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-
-This is a reference manual for SolveSpace. This document is not intended
-for new users; to learn about this program, see the video tutorials.
-
-General Navigation
-
- 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 text window provides information about the model,
- and may also be used to modify settings and numerical parameters.
-
- Graphics Window and Model View
-
- To pan the view, right-drag with the mouse.
-
- 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.
-
- To rotate the view within the plane of the monitor,
- Ctrl+center-drag with the mouse.
-
- It is also possible to pan by Shift+center-dragging, or to rotate
- by Shift+right-dragging.
-
- 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.
-
- To zoom to the extent of the part, choose View -> 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.
-
- 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, and
- the center of the workplane is at the center of the screen. The
- zoom level is not affected.
-
- 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.)
-
- Dimension Entry and Units
-
- Dimensions may be displayed in either millimeters or inches.
- Millimeter dimensions are always displayed with two digits
- after the decimal point (45.23), and inch dimensions are always
- displayed with three (1.781).
-
- Choose View -> Dimensions in Inches/Mm 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.
-
- Text Window
-
- The text window appears as a floating palette window. It may
- be shown or hidden by pressing Tab, or by choosing View ->
- Show Text Window.
-
- The text window 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 text window. For
- example, the "home" screen is a list of groups in the sketch:
-
- 
-
- To navigate to a group's page, click on 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 on the word "yes" in the
- "show" column.
-
- As a convenience, the text window will sometimes automatically
- navigate to a page that is likely to be relevant. For example,
- when a new group is created, the text window 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.
-
- When sketch entities are selected (e.g., the user has clicked
- on them with the mouse), information about those entities is
- displayed in the text window. 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.
-
- If multiple entities are selected, then the text window can
- sometimes display information about all of them. These cases
- include:
-
- two points: the distance between the points
-
- a point and a plane face: the distance from the point to the
- plane
-
- two points, and a vector: the distance between the points,
- projected along the vector
-
- two plane faces: the angle between the plane faces
-
-
- Show / Hide Entities
-
- As the sketch becomes more complex, it may be useful to hide
- unnecessary information. SolveSpace provides several different
- ways to do this.
-
- In the second and third line of the text window, links are
- provided to hide and show different things. 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 hide 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 rectangular face is
- represented by two triangles. Use this link to
- show the triangles on the model. This is a good
- way to see how fine or coarse 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 they are buried inside the solid part.
- To show those lines anyways, as if the part
- were transparent, use this link. This is useful
- when drawing 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. 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.
-
- To hide a group, go to the home screen in the text window, by
- pressing Esc or choosing the link at the top left. A list of
- groups is displayed, along with their visibility. If a group is
- visible, then the "show" column contains the word "yes" in green.
- Click the "yes"; it now appears as a greyed "no", and the group
- is hidden.
-
- The show / hide status of groups is saved in the part file. If
- a part is imported into an assembly, then entities that were
- visible in the part file will be visible in the assembly, and
- entities that were hidden will be hidden.
-
- Active Workplane
-
- SolveSpace 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 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 ("wrkpl") is indicated in the top line of
- the text window, at the right.
-
- 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 -> Anywhere In 3d.
-
- To activate a workplane, select it, and then choose Sketch ->
- In Workplane. When a workplane is activated, the view is aligned
- onto that workplane. (The workplane remains active until the
- user chooses Sketch -> 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.)
-
- In a "Sketch in New Workplane" group, the group's associated
- workplane may be activated by choosing Sketch -> In Workplane;
- there is no need to select it first.
-
- Active Group
-
- 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.
-
- In the text window'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 "yes" in the "actv" column. All other groups
- (except g001-#references, which cannot be activated) have "no"
- in that column. To activate an inactive group, click on the "no".
-
-
-Sketch Entities
-
- Construction Geometry
-
- 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.
-
- 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.
-
- To mark an entity as construction-only, choose Sketch -> 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 (or to the section that
- will be extruded or lathed or swept).
-
- Datum Point
-
- This entity is defined by a single point.
-
- 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.)
-
- 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.
-
- Workplane
-
- This entity is specified by a point and a normal. The point
- defines its origin, and the normal defines its orientation.
