bracket.pl

#!/usr/bin/perl

use TEMPL;
TEMPL::Init();

$TEMPL::TITLE = 'SolveSpace - Tutorial - Drawing an Angle Bracket';
$TEMPL::SHOW_VERSION = 1;

TEMPL::OutputWithHeader("TUTORIAL: DRAWING AN ANGLE BRACKET", <<EOT

<p>
    In this tutorial, we will draw the part shown below. This
    is an angle bracket, with a radiused inside corner and a gusset. Both
    legs of the angle, and the gusset, are the same thickness. There are
    two equal-diameter mounting holes placed symmetrically on one of the
    legs.
</p>

<div class="forimg">
    <img src="pics/tut-finished-all-hidden.png">
</div>

<p>
    When we first run SolveSpace, we will begin with an empty
    part. Initially, our view of the part will be oriented onto the XY
    plane; the label for that plane is displayed at the bottom left of
    the screen (#XY, in dark grey). The axes are also indicated by the
    three colored arrows at the bottom left; the X, Y, and Z axes are
    drawn in red, green, and blue respectively.
</p>
<p>
    When we hover the mouse over any entity, constraint, or other
    object in the sketch, that object will appear highlighted in yellow.
    For example, the XY plane, which is drawn as a dashed square, will
    appear highlighted when we hover the mouse over it. The YZ and ZX
    planes initially look like dashed lines, because they are being
    viewed on edge; but they still appear highlighted in yellow when
    we hold the mouse over them. It is similarly possible to highlight
    the X, Y, and Z axes (which are drawn as arrows), or the origin
    (which like all points is drawn as a green square).
</p>

<div class="forimg">
    <img src="pics/tut-planes.png">
</div>

<p>
    To rotate our view of the part, click and drag with the center
    button (or the wheel) of the mouse. To pan, click and drag with
    the right mouse button. To zoom, use the mouse wheel, or choose
    View &rarr; Zoom In or Out.
</p>
<p>
    Initially, we are sketching in the XY plane. After rotating the view
    by center-dragging, we could try to drag the view back to the XY
    plane, but it would be almost impossible to get it exactly correct.
    To return the view to the XY plane (so that our view is parallel
    to the XY plane, and centered at the origin), choose View &rarr;
    Align View to Workplane, or press W, or choose the equivalent button from the
    toolbar. (The toolbar button for "Align View to Workplane" is at the
    bottom right. To learn what a button on the toolbar does, hover the
    mouse over it; a tool tip will be displayed.)
</p>
<p>
    We will construct this part by drawing the 2d cross-section of the
    angle, and extruding it to form the angle. We will then add the
    gusset using a Boolean union, and cut the mounting holes using
    a Boolean difference.
</p>
<p>
    So to start, we must sketch the profile of the angle. This is made
    from line segments, plus one arc (for the radiused inside corner).
    We will start with the line segments; so choose Sketch &rarr; Line
    Segment, or the equivalent button from the toolbar. Then move the
    mouse pointer somewhere close to the vertical axis, but not exactly on
    top of it, so that nothing is highlighted. (By starting a line when
    something is highlighted, we can insert certain types of constraints
    automatically. But we don't want to do that now.)
</p>
<p>
    To start the line, left-click. To end the line, left click again. A
    new line segment will automatically be created, that shares an
    endpoint with the old line segment. As we draw, SolveSpace will warn
    us that the profile is not yet a closed contour.
</p>
<div class="forimg">
    <img src="pics/tut-open-contour.png">
</div>
<p>
    Before left-clicking the last time, place the mouse over the first
    point of the first line that we drew. That point will appear
    highlighted in yellow. When we click, the endpoint of the line
    segment we were drawing will snap to that point, forming a closed
    contour, and we will stop drawing. (It would also be possible to
    stop drawing by pressing Escape, or by right-clicking. But here, we
    wanted to draw until we had a complete closed contour.)
</p>
<div class="forimg">
    <img src="pics/tut-closed-contour.png">
</div>
<p>
    The profile now consists of six line segments, that join at six
    endpoints. We can move any of these endpoints by left-dragging with
    the mouse, and the contour will remain closed. The "not closed
    contour" message has disappeared, and the area inside the contour is
    shaded in very dark blue.
</p>
<p>
    We can now use constraints to specify more about the geometry of this
    section. For example, we should place the bottom left corner of the
    profile at the origin. (Of course, we don't have to. But it will just
    make life easier for us later if we align our part to the
    coordinate system.) To do this, we hover the mouse over that bottom
    left point, so that it appears highlighted in yellow. We then
    left-click; the point now appears highlighted in red. This means that
    the point is selected. (To de-select the point, we could click it
    again, or press Escape, or select Edit &rarr; Unselect All. But we
    don't want to do that now.)
</p>
<p>
    Similarly, we can select the origin by left-clicking it. In the
    Property Browser, we see that two points are selected. As a convenience,
    it tells us their exact coordinates (x, y, z), although we don't care
    about that now.

