transfering an assembly file to another
    computer, it's necessary to transfer all of the linked files
    as well.
</div>

<h2><a id="LineStyles" href="#LineStyles" class="anchor"></a>
Line Styles</h2>

<div class="refind">
<p>
It is never possible to change a line or curve's color, line width, or
other cosmetic properties directly. Instead, the cosmetic properties of
an entity may be specified by assigning that entity to a line style. The
style specifies color, line width, text height, text origin, text rotation,
and certain other properties that determine how (and whether) an object
appears on-screen and in an exported file.
</p>

<p>
SolveSpace's basic color scheme is defined by the default styles. To view
them, choose "line styles" from the home screen in the Property Browser. This
is where, for example, lines are specified to be white by default, and
constraints to be magenta, and points to be green. The default styles may
be modified. These modifications will be saved in the user config (the
registry on Windows, a .json file on other platforms), and will apply to
all files opened on that computer.  </p>

<p>
It is also possible to create custom styles, for cosmetic or other purposes.
(For example, laser cutters often use the color of a line to specify the
power and feed with which to cut it.) To create a custom style, choose "new
custom style" in the style screen. The new style will appear at the bottom
of the list of styles, with default name new-custom-style.
</p>

<p>To modify a style, click its link in the list of styles. Color is specified
as red, green, blue, where each component is between 0 and 1. The line width
may be specified either in pixels, or in inches or millimeters. If the
line width is specified in pixels, then the line width in an exported file
will depend on the on-screen zoom level. If the user zooms out (so that the
model appears smaller on screen), then the geometry shrinks but the lines,
measured in pixels, stay the same size; this means that lines will appear
thicker compared to the model in the exported file.</p>

<p>Entities (like lines, circles, or arcs) may be assigned to a line style.
One way to do so is to enter the desired line style's screen in the text
window, and then select the desired entities. Then click the "assign to
style" link in the Property Browser. Another way to do so is to right-click
the entity, and assign it to the style using the context menu.</p>

<p>Comments (Constrain &rarr; Comment) may also be assigned to styles. The
style may be used to specify the text height, the rotation of the text in
degrees, and from what point (top, bottom, left, right, center) the text
is aligned. The snap grid (View &rarr; Show Snap Grid, Edit &rarr; Snap to
Grid) is often useful when creating cosmetic text.</p>

<p>User-created styles are saved in the .slvs file, along with the geometry.
If a part with user-created styles is linked in, then the styles are not
imported; but the style identifiers for the linked in entities are maintained.
This means that the user can specify the line styles in the file doing the
linking (i.e., the "assembly").</p>

<p>If a style is hidden, then all objects within that style will be hidden,
even if their group is shown. If a style is not marked exportable, then
objects within that style will appear on-screen, but will not appear in an
exported file. This behavior is similar to that of construction lines.</p>

<p>Not all export file formats support all line style information. For
example, lines in an HPGL file are exported without any line width
or color.</p>

</div>

<h2><a id="Analysis" href="#Analysis" class="anchor"></a>
Analysis</h2>

<div class="refind">
<h3><a id="Trace" href="#Trace" class="anchor"></a>
Trace Point</h3>

<p>
    SolveSpace can draw a "trail" behind a point as it moves. This
    is useful when designing mechanisms. The sketch shown below is
    a four-bar linkage:

<div class="forimg">
    <img src="pics/ref-point-traced.png">
</div>

<p>
    As the linkage is worked, the midpoint of the top link moves
    along the cyan curve. This image was produced by drawing the
    linkage, tracing that midpoint, and then dragging the linkage
    through its full range of motion with the mouse.

<p>
    To start tracing, select a point, and choose Analyze &rarr; Trace
    Point. When the point moves, a cyan trail will be drawn behind it.

<p>
    To stop tracing, choose Analyze &rarr; Stop Tracing. A dialog
    will appear, with the option to save the trace as a CSV
    (comma-separated value) file. To save the trace, enter a
    filename. To abandon the trace, choose Cancel or hit Esc.