-
- 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.
-
- It's almost never necessary to create workplanes explicitly.
- Instead, create a new Sketch in New Workplane group.
-
- Line Segment
-
- This entity is specified by its two endpoints. If a workplane is
- active, then the two endpoints will always lie in that workplane.
-
- To create the line segment, choose Sketch -> Line Segment, and
- then left-click one endpoint of the line. Then release the mouse
- button; the other endpoint is now being dragged.
-
- 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.
-
- 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.)
-
- Rectangle
-
- 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.
-
- It would be possible to draw the same figure by hand, by drawing
- four line segments and inserting the appropriate constraints. The
- rectangle command is a faster way to draw the exact same thing.
-
- A workplane must be active when the rectangle is drawn, since
- the workplane defines the meaning of "horizontal" and "vertical".
-
- Circle
-
- This entity is specified by its center point, by its diameter,
- and by its normal.
-
- To create the circle, choose Sketch -> 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.
-
- 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).
-
- 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.
-
- Arc of a Circle
-
- This entity is specified by its center point, the two endpoints,
- and its normal.
-
- To create the arc, choose Sketch -> 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.
-
- 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.
-
- The arc must be drawn in a workplane; it cannot be drawn in
- free space.
-
- Tangent arcs may be created automatically. To do so, first select
- a point where two line segments join. Then choose Sketch ->
- Arc of a Circle; the arc will be created, and automatically
- constrained tangent to the two line segments.
-
- The initial line segments will become construction lines, and
- two new lines will be created, that join up to the arc.
-
- The arc's diameter may then be constrained in the usual way, with
- Distance / Diameter or Equal Length / Radius constraints. This
- is a simple way to round a sharp corner.
-
- Bezier Cubic Segment
-
- This entity is specified by its four Bezier points: two endpoints,
- and two (in general, off-curve) control points.
-
- To create the Bezier cubic, choose Sketch -> Bezier Cubic
- Segment. Then left-click one endpoint of the cubic segment.
- Release the mouse button; the other endpoint of the cubic segment
- is now being dragged.
-
- 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.
-
- Text in a TrueType Font
-
- This entity is defined by two points, at the top left and bottom
- left of the text. The distance between the points determines the
- height of the text; the angle of the line between them determines
- the orientation of the text, and their position determines the
- text's position.
-
- To create the text, choose Sketch -> 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.
-
- To change the font, select the text entity. A list of installed
- fonts appears in the text window; click the font name to select
- it. To change the displayed text, select the text entity and
- click the [change] link in the text window.
-
-
-Constraints
-
- General
-
- 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.
-
- 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.
-
- 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 actually geometry
- in free space.
-
- For example, consider the line shown below:
-
- 
-
- 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.
-
- 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.
-
- 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.
-
- 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.
-
- 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.
-
- Failure to Solve
-
- 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.
-
- 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.
-
- 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 text window:
-
- 
-
- 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 text window; 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.
-
- 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 -> Undo.
-
-
- Reference Dimensions
-
- By default, the dimension drives the geometry. If a line segment
- is constrained to have a length of 20.00 mm, then the line
- segment is modified until that length is accurate.
-
- A reference dimension is the reverse: the geometry drives the
- dimension. If a line segment has a reference dimension on its
- length, then it's still possible to freely change that length,
- and the dimension displays whatever that length happens to be. A
- reference dimension does not constrain the geometry.
-
- To convert 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, so it is
- not meaningful to type in a new value for the reference dimension.
-
- Specific Constraints
-
- 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.
-
- 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 exists, and are noted below.
-
- Distance / Diameter
-
- 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.
-
- 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.
-
- Angle
-
- 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.
-
- 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.
-
- 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.
-
- 
-
- (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.)
-
- 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.
-
- If the wrong supplementary angle is constrained, then select the
- constraint and choose Constrain -> Other Supplementary Angle. A
- constraint of 30 degrees on one supplementary angle is exactly
- equivalent to a constraint of 150 degrees on the other.
-
- Horizontal / Vertical
-
- 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.
-
- A workplane must be active, because the meaning of "horizontal"
- or "vertical" is defined by the workplane.
-
- 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.
