solvespace/doc/reference.txt

<h2>General Navigation</h2>

    <h3>Model View</h3>

        To pan the view, center-drag with the mouse. (The center button
        is typically actuated by pressing on the scroll wheel.)

        To rotate the view, right-drag with the mouse. This will rotate
        the part about a horizontal or vertical axis. To rotate the part
        within the plane of the screen, Ctrl+right-drag with the mouse.

        To zoom in or out, rotate the scroll wheel. It is also possible
        to zoom in or out by using the View menu, or the associated
        keyboard shortcuts (+ and -).

        It is also possible to pan by Shift+right-dragging, or to rotate
        by Shift+center-dragging. This makes MechSketch usable on certain
        laptop keyboards that don't provide a center mouse button.

        If a workplane is active, then choose Sketch -> In Workplane (or
        press W) to align the view to the workplane. After doing this,
        the plane of the screen is coincident with the workplane.

    <h3>Dimension Entry and Units</h3>

        Dimensions may be displayed in either millimeters or inches.
        Millimeter dimensions are always displayed with two digits
        after the decimal point (45.23), and inch dimensions are always
        displayed with three (1.781).

        Choose View -> Dimensions in ... to change the current display
        units. This does not change the model; if the user changes from
        inches to millimeters, then a dimension that was entered as 1.0
        is now displayed as 25.40.

        All dimensions are entered in the current display units. In most
        places where a dimension is expected, it's possible to enter an
        arithmetic expression ("4*20 + 7") instead of a single number.

    <h3>Show / Hide Entities</h3>

        As the sketch becomes more complex, it may be useful to hide
        unnecessary information. MechSketch provides several different
        controls for this.

        In the second and third line of the text window, links are
        provided to hide and show different types of entity. These are:

               wrkpls  -- When a new "Sketch In New Workplane" group is
                          created, an associated workplane is created
                          automatically. If wrkpls is hidden, then that
                          workplane is visible only when its associated
                          group is active. If wrkpls is shown, then the
                          workplane is always visible.

               normals -- By default, normals are drawn as blue-grey arrows,
                          in the direction of the normal. These normals may
                          be hovered and selected with the mouse, for
                          example in order to constrain them. This link
                          may be used to hide them.

               points  -- By default, points are drawn as green squares.
                          These points may be hovered and selected with the
                          mouse, for example in order to constrain them.
                          This link may be used to hide them. If points are
                          hidden, then they will still appear when the mouse
                          hovers over them, and may still be selected.

            constraints - When a constraint is created, a graphical
                          representation of that constraint is displayed
                          in purple. The constraints in a group are
                          visible only when that group is active. To hide
                          them even then, use this link.

               shaded --  The 3d part is displayed as an opaque solid,
                          with lighting effects to give the impression of
                          depth. This link may be used to disable that
                          view.

               faces  --  Some surfaces on the 3d model may be selected.
                          For example, the user can select a plane face
                          of the part, and constrain a point to lie on
                          that plane. If faces are shown, then the faces
                          will appear highlighted when the mouse hovers
                          over them. The user can click the mouse to
                          select the face, as they would for any other
                          entity.

                          As a convenience, faces are automatically
                          hidden when a new sketch group is created,
                          and automatically shown when a new extrusion is
                          created. If this behavior is not what's desired,
                          then the faces can be shown or hidden manually
                          with this link.

                 mesh --  The 3d model of the part consists of many
                          triangles; for example, a flat polygon with
                          n sides is broken down into n - 2 triangles.
                          Use this link to show the triangles on the
                          model. In general, this is useful only for
                          debugging, or to see how fine the mesh is
                          before exporting it.

           hidden-lines - With the part in a given orientation, some of
                          the lines in the part will be invisible,
                          because an opaque solid is between the line and
                          the "camera". To show those lines anyways, as
                          if the part were transparent, use this link.
                          This may be useful when creating a sketch that
                          lies within the volume of the part.

        In addition to the above options, it is possible to hide and show
        entire groups. If a group is hidden, then all of the entities
        (line segments, circles, arcs, points, etc.) from that group
        are hidden.

        To hide a group, go to the home screen in the text window, by
        pressing Esc or choosing the link at the top left. A list of
        groups is displayed, along with their visibility. If a group is
        visible, then the "show" column contains the word "yes" in green.
        Click the "yes"; it now appears as a greyed "no", and the group
        is hidden.

        The show / hide status of groups is saved in the part file. If
        a part is imported into an assembly, then entities that were
        visible in the part file will be visible in the assembly, and
        entities that were hidden will be hidden.