<p>
    The trace is saved as a text file, with one point per line. Each
    point appears in the format x, y, z, separated by commas. Many
    programs, including spreadsheets like Excel, can read this format.
    The units for the coordinates are determined by the export
    scale factor. (If the export scale factor is 1, then they are
    millimeters, and if it's 25.4, then they're inches.)

<p>
    If the mechanism is worked by dragging it with the mouse, then
    the points in the trace will be unevenly spaced, because the
    motion of the mouse is irregular. A plot of x vs. y (like the
    cyan trace above) is not affected, but a plot of x or y vs. t
    is useless, because the "speed" along the curve is not constant.

<p>
    To avoid this problem, move the point by stepping a dimension,
    rather than by dragging with the mouse. Select the dimension to
    be stepped; this can be any distance or angle. Choose Analyze &rarr;
    Step Dimension. Enter the new final value for that dimension,
    and the number of steps; then click "step dimension now".

<p>
    The dimension will be modified in multiple steps, and solved
    at each intermediate value. For example, consider a dimension
    that is now set to 10 degrees. The user steps this dimension to
    30 degrees, in 10 steps. This means that SolveSpace will solve
    at 12 degrees, then 14 degrees, then 16, and so on, until it
    reaches 30 degrees.

<p>
    The position of the traced point will be recorded at each
    intermediate value. When the trace is exported, it represents
    the position of that point, as the dimensioned link rotates with
    constant angular speed.

<p>
    The step dimension feature can also improve convergence. In some
    difficult cases, the solver will fail to find a solution when a
    dimension is changed. If the specified constraints have multiple
    solutions, then the solver may also find an undesired solution. In
    this case, it may be useful to try stepping the dimension to
    its new value, instead of changing it in a single step.

<h3><a id="MeasureVolume" href="#MeasureVolume" class="anchor"></a>
Measure Volume</h3>

<p>
    This feature reports the volume of the part. Depending on
    the active units, the volume is given in cubic inches, or in
    millilitres and cubic millimeters.

<p>
    If the part contains smooth curves (e.g. circles), then the
    mesh is not an exact representation of the geometry. This means
    that the measured volume is only an approximation; for a mesh
    that looks fairly smooth on-screen, expect an error around one
    percent. To decrease this error, choose a finer chord tolerance.

<h3><a id="MeasureArea" href="#MeasureArea" class="anchor"></a>
Measure Area</h3>

<p>
    This feature reports the area of the current sketch. Depending on
    the active units, the area is given in square inches, or in square
    millimeters.

<p>
    The area measurement is calculated using a piecewise linear
    approximation to any curves. This introduces some error; to decrease
    that error, choose a finer chord tolerance. If the current sketch is
    not a well-formed plane curve (for example, if it isn't a closed
    curve, or if it intersects itself) then an error is reported,
    because the area cannot be defined.

<h3><a id="Show" href="#Show" class="anchor"></a>
Show Degrees of Freedom</h3>

<p>
    This feature indicates which points in the sketch are not completely
    constrained (i.e., which points would move if the user dragged them
    with the mouse). The free points are drawn with a large cyan square
    over them. In a sketch with zero degrees of freedom, nothing would
    be drawn. In a sketch with one degree of freedom, one or more points
    would be marked; it's possible that more than one point would be
    marked, since that one degree of freedom might be draggable via
    multiple points.

<p>
    To erase the large cyan squares, re-solve the sketch by choosing
    Edit &rarr; Regenerate All or by dragging a point.

</div>

<h2><a id="Export" href="#Export" class="anchor"></a>
Export</h2>

<div class="refind">
<h3><a id="Bitmap" href="#Bitmap" class="anchor"></a>
Bitmap Image</h3>

<p>
    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 output.

<p>
    Choose File &rarr; Export Image. The file is exported as a PNG,
    which most graphics software can open.