-
- On Point / Curve / Plane
-
- This constraint forces two points to be coincident, or a point
- to lie on a curve, or a point to lie on a plane.
-
- 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.
-
- 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.
-
- Equal Length / Radius
-
- This constraint forces two lengths, angles, or radiuses to
- be equal.
-
- 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 -> Other Supplementary Angle, as for the
- angle constraint.
-
- Length Ratio
-
- 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.
-
- 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.
-
- At Midpoint
-
- This constraint forces a point to lie on the midpoint of a line.
-
- 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.
-
- Symmetric
-
- 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.
-
- 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.
-
- Perpendicular
-
- This constraint is exactly equivalent to an angle constraint
- for ninety degrees.
-
- Parallel / Tangent
-
- This constraint forces two vectors to be parallel.
-
- 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.
-
- 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.
-
- 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.
-
- This constraint can also force a line to be tangent to a curve.
- In order to do this, the line must already share an endpoint with
- the curve; this would usually be achieved with a point-coincident
- constraint. The constraint will force them to also be tangent
- at that point.
-
- Same Orientation
-
- This constraint forces two normals to have the same orientation.
-
- 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.
-
- (Technically, a normal represents a rotation matrix from one
- coordinate system to another. It is represented internally as
- a unit quaternion.)
-
- For example, the picture below shows two workplanes, whose
- normals are constrained to be parallel:
-
- 
-
- 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.
-
- If we replace the "parallel" constraint with a "same orientation"
- constraint, then the two workplanes become identical, and the
- two horizontal lines become parallel.
-
- This is a useful constraint when building an assemblies; a single
- "same orientation" constraint will fix all three of the imported
- part's rotational degrees of freedom.
-
- Comment
-
- A comment is a single line of text that appears on the drawing.
- When the comment is created, it appears in the center of the
- screen. To move the comment, drag it with the mouse. To change
- the text, double-click it.
-
- The comment has no effect on the geometry; it is only a
- human-readable note.
-
-
-Groups
-
- General
-
- To view a list of groups, go to the home page of the text window.
- 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 on
- its name in the list.
-
- 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.
-
- These groups also have a color, which determines the color of
- the surfaces they produce. To change the color, click on one of
- the swatches in the group's page in the text window.
-
- The group's page in the text window also includes a list of all
- requests, and of all constraints. To identify a constraint or a
- request, hover the mouse over its name; it will appear highlighted
- in the graphics window. To select it, click on the link in the
- text window. This is equivalent to hovering over and clicking
- the actual object in the graphics window.
-
- Sketch in 3d
-
- This creates a new empty group, in which the user may draw lines,
- circles, arcs, and other curves.
-
- 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.
-
- 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.
-
- Sketch in New Workplane
-
- 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:
-
- 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 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).
-
- 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.
-
- The new group's associated workplane is automatically set to be
- the active workplane.
-
- 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.
-
- Step Translating
-
- This group takes geometry in the active group, and copies it
- multiple times along a straight line.
-
- 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.
-
- 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 text window.
-
- 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.
-
- 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.)
-
- 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.
-
- If the active group is a solid (extrude, sweep, lathe), 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.
-
- 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.
-
- Step Rotating
-
- This group takes the geometry in the active group, and copies
- it mutiple times along a circle.
-
- 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.
-
- 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.
-
- The step and repeat options (one side / two sides, with original /
- with copy #1) are the same as for step translating groups.
-
- 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.
-
- 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.
-
- Extrude
-
- 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.)
-
- 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.
-
- 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.
-
- 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.
-
- 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 -> In Workplane).
-
- Lathe
-
- 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.
-
- To create a lathe group, first select a line segment. Then choose
- New Group -> Lathe. The line segment is the axis of revolution.
-
- 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.
-
- Sweep
-
- This group takes a flat sketch, and sweeps it along an arbitrary
- trajectory. The section is taken from the group that is active
- when the sweep group is created. The path is taken from the
- group that precedes the active group.
-
- The section to sweep should be drawn approximately normal
- (perpendicular) to the trajectory. As the section is swept,
- it is maintained normal to the trajectory.