<div class="forimg">
    <img src="pics/tut-points-selected.png">
</div>

<p>
    We want to put the bottom-left corner of the profile at the origin;
    so that means that we want those two points to be coincident. We can
    achieve this with a constraint. Choose Constrain &rarr; On Point /
    Curve / Plane to constrain point-on-point, or use the equivalent
    button on the toolbar. The origin can't move, so that bottom-left
    corner moves in order to satisfy the constraint.
</p>
<p>
    We should also make the roughly-horizontal leg of the angle exactly
    horizontal. We can do this with a horizontal constraint on those line
    segments. So hover the mouse over the bottom line segment, and left
    click so that the line is selected. The line will be drawn in red,
    and information about the line will be displayed in the Property Browser;
    selection works the same for lines and curves as for points.
</p>
<div class="forimg">
    <img src="pics/tut-line-selected.png">
</div>
<p>
    Now choose Constrain &rarr; Horizontal, or use the equivalent button
    from the toolbar. The line is now horizontal, and a small magenta H
    is drawn to indicate the constraint. The H appears in yellow if we
    hover the mouse over it; that constraint can be selected (and then
    deleted, for example) in the same way as for entities.
</p>
<p>
    Repeat this process for the line just above that one, which should
    also be horizontal, and for the short rightmost line, which should be
    vertical.
</p>
<p>
    The other leg of the angle is slightly more complicated. If this were
    a ninety degree angle, then those lines would be horizontal and
    vertical too; but it's not, so they're not. We do know that the two
    long lines should be parallel to each other. To constrain that, we
    first select those two lines by left-clicking them. They will both
    appear highlighted in red.
</p>
<div class="forimg">
    <img src="pics/tut-lines-selected.png">
</div>
<p>
    We then choose Constrain &rarr; Parallel / Tangent, or use the
    equivalent button in the toolbar. This forces the two lines parallel,
    and the constraint is indicated by the pairs of short magenta lines
    drawn parallel to and near the midpoint of each of the two line
    segments. Of course, all of the previous constraints still hold. If
    we drag one of the points, then the other points will move in such
    a way as to still satisfy all of the constraints.
</p>
<div class="forimg">
    <img src="pics/tut-parallel.png">
</div>
<p>
    Then constrain the short endcap of the roughly-vertical leg of the
    angle to be perpendicular to either of the two parallel lines; it
    doesn't matter which one. (Just select the short line, and one of the
    parallel lines, and choose Constrain &rarr; Perpendicular. The
    constraint is drawn as a magenta perpendicular symbol near the midpoint
    of each of the line segments.)
</p>
<p>
    And constrain the two short endcaps to have equal length, so that
    the two legs of the angle will have equal thickness. (Select the
    two short line segments, and Choose Constrain &rarr; Equal Length /
    Radius / Angle. The constraint is drawn as a single short magenta
    line, perpendicular to each line segment. SolveSpace inferred what
    type of constraint (equal length, equal radius, equal angle, etc.)
    was desired based on what was selected when we chose that menu
    option.)
</p>
<p>
    Finally, we want to radius the inside corner of the profile. We
    could sketch an arc of a circle explicitly, and constrain it to lie
    tangent to the line segments where it joins. That would work, but
    SolveSpace provides a quicker way to get the exact same result.
    Select the inside corner point of the profile, so that it is
    highlighted in red. Then choose Sketch &rarr; Tangent Arc at Point; a tangent
    arc will automatically be created at that point. Drag the endpoints
    or center of the arc to change the radius.
</p>
<div class="forimg">
    <img src="pics/tut-section-done.png">
</div>
<p>
    This completes our section. It's not fully constrained, so if we
    drag some of the points, then they still can move. This means that we