    <h3>Active Workplane</h3>

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

        This freedom is not always useful, so MechSketch also makes it
        possible to draw in a plane. If a workplane is active, then all
        entities that are drawn will be constrained to lie that plane.

        When MechSketch starts with a new empty file, a workplane parallel
        to the XY plane is active.

    <h3>Active Group</h3>

        Any groups that go after the active group will be hidden



<h2>Sketch Entities</h2>

    <h3>Datum Point</h3>

    <h3>Workplane</h3>

    <h3>Line Segment</h3>

    <h3>Rectangle</h3>

        A rectangle consists of two vertical line segments, and two
        horizontal line segments, arranged to form a closed curve.
        Initially, the rectangle is specified with the mouse by two
        diagonally opposite corners. The line segments (and points)
        in the rectangle may be constrained in the same way as ordinary
        line segments.

        It would be possible to draw the same figure by hand, by drawing
        four line segments and inserting the appropriate constraints. The
        rectangle command is a faster way to draw the exact same thing.

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

    <h3>Circle</h3>

    <h3>Arc of a Circle</h3>

        Tangent arcs may be created automatically. To do so, first select
        a point where two line segments join. Then choose Sketch ->
        Arc of a Circle; the arc will be created, and automatically
        constrained tangent to the two line segments.

        The initial line segments will become construction lines, and
        two new lines will be created, that join up to the arc.

        The arc's diameter may then be constrained in the usual way, with
        Distance / Diameter or Equal Length / Radius constraints. This
        is a simple way to round a sharp corner.

    <h3>Bezier Cubic Segment</h3>

    <h3>Text in a TrueType Font</h3>


<h2>Constraints</h2>
    
    <h3>General</h3>

    <h3>Reference Dimensions</h3>

        By default, the dimension drives the geometry. If a line segment
        is constrained to have a length of 20.00 mm, then the line
        segment is modified until that length is accurate.

        A reference dimension is the reverse: the geometry drives the
        dimension. If a line segment has a reference dimension on its
        length, then it's still possibly to freely change that length,
        and the dimension displays whatever that length happens to be. A
        reference dimension does not constrain the geometry.

        To change a dimension into a reference dimension, choose
        Constrain -> Toggle Reference Dimension. A reference dimension
        is drawn with "REF" appended to the displayed length or angle.
        Double-clicking a reference dimension does nothing; the dimension
        is specified by the geometry, not the user.

    <h3>Angle</h3>

        When two lines intersect, four angles are formed. The
        opposite angles are equal; to change which opposite angle is
        displayed, drag the label, and the arc will follow. If the wrong
        supplementary angle is displayed, then select the constraint
        and choose Constrain -> Other Supplementary Angle.

    <h3>Comment</h3>

        A comment is a single line of text that appears on the drawing.
        When the comment is created, it appears in the center of the
        screen. To move the comment, drag it with the mouse. To change
        the text, double-click it.

        The comment has no effect on the geometry; it is only a
        human-readable note.


<h2>Groups</h2>

    <h3>General</h3>

        All groups have a name. When the group is created, a default name
        (e.g., "g008-extrude") is assigned. The user may change this name;
        to do so, go to the group's page in the text window, and choose
        [rename].

        Groups that create a solid (e.g. extrudes or sweeps) have a "MERGE
        AS" option, which is displayed in the page in the text window.
        The group can be merged as union, which adds material to the
        model, or as difference, which cuts material away.

        The group's page in the text window also includes a list of all
        requests, and of all constraints. To identify a constraint or a
        request, hover the mouse over its name; it will appear highlighted
        in the graphics window. To select it, click on the link in the
        text window. This is equivalent to hovering over and clicking
        the actual object in the graphics window.


    <h3>Sketch in 3d</h3>

    <h3>Sketch in New Workplane</h3>

        A point and two line segments

            The new workplane has its origin at the specified point. The
            workplane is parallel to the two lines. If the point and
            two are two edges on a plane face of the part, and a vertex
            on that plane face, then the resulting workplane will be
            coincident with that face (i.e., the user will be drawing
            on that face).

        A point

            The new workplane has its origin at the specified point. The
            workplane is orthogonal to the base coordinate system; for
            example, its horizontal and vertical axes might lie in the
            +y and -z directions, or +x and -z, or any other combination.

            The orientation of the workplane is inferred from the
            position of the view when the workplane is created; the
            view is snapped to the nearest orthographic view, and the
            workplane is aligned to that.