<h3><a id="2dSection" href="#2dSection" class="anchor"></a>
2d Section</h3>

<p>
    This option will cut the solid model along a specified plane. All
    lines and curves from the solid model that lie in this plane will
    be exported. Lines and curves from the solid model that do not lie
    in this plane are ignored. Lines and curves that do not come from
    the solid model (for example, a line in a sketch that has not been
    extruded) are ignored. This option is typically appropriate when
    generating 2d CAM data from a 3d model, for example for a laser or
    waterjet cutter.

<p>
    Before exporting a section, it is necessary to specify which plane of
    the part should be exported. This may be specified by:

    <table class="cellpad">
    <tr>
    <td class="showleft"><p>a face</p></td>
    <td class="showright"><p>
        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 Property Browser.
    </p></td>

    </tr><tr>

    <td class="showleft"><p>a point, and two lines or vectors</p></td>
    <td class="showright"><p>
        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
        exported file. Whichever line is more horizontal in the current
        view becomes the x axis, and the other one becomes the y.</p>

        <p>This means that it's possible to rotate the exported file
        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 file is mirrored.
    </p></td>

    </tr><tr>

    <td class="showleft"><p>the active workplane</p>
    <td class="showright"><p>
        If a workplane is active, and nothing is selected when the
        export command is chosen, then SolveSpace 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 exported file.</p>
    </td>
    </tr>
    </table>

<p>
    The units of the exported file are determined by the export scale
    factor, which may be specified in the configuration screen.
</p>
<p>
    If the
    sketch contains curves, then the exported file may represent those
    curves exactly (for example, a circle in an SVG file, since SVG
    supports exact circles), approximately but with a smooth curve
    (for example, a circle in a PDF file, since PDF supports only cubic
    splines, which can't represent a circle exactly), or as piecewise
    linear segments (for example, a circle in an HPGL file). To force
    curves to be output as piecewise linear, choose "curves as piecewise
    linear" in the configuration screen. Colors in the output file may
    not exactly match colors of the model viewed on-screen, depending
    on the color space used by your viewer.
</p>

<h3><a id="2dView" href="#2dView" class="anchor"></a>
2d View</h3>

<p>
    This option will project the 3d model onto a plane, in the same way
    that it is projected when you view the model on screen. Lines and
    curves that happen to lie in the projection plane are exported without
    any changes; lines and curves that do not lie in the projection plane
    will appear shortened due to the projection.

<p>
    This option is typically appropriate when generating a human-readable
    drawing in vector format. It is also useful because it exports all
    lines, not just lines from the solid model; so if the user draws a
    sketch from lines and curves, but does not wish to extrude it to form
    a solid model, then they can extrude their bare sketch using this
    option. This may be desirable when using SolveSpace for 2d drawing.

<p>
    The projection plane is selected by rotating the model on-screen, by
    center-dragging with the mouse. The origin of the exported file
    corresponds to the center of the view on screen, and may therefore
    be moved by panning (by right-dragging with the mouse). To specify
    the projection plane exactly, orient the view onto a workplane,
    or use the View &rarr; Nearest Ortho / Iso View and View &rarr;
    Center View at Point commands.

<p>
    By default, the view will be output with hidden lines removed,
    and additional lines will be drawn wherever a curved surface turns
    from front-facing to back-facing. This is typically the desired
    result. To create a wireframe view of the part, show "hidden-lns"
    before exporting.
</p>

<p>
    Some file formats (EPS, SVG, PDF) support shaded surfaces. If the
    user is exporting to such a file format, and the "export shaded
    2d triangles" option is set in the configuration screen, then the
    view will contain flat-shaded surfaces of the model. Lighting is
    calculated in the same way as for the view of the model on-screen. It
    may therefore be modified by changing the light directions and
    intensities in the configuration screen.
</p>

<p>
    The units of the exported file are determined by the export scale
    factor, which may be specified in the configuration screen.  If hidden
    line removal is performed (for example, if a solid model is present),
    then the exported file will contain only line segments; all curves
    are broken down into lines, with the specified chord tolerance. If
    no hidden line removal is performed (for example, if nothing has
    been extruded or lathed, so no solid model is present) then curves
    will be exported in exact form when possible.