    can still adjust the geometry by dragging points with the mouse, but
    as we drag, all of the constraints that we have specified will be
    respected. It would be possible for us to add constraints until they
    completely described the geometry, so that it was impossible to drag
    anything with the mouse. But it's not necessary to do that, and we
    won't do that now.
</p>
<p>
    Note that if we drag a point beyond certain limits (that depend on
    the constraints that we have specified), the sketch may fail to
    solve, or it may solve to an unexpected solution. In that case, it is
    always possible to go back by choosing Edit &rarr; Undo.
</p>
<p>
    We can take our two-dimensional section, and extrude it to produce a
    three-dimensional solid. To do that, choose New Group &rarr; Extrude,
    or choose the equivalent button from the toolbar. This will create
    our extrusion. To see our extrusion, rotate the view by
    center-dragging with the mouse.
</p>
<div class="forimg">
    <img src="pics/tut-extruded.png">
</div>
<p>
    By default, extrusions are one-sided; so our original sketch is the
    beginning of our extrusion, and the solid is either entirely to the
    right or entirely to the left of that original sketch. We can change
    the extrusion depth by dragging a point on the extruded face.
</p>
<p>
    But in fact, we would rather extrude on both sides, so that our
    original sketch forms the middle of the extrusion instead of its
    start or finish. That way our part will be symmetric about the XY
    plane. It's a good idea to draw parts with symmetry about the
    coordinate axes whenever possible, because it's usually simpler to
    construct the desired constraints when that symmetry exists.
</p>
<p>
    In the Property Browser, SolveSpace has automatically shown information
    about the extrusion that we've just created. (If it didn't then we
    could view that information by choosing the "home" link at the top
    left of the Property Browser. We would then see a list of groups,
    including g003-extrude, the extrusion that we've just created. We
    could click on that name to view the same screen that is shown
    automatically. If the Property Browser is not visible, then choose View
    &rarr; Show Property Browser or press Tab.)
</p>
<p>
    We can see that the extrusion, named g003-extrude, is one-sided.
    To change it to be two-sided, click "two-sided" in the Property Browser.
</p>
<div class="forimg">
    <img src="pics/tut-both-sides.png">
</div>
<p>
    The extrusion now
    appears symmetrically about the XY plane, as desired. If we drag a
    point on one of the end faces of the extrusion, then the other end
    face will move to maintain the symmetry.
</p>
<p>
    We now wish to sketch the gusset. We will need to create a new
    sketch, in a new workplane. We can place the origin of that workplane
    at the midpoint of the inside corner of that angle. That point
    exists, but it is currently not visible, because it lies within the
    solid object that we have just extruded. To make it visible, we must
    show "hidden lines", by clicking that icon at the top far right of the
    Property Browser. This causes all lines and points to be displayed, even
    if they lie within the solid model. (So it's as if the part becomes
    transparent.)
</p>
<div class="forimg">
    <img src="pics/tut-hidden-lines.png">
</div>
<p>
    We have left-clicked to select that point here, so it is highlighted
    in red. We then center-drag the view so that we are looking at the
    extrusion roughly on end, and choose New Group &rarr; Sketch in
    New Workplane.  This creates a new workplane, with origin at the
    selected point, and parallel to the XY plane. (If no other information
    is provided, then SolveSpace snaps to the nearest workplane parallel
    to the coordinate axes; so it was important for us to rotate the view
    so that it was approximately correct before we created the workplane.
    Otherwise, SolveSpace might have snapped to the YZ plane or the (Y,
    -X) plane or some other plane instead.)
</p>
<p>