            If a part consists mostly of ninety degree angles, then this
            is a quick way to create workplanes.

    <h3>Step Translating</h3>

    <h3>Step Rotating</h3>

    <h3>Extrude</h3>

        If a workplane is active when the group is created, then the
        extrude path is automatically constrained to be normal to that
        workplane. This means, for example, that a rectangle is extruded
        to form a rectangular prism. The extrusion has one degree of
        freedom, so a single distance constraint will fully constrain it.
        This is usually the desired behaviour.

        If no workplane is active when the group is created, then the
        extrude path may be in any direction. This means that a rectangle
        could be extruded to form a parallelepiped. The extrusion has
        three degrees of freedom. This is not typically useful.

    <h3>Lathe</h3>

    <h3>Sweep</h3>

    <h3>Helical Sweep</h3>

    <h3>Import / Assemble</h3>

        In MechSketch, there is no distinction between "part" files and
        "assembly" files; it's always possible to import one file into
        another. An "assembly" is just a part file that imports one or
        more other parts.

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

        To move (translate) the part, click any point on the imported
        part and drag it. To rotate the part, click any point and Shift+
        or Ctrl+drag it. The position and orientation of the part may be
        fixed with constraints, in the same way that any other geometry
        is constrained.

        The Same Orientation constraint is particularly useful when
        importing parts. This one constraint completely determines the
        imported part's rotation. (Select a normal on the imported part,
        select some other normal to constrain it against, and choose
        Constrain -> Same Orientation).

        Import groups have a special "MERGE AS" option: in addition
        to the usual "union" and "difference", they have "assemble".
        The "assemble" option is identical to "union", except that
        it displays a warning if the components intersect with each
        other. This is useful when checking to see if the assembled parts
        interfere. If the parts interfere, then a warning is displayed
        underneath the "MERGE AS" line in the group's text window page.
        The interfering surfaces are also highlighted in the graphics
        window, in red with black stripes.

        When an assembly file is loaded, MechSketch loads all of the
        imported files as well. If the imported files are not available,
        then an error occurs. When transfering an assembly file to another
        computer, it's necessary to transfer all of the imported files
        as well.


<h2>Export</h2>

    <h3>Bitmap Image</h3>

        This option will export a bitmap image of whatever is displayed
        on-screen. It is equivalent to taking a screenshot. This option
        is useful for producing human-readable drawings.

        Choose File -> Export Image. The file is exported as a PNG,
        which most graphics software can open.

    <h3>2d Vector (DXF)</h3>

        This option will generate a 2d vector file that represents a
        specified plane in the part. Most 2d CAM software, including the
        software that ships with laser or waterjet cutters, will accept
        a DXF file.

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

        a face:

            Any surfaces coplanar with that plane face will appear in the
            file. The faces must be shown before they can be selected;
            click the link in the third line of the text window.

        a point, and two lines or vectors:

            The export plane is through the point, and parallel to
            the two lines or vectors. If the two lines or vectors are
            perpendicular, then they will become the x and y axis in the
            DXF file. Whichever line is more horizontal in the current
            view becomes the x axis, and the other one becomes the y.

            This means that it's possible to rotate the exported DXF
            through ninety degrees by rotating the view through ninety
            degrees (in the plane of that face). Similarly, by rotating
            the part around to look at the face from behind instead of
            in front, the exported DXF is mirrored.

        the active workplane

            If a workplane is active, and nothing is selected when the
            export command is chosen, then MechSketch will export any
            surfaces that are coplanar with the active workplane. The
            workplane's horizontal and vertical axes become the x and
            y axis in the DXF file.

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

    <h3>3d Mesh (STL)</h3>

        This option will generate a 3d triangle mesh that represents
        the entire part. Most 3d CAM software, including the software
        for most 3d printers, will accept an STL file.

        The mesh from the active group will be exported; this is the
        same mesh that is displayed on screen. The coordinate system
        for the STL file is the same coordinate system in which the part
        is drawn. To use a different coordinate system (e.g., to rotate
        or translate the part), create an assembly with the part in the
        desired position, and then export an STL file of the assembly.

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

<h2>Configuration</h2>

    <h3>Material Colors</h3>

        In the text window screen for certain groups (extrude, lathe,
        sweep), a palette of eight colors is displayed. This palette
        allows the user to choose the color of any surfaces generated
        by that group.

        These eight colors are specified here, by their components.
        The components go from 0 to 1.0. The color "0, 0, 0" is black,
        and "1, 1, 1" is white. The components are specified in the order
        "red, green, blue".