-
- Helical Sweep
-
- This group takes a flat sketch, and sweeps it along a helix. The
- section is taken from the group that is active when the helical
- sweep is created.
-
- To create a helical sweep, first select a line segment and a
- point. Then choose New Group -> Helical Sweep. The line segment
- is the axis of the helix, and the point determines the radius
- of the helix.
-
- To change the parameters of the helix, enter new values in the
- helical sweep's page in the text window. For example, a 1/2"-10
- screw thread has axial pitch 0.100" per turn (since ten turns
- of 0.100" make an inch), and dRadius = 0. A flat coil has axial
- pitch zero, but some dRadius. A sweep with nonzero pitch and
- dRadius produces a conical helix.
-
- Import / Assemble
-
- In SolveSpace, 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, SolveSpace 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.
-
-Analysis
-
- Trace Point
-
- 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:
-
- 
-
- 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.
-
- To start tracing, select a point, and choose Analyze -> Trace
- Point. When the point moves, a cyan trail will be drawn behind it.
-
- To stop tracing, choose Analyze -> 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.
-
- 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.)
-
- 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.
-
- 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 ->
- Step Dimension. Enter the new final value for that dimension,
- and the number of steps; then click "step dimension now".
-
- 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.
-
- 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.
-
- 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.
-
- Measure Volume
-
- 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.
-
- 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.
-
-
-Export
-
- Bitmap Image
-
- This option will export a bitmap image of whatever is displayed
- on-screen. It is equivalent to taking a screenshot. This option
- is useful for producing human-readable output.
-
- Choose File -> Export Image. The file is exported as a PNG,
- which most graphics software can open.
-
- 2d Vector (DXF)
-
- This option will generate a 2d vector file that represents a
- specified plane in the part. Most 2d CAM software, including
- the software that ships with most 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 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 DXF file.
-
- The units of the DXF file are determined by the export scale
- factor, which may be specified in the configuration screen.
-
- The exported DXF contains only line segments; all curves are
- broken down into lines, with the specified chord tolerance.
-
- 3d Mesh (STL)
-
- This option will generate a 3d triangle mesh that represents
- the entire part. Most 3d CAM software, including the software
- for most 3d printers, will accept an STL file.
-
- The mesh from the active group will be exported; this is the
- same mesh that is displayed on screen. The coordinate system
- for the STL file is the same coordinate system in which the part
- is drawn. To use a different coordinate system (e.g., to rotate
- or translate the part), create an assembly with the part in the
- desired position, and then export an STL file of the assembly.
-
- The units of the STL file are determined by the export scale
- factor, which may be specified in the configuration screen.
-
-Configuration
-
- Material Colors
-
- In the text window screen for certain groups (extrude, lathe,
- sweep), a palette of eight colors is displayed. This palette
- allows the user to choose the color of any surfaces generated
- by that group.
-
- These eight colors are specified here, by their components.
- The components go from 0 to 1.0. The color "0, 0, 0" is black,
- and "1, 1, 1" is white. The components are specified in the order
- "red, green, blue".
-
- A change to the palette colors does not change the color of any
- existing surfaces in the sketch, even if the color of an existing
- surface no longer appears in the palette.
-
- Light Directions
-
- The 3d part is displayed with simulated lighting, to produce
- the impression of depth. The directions and intensities of these
- lights may be modified according to user preference.
-
- The lights do not have a position; they have only a direction,
- as if they were coming from very far away. This direction is
- specified in 3 components, "right, top, front". The light with
- direction "1, 0, 0" is coming from the right of the screen.
- The light with direction "-1, 0, 0" is coming from the left of
- the screen. The light with direction "0, 0, 1" is coming from
- in front of the screen.
-
- The intensity must lie between 0 and 1. A light with intensity
- 0 has no effect, and 1 is full brightness.
-
- Two lights are available. If only one is desired, then the second
- may be disabled by setting its intensity to zero. When the part
- is rotated or translated, the lights do not move.
-
- Chord Tolerance, and Max Segments
-
- SolveSpace 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.
-
- 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.