<p>
    Normals, datum points and image entities are not exported for vector
    formats.

<h3><a id="3dWireframe" href="#3dWireframe" class="anchor"></a>
3d Wireframe</h3>

<p>
    This option behaves almost identically to File &rarr; Export 2d View;
    but instead of projecting the lines and curves into the specified
    2d plane, it exports the lines and curves in 3d.

<p>
    The 3d wireframe does not contain any surfaces or solids. This means
    that it is generally not appropriate for the viewing or manufacturing
    of solid parts. For that, use a triangle mesh or a NURBS surface (STEP)
    file.

<h3><a id="Triangle" href="#Triangle" class="anchor"></a>
Triangle Mesh (STL, OBJ)</h3>

<p>
    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.

<p>
    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.

<p>
    The units of the STL file are determined by the export scale
    factor, which may be specified in the configuration screen.

<h3><a id="NURBS" href="#NURBS" class="anchor"></a>
NURBS Surfaces (STEP)</h3>

<p>
    If the model is represented as NURBS surfaces (and not just as a triangle
    mesh), then the user can export those exact surfaces as a STEP file.
    When this is possible, it is usually the best choice, since it does not
    introduce any error. Many CAM, rapid prototyping, and other CAD tools
    will accept a STEP file.
<p>
    The STEP file will always indicate millimeter units, no matter what
    scale factor is applied.

</div>

<h2><a id="Configuration" href="#Configuration" class="anchor"></a>
Configuration</h2>

<div class="refind">
<h3><a id="Material" href="#Material" class="anchor"></a>
Material Colors</h3>

<p>
    In the Property Browser 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.

<p>
    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".

<p>
    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><a id="Light" href="#Light" class="anchor"></a>
Light Directions</h3>

<p>
    The 3d part is displayed with simulated lighting, to produce the
    impression of depth. There are two types of lights, directional and
    ambient.  The directions and intensities of these lights may be
    modified according to user preference.

<p>
    Directional 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 ambient
    light has no direction and acts as a fill light of uniform intensity
    from all directions.

<p>
    The intensity must lie between 0 and 1. A light with intensity
    0 has no effect, and 1 is full brightness.  Lighting from ambient and
    directional lights is additive.  If the ambient light intensity is set
    to 1 a "flat shading" effect will be achieved.

<p>
    Two directional 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><a id="Chord" href="#Chord" class="anchor"></a>
Chord Tolerance, and Max Segments</h3>

<p>
    SolveSpace does not always represent curved edges or surfaces
    exactly. Curves are sometimes broken down into piecewise linear
    segments, and surfaces are sometimes broken down into triangles.


<p>
    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.

<p>
    There are two chord tolerance values in the configuration screen.
    The first is specified as a percent of the overall size of the
    sketch and its value in length units is also calculated and shown.
    This means a sketch consisting of a single circle will have very
    smooth curves, while a large object with small holes may have
    fewer segments because the hole is much smaller than the overall
    sketch and closer in size to the chord tolerance.
    
<p> The second value is the "export chord tolerance" which is an
    absolute value in mm. When exporting a triangle mesh for 3d printing
    or g-code for machining, this value will determine how much the
    resulting part can deviate from the ideal curved surfaces.
    
<p>
    When combining NURBS surface or triangle meshes from different
    groups, SovleSpace uses the chord tolerance in some calculations.
    That means when a boolean operation fails, making adjustments to
    the chord tolerance can "fix" the problem in some cases.

<p>
    The fineness of the mesh is also limited by the specified maximum
    number of piecewise linear segments. A single curve will never
    be broken down into more than that number of line segments,
    no matter how fine the chord tolerance.

<h3><a id="Perspective" href="#Perspective" class="anchor"></a>
Perspective Factor</h3>

<p>
    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.

<p>
    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.

<p>
    The image below is a perspective projection. All of the square
    cutouts are the same size, but the ones at the front (closer to
    the viewer) are drawn larger, and the ones at the back are drawn
    smaller.