        A change to the palette colors does not change the color of any
        existing surfaces in the sketch, even if the color of an existing
        surface no longer appears in the palette.

    <h3>Light Directions</h3>

        The 3d part is displayed with simulated lighting, to produce
        the impression of depth. The directions and intensities of these
        lights may be modified according to user preference.

        The lights do not have a position; they have only a direction,
        as if they were coming from very far away. This direction is
        specified in 3 components, "right, top, front". The light with
        direction "1, 0, 0" is coming from the right of the screen.
        The light with direction "-1, 0, 0" is coming from the left of
        the screen. The light with direction "0, 0, 1" is coming from
        in front of the screen.

        The intensity must lie between 0 and 1. A light with intensity
        0 has no effect, and 1 is full brightness.

        Two lights are available. If only one is desired, then the second
        may be disabled by setting its intensity to zero. When the part
        is rotated or translated, the lights do not move.

    <h3>Chord Tolerance</h3>

        MechSketch does not represent curved edges or surfaces exactly.
        Any curves are broken down into piecewise linear segments,
        and surfaces are represented as triangles.

        This introduces some error. The chord tolerance determines how
        much error is introduced; it is the maximum distance between
        the exact curve and the line segments that approximate it. If
        the chord tolerance is decreased, then more line segments will
        be generated, to produce a better approximation.

        The chord tolerance is specified in units of screen pixels. This
        means that when the user zooms in on the model, a better
        approximation is produced.

        The same tolerance is used for the mesh that's displayed on
        screen, and for the mesh that is used to export to a file. It
        may be helpful to use a large chord tolerance (2-5 pixels) while
        drawing, for fast response, and then temporarily specify a small
        chord tolerance (~0.5 pixels) before exporting an STL or DXF file.

    <h3>Perspective Factor</h3>

        To display a 3d part on-screen, it must be projected into 2d. One
        common choice is a parallel projection. In a parallel projection,
        any two lines that are parallel in real life are also parallel
        in the drawing. A parallel projection is also known as an
        axonometric projection. Isometric and orthographic views are
        examples of parallel projections.

        Another way to transform the image into 2d is with a perspective
        projection. In a perspective projection, objects closer to the
        "camera" appear larger than objects that are farther away. This
        means that some lines that are parallel in real life will not be
        parallel in the drawing; they will converge at a vanishing point.

        A perspective projection will often look more realistic, and
        gives a better impression of depth. The disadvantage is that
        the perspective distorts the image, and may cause confusion.

        By default, MechSketch displays a parallel projection. To display
        a perspective projection, set the perspective factor to something
        other than zero. The distance from the "camera" to the model is
        equal to one thousand pixels divided by the perspective factor.

    <h3>Edge Color</h3>

        The surfaces of the 3d part are shaded according to the specified
        lighting. Different faces will catch the light at slightly
        different angles, and will therefore appear slightly brighter
        or darker. This permits the viewer to distinguish the boundary
        between the faces.

        Depending on the lighting, this may not provided very much
        constrast. To make the edges of the part more visible, it's
        possible to emphasize them with a solid-color line.

        If the edge color is specified as "0,0,0", then no emphasized
        edges will be drawn. If any other color is specified, then the
        edges will be drawn in that color. The edge color is specified
        in the same format as for the material color.

    <h3>Export Scale Factor</h3>

        Internally, MechSketch represents lengths in millimeters. Before
        exporting geometry to an STL or DXF file, these lengths are
        divided by the export scale factor. This scale factor determines
        the units for the exported file.

        If the scale factor is set equal to 1, then exported files are
        in millimeter units. If the scale factor is set equal to 25.4,
        then the exported files are in inch units, since 1 inch = 25.4 mm.

        MechSketch works in a right-handed coordinate system. If the
        scale factor is negative, then the exported file will appear in
        a left-handed coordinate system (so that a right-handed screw
        thread will become left-handed).

<h2>Licensing</h2>

    As downloaded, MechSketch does not include a license file. This means
    that it cannot create files with more than seven groups. Larger files
    may be opened, but not modified. This light version of MechSketch
    is intended for evaluation, but non-commercial / personal use is
    also permitted.

    The licensed version of MechSketch can create files with an unlimited
    number of groups.

    When a license is purchased, a license file ("mechsketch.license")
    will be sent via email. To activate the license, save this file
    somewhere on your computer. In MechSketch, choose Help -> Load
    License... A file dialog box will appear; select the license file.

    No license server or dongle is required, and licenses do not expire.