-
- Perspective Factor
-
- To display a 3d part on-screen, it must be projected into 2d. One
- common choice is a parallel projection. In a parallel projection,
- any two lines that are parallel in real life are also parallel
- in the drawing. A parallel projection is also known as an
- axonometric projection. Isometric and orthographic views are
- examples of parallel projections.
-
- Another way to transform the image into 2d is with a perspective
- projection. In a perspective projection, objects closer to the
- "camera" appear larger than objects that are farther away. This
- means that some lines that are parallel in real life will not be
- parallel in the drawing; they will converge at a vanishing point.
-
- 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.
-
- 
-
- 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.)
-
- 
-
- 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, SolveSpace displays a parallel projection. To display
- a perspective projection, set the perspective factor to something
- other than zero. The distance from the "camera" to the model is
- equal to one thousand pixels divided by the perspective factor.
-
- Edge Color
-
- The surfaces of the 3d part are shaded according to the specified
- lighting. Different faces will catch the light at slightly
- different angles, and will therefore appear slightly brighter
- or darker. This permits the viewer to distinguish the boundary
- between the faces.
-
- Depending on the lighting, this may not provided very much
- constrast. To make the edges of the part more visible, it's
- possible to emphasize them with a solid-color line.
-
- If the edge color is specified as "0,0,0", then no emphasized
- edges will be drawn. If any other color is specified, then the
- edges will be drawn in that color. The edge color is specified
- in the same format as for the material color.
-
- Export Scale Factor
-
- Internally, SolveSpace 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.
-
- 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).
-
- Draw Back Face
-
- 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.
-
- 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.
-
-Licensing
-
- As downloaded, SolveSpace does not include a license key. This means
- that it cannot create files with more than six groups. Larger files
- may be opened, but not modified. This light version of SolveSpace
- is intended for evaluation, but non-commercial / personal use is
- also permitted.
-
- The licensed version of SolveSpace can create files with an unlimited
- number of groups.
-
- When a license is purchased, a license file ("solvespace.key")
- will be sent via email. To activate the license, save this file
- somewhere on your computer. In SolveSpace, 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.
-
-
-Bugs
-
- Boolean operations are performed on triangle meshes, and not on
- exact curved surfaces. This often results in poor mesh quality. 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.
-
- This means that the exported STL files do not contain a high
- quality mesh. This is generally not a problem, but could be in
- some applications.
-
- Another consequence is that the program runs slower as the number
- of triangles increases. To obtain a coarser mesh, increase the chord
- tolerance in the configuration screen.
-
- To improve speed and mesh quality, draw the part using fewer Boolean
- operations. For example, a plate with a hole might be modeled
- by extruding the plate, and then cutting the hole with a second
- extrusion. Instead, make a single sketch with both the outline of
- the plate and the hole, and extrude only once.
-
-
-This is the introductory tutorial. We review the basic user interface,
-and draw a simple 2d part. This covers rectangles, symmetry constraints,
-distance/length constraints, and equal length constraints.
-
-We draw a slightly more complex part, by combining multiple extrusions.
-This introduces workplanes and Boolean ops, and several new constraints.
-
-We look at constraints in more detail. This covers inconsistent
-and nonconverging sketches (two common error conditions), projected
-constraints in 3d, reference dimensions, and construction geometry.
-
-We look at step and repeat; this takes entities, and copies them multiple
-times along a line (translating) or the arc of a circle (rotating). The
-details of the step are specified using constraints.
-
-We build an assembly from multiple parts. The positions and orientations
-of the parts are enforced using constraints. We run a computed
-intersection check, to verify that the parts don't interfere.
-
-We draw linkages and other mechanisms, and simulate their operation using
-the constraint solver. The trajectory of certain points on the linkage
-is traced and exported. We also attach a linkage to a solid model,
-and animate the solid model by dragging the linkage.
-
-
diff --git a/doc/rep.txt b/doc/rep.txt
deleted file mode 100644
index 875d4ff..0000000
--- a/doc/rep.txt
+++ /dev/null
@@ -1,59 +0,0 @@
-
-The user enters requests. A request might be a line segment, or a plane,
-or to step and repeat a group of entities, or anything else. Each
-request has a groupid associated with it; a group will contain one or
-more requests. The request will generate entities, and possibly equations.