<div class="forimg">
    <img src="pics/ref-perspective.png">
</div>

<p>
    The next image is a parallel projection. All of the square
    cutouts are the same size on the drawing. (The cutouts at the
    top might look slightly larger, but that is an optical illusion,
    because the eye is accustomed to seeing images with perspective.)

<div class="forimg">
    <img src="pics/ref-no-perspective.png">
</div>

<p>
    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.

<p>
    By default, SolveSpace displays a parallel projection. To display a
    perspective projection, choose View &rarr; Use Perspective Projection,
    and make sure that the perspective factor is not zero. By default,
    the perspective factor is 0.3. The distance from the "camera" to
    the model is equal to one thousand pixels divided by the perspective
    factor.

<h3><a id="Snap" href="#Snap" class="anchor"></a>
Snap Grid Spacing</h3>

<p>
    This specifies the pitch of the snap grid, in inches or millimeters. By
    default, the grid is not displayed; it may be shown by choosing View
    &rarr; Show Snap Grid. Points are never automatically snapped to the
    grid. To snap a point, select that point, and then choose Edit &rarr;
    Snap to Grid. Comments (Constrain &rarr; Comment, cosmetic text) may
    be snapped to grid in the same way.
</p>

<h3><a id="ExportScale" href="#ExportScale" class="anchor"></a>
Export Scale Factor</h3>

<p>
    Internally, SolveSpace represents lengths in millimeters. Before
    exporting geometry, these lengths are divided by the export scale
    factor. This scale factor determines the units for the exported file.

<p>
    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.

<p>
    SolveSpace 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, and text would appear mirrored).

<h3><a id="Cutter" href="#Cutter" class="anchor"></a>
Cutter Radius Offset</h3>

<p>
    When exporting a 2d view or section, this option may be used to
    apply cutter radius compensation. All curves in the exported geometry
    are offset by the specified radius. This may in some cases make it
    possible to work without dedicated CAM software.
</p>

<p>
    The cutter radius is specified in inches or millimeters, according
    to the current mode. To disable cutter radius compensation, set this
    offset to zero.
</p>

<p>
    The cutter radius compensation works only on piecewise linear
    segments. This means that curves (circles, Beziers, etc.) will be
    approximated as line segments in the output file, even if
    "curves as piecewise linear" is set to "no".
</p>

<h3><a id="ExportShaded" href="#ExportShaded" class="anchor"></a>
Export Shaded 2d Triangles</h3>

<p>
    When exporting a view of the part, the user can export only the
    edges of the part (to produce a wireframe or hidden line removed
    drawing), or the user can export flat-shaded surfaces, to show
    the color and lighting of the faces of the part.

<p>
    Not all export file formats support shaded triangles; currently,
    SVG, EPS, and PDF do, but DXF and HPGL do not.

<h3><a id="ExportCurves" href="#ExportCurves" class="anchor"></a>
Export Curves as Piecewise Linear</h3>

<p>
    A smooth curve (like a circle, or a Bezier curve) may be exported
    in one of two ways: either exactly, or as a set of line segments
    that approximates it. If this box is not checked, then whenever
    possible, geometry will be output as exact curves. If it is checked,
    then curves will always be exported as piecewise linear
    segments.

<p>
    This option is useful because some CAM or other software is incapable
    of importing exact curves, but almost all software will be capable
    of importing piecewise linear segments.

<h3><a id="ExportCanvas" href="#ExportCanvas" class="anchor"></a>
Export Canvas Size</h3>

<p>
    This specifies the canvas size for any exported 2d geometry. For example,
    the canvas size in a PDF file is the paper size, and the canvas size
    in a PostScript file is the EPS BoundingBox. This may be specified in
    one of two ways: either as a fixed size, or as a set of margins around
    the exported geometry.

<h3><a id="FixWhite" href="#FixWhite" class="anchor"></a>
Fix White Exported Lines</h3>

<p>
    By default, SolveSpace draws white lines on a black background. But
    most export file formats assume a white background, which means that
    white lines would be illegible. By default, SolveSpace will rewrite any
    white (lighter than approximately 75% gray) colors to black when
    exporting into such a file format. That behavior may be disabled with
    this option.