-
-Special requests would include an include, which gives us a concept of
-hierarchy. An include pulls in all the entities from another SolveSpace
-part, and fixes them up to a rotation and translation; so that introduces
-six free variables. This means that the part is rigidly constrained,
-but that it still must be placed, and that entities within the included
-part are available to constrain against.
-
-An entity is some geometric thing in the sketch. This might be a
-line segment, or a datum point, or something else. Some requests
-correspond to a single entity, in a straightforward way. Other requests
-generate multiple entities, in some relationship (that is constrained
-automatically, through the generated equations) to other parts of the
-sketch. Each entity has a groupid, which is inherited from the request
-that generated it.
-
-One important entity is a pwl. That's a piecewise linear segment. Its
-endpoints are fixed, so it generates no parameters.
-
-The entity is described in terms of paramgroups. A paramgroup corresponds
-to one or more solver parameters, grouped in such a way as to have
-geometric meaning. For example, a point would correspond to three params,
-x, y, and z.
-
-The paramgroups break down in to params. These are the unknowns in the
-solver equations.
-
-The user enters constraints. Each constraint has groupid. The constraints
-generate equations too.
-
-
-
-
-The items that generate unknowns are:
-
- POINT:
-
- three unknowns, (x, y, z)
-
-
-Entities are:
-
- DATUM POINT:
-
- one point
-
- DATUM PLANE:
-
- one point; the plane is through that point, and normal to the
- vector from that point to the origin
-
- LINE SEGMENT:
-
- two endpoints
diff --git a/doc/tutorial.txt b/doc/tutorial.txt
deleted file mode 100644
index f51bd89..0000000
--- a/doc/tutorial.txt
+++ /dev/null
@@ -1,65 +0,0 @@
-
-In mechanical drawing, it's common to use a parallel projection of a
-3d model into a 2d drawing. A parallel projection is also known as an
-axonometric projection; orthographic, isometric, dimetric, and trimetric
-projections are examples of such a projection. In a parallel projection,
-any two lines that are parallel in real life must also appear parallel
-on the drawing.
-
-This differs from a perspective projection. In a perspective projection,
-objects that are 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 on the drawing; they will converge at a
-vanishing point. This may cause confusion.
-
-By default, NTsolver displays a parallel projection of the model. To
-display a perspective projection, choose #LINK(configuration) in the text
-window, and 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.
-
-
-
-The user interface consists of two windows: a large graphics window that
-displays the model being drawn, and a smaller text window, that displays
-information about the model.
-
-After starting a new file, the model is empty except for the three
-coordinate planes. The graphics window's view is aligned so that the XY
-plane is parallel to the plane of your monitor.
-
-NTsolver requires a mouse with a scrollwheel or center button. To pan
-the view to the left or right, center-drag the mouse. To rotate the view
-around the horizontal or vertical axes of the screen, shift-center-drag
-the mouse. To rotate the view around the axis perpendicular to the screen,
-control-center-drag the mouse.
-
-After moving the view, it's possible to orient the view back on to the
-active workplane. Choose #MENU(Sketch -> Draw in Workplane), or press
-#KEY(W). This produces an orthographic projection of the model. When
-drawing lines and curves in a workplane, it's convenient to work with
-the view oriented on to that workplane.
-
-To zoom in, rotate the mouse wheel, or choose #MENU(View -> Zoom In /
-Out). This will not have any visible effect until a model has been
-drawn, though, since the coordinate planes are automatically scaled to
-fit on-screen.
-
-The text window works like a web browser; any underlined text is a link,
-which may be activated by clicking on it. At the top of the text window,
-two rows of links will show and hide different features of the sketch
-(workplanes, normals, points, constraints, shaded, faces, mesh, hidden
-lines).
-
-Below that, the text window displays a list of groups. A group is a set of
-entities, like lines, circles, or planes. In a new file, two groups exist:
-the references, and a drawing group. The references are the coordinate
-planes (XY, YZ, and ZX); they provide the initial geometric entities to
-constrain against. The drawing group is active; if you draw a line, or
-a rectangle, or some other new geometry, then that geometry will appear
-in the active drawing group.
-
-
-
-
-To start, we