<h3><a id="Draw" href="#Draw" class="anchor"></a>
Draw Triangle Back Faces in Red</h3>

<p>
    SolveSpace always works with solid shells. This means that in
    normal operation, only the outside of a surface should be visible.
    This setting should therefore have no effect.

<p>
    If a self-intersecting shell is drawn, then inside surfaces may
    be exposed. Even if the shell is watertight, a few stray pixels
    from an inside surface may "show through", depending on how the
    graphics card renders triangles. This setting determines whether
    those surfaces are discarded, or drawn highlighted in red.

<h3><a id="Check" href="#Check" class="anchor"></a>
Check for Closed Contours</h3>

<p>
    Most solid operations (like extrudes and lathes) work only on closed,
    planar sections that are not self-intersecting. By default, SolveSpace
    will warn the user if the sketched section violates any of these
    rules, by indicating the problem on the sketch. For example, if a
    contour is open, then a message is drawn at one of the hanging endpoints.
    If a contour is self-intersecting, then a message is drawn at the
    intersection.

<p>
    For general 2d and 3d wireframe CAD work, this behavior may not be
    desired. The warnings may therefore be disabled with this option.

<h3><a id="GCode" href="#GCode" class="anchor"></a>
G Code Parameters</h3>

<p>SolveSpace is not a CAM program, but it is capable of exporting
simple G code for 2d parts. By applying the correct cutter radius
compensation (or by drawing the sketch with the cutter radius in mind),
it is possible to profile 2d parts with no additional CAM software. The
part is assumed to lie in the XY plane. The cutting depth along the Z axis
is as specified here; enter a positive or negative value, depending on
which sign corresponds to down. The top of the workpiece is assumed to
lie at Z = 0, and the cutter will move to a clearance plane 5mm above
the workpiece while slewing.</p>

<p>All units are in either inches or millimeters (or inches or millimeters
per minute, for the feeds), according to the current mode.</p>

</div>

<h2><a id="Known" href="#Known" class="anchor"></a>
Known Bugs and Issues</h2>

<div class="refind">

<p>
    When Boolean operations are performed on triangle meshes (instead
    of exact NURBS surfaces), the resulting mesh quality will often be
    poor. An equally good mesh might have been achieved with fewer
    triangles, if the curves were piecewise-linear approximated
    differently. Or the mesh may contain long skinny triangles.

<p>
    This means that the exported STL files will not contain a high
    quality mesh. This is generally not a problem, but could be in
    some applications. In particular, the exported mesh may no
    longer be exactly 2-manifold (i.e., watertight). Check for this
    problem with Analyze &rarr; Show Naked Edges.

<p>
    Another consequence is that the program runs slower as the number
    of triangles increases. It's a good idea to draw with a fairly
    coarse mesh. Before exporting, reduce the chord tolerance; the
    part will be regenerated with a finer mesh.

<p>
    When Boolean operations are performed on NURBS surfaces, the mesh
    quality will in general be much better. But some types of surface
    intersection are not handled by the current NURBS Booleans, so it
    may in some cases be impossible to perform the desired operation
    as a NURBS Boolean.

<p>
    The NURBS Booleans are also affected by the chord tolerance.
    Operations may fail if that tolerance is too coarse, but the routines
    become slower as the tolerance gets finer. If problems occur, then
    it is often useful to change that tolerance.

<p>
    To improve speed and mesh quality, draw the part using fewer Boolean
    operations. For example, a plate with a hole might be modeled in
    two different ways. The user might extrude the plate, and then cut
    a hole by extruding a circle as difference. Or the user might draw
    a single sketch with both the outline of the plate and the hole,
    and extrude only once. The latter option is preferable. The trim
    command (Sketch &rarr; Split Curves at Intersection) may be useful
    while drawing complicated sections.
</div>

EOT
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