    When we create the new workplane, the view will be aligned to the
    workplane; so we will see the part rotate so that we are viewing the
    extrusion exactly on end. We could rotate the view out of that
    workplane by center-dragging as before, and then return the view to
    that workplane by choosing View &rarr; Align View to Workplane.
<p>
    In that new workplane, we can draw our gusset. Choose Sketch &rarr;
    Line Segment. Left-click to begin the line, again being careful that
    nothing is highlighted when we click (to stop SolveSpace from
    inserting an automatic constraint that we don't want). As before,
    hover the mouse over the first point that we drew before clicking
    the last time, so that the contour is automatically constrained
    closed. The "not closed contour" warning will disappear, and the
    contour will be filled in very dark blue, as before.
</p>
<div class="forimg">
    <img src="pics/tut-triangle.png">
</div>
<p>
    One point of the triangle should lie exactly on the inside corner of
    the angle. (This is also the origin of our current workplane, although
    that doesn't matter now.) So select a point of the triangle, and select
    the inside corner of the existing extrusion, and choose Constrain
    &rarr; On Point.
</p>
<p>
    The other two points of the triangle should each lie on one of the
    legs of the angle. So select one of the points, and select one of
    those line segments, and choose Constrain &rarr; On Curve. This
    creates a point-on-line constraint, which is drawn as a small magenta
    box around the constrained point. Drag the point; it will move along
    the line, but the constraint will be maintained. Repeat the process
    for the other point.
</p>
<p>
    Finally, constrain the two legs of the gusset to have the same
    length. To do so, select both line segments, and then choose
    Constrain &rarr; Equal. This is the same equal-line-length constraint
    that we used in the first sketch.
<div class="forimg">
    <img src="pics/tut-triangle-constrained.png">
</div>
<p>
    Once the sketch is complete, we can rotate our view (center-drag) to
    verify that we've drawn it in the right place. We can see that the
    sketch is at the center of the part&mdash;in fact, it lies in the
    original XY plane&mdash;and that two of the edges of our gusset lie
    coincident with the faces of the angle. This is probably a good time
    to re-hide the occluded lines, to make the view less confusing. Click the
    button in the far top right of the Property Browser twice more, to cycle
    from "occluded lines are dashed" through "occluded lines are solid" to
    arrive back at "occluded lines are hidden".
</p>
<div class="forimg">
    <img src="pics/tut-triangle-3d.png">
</div>
<p>
    We then extrude that section, by choosing New Group &rarr; Extrude,
    in the same way as before. Once again we want a two-sided extrusion,
    so change that in the Property Browser. We can also change the color
    of the extrusion, by clicking on one of the color swatches. Notice that
    it was very simple to place the gusset in the middle of the angle
    bracket, because we originally drew the angle symmetric about the XY
    plane. If we hadn't, then we could still have drawn the gusset at its
    middle (for example, by placing a datum point and using a midpoint
    constraint), but it would have been more complex.
</p>
<div class="forimg">
    <img src="pics/tut-triangle-extruded.png">
</div>
<p>
    We can change the thickness of the gusset by dragging a point on
    either surface of the gusset. But we want the gusset to have the same
    thickness as the angle itself, so it's better to use a constraint.
    That way, the thicknesses will automatically get forced to be equal.
    We can do that by constraining a line along the thickness of the
    gusset to have equal length to a line along the thickness of the
    angle. Select those lines as usual, by hovering the mouse over them
    and then left-clicking. The selected lines will be displayed in red.
</p>
<p>
    One possible choice of two lines is shown above; of course many
    others exist. After selecting, choose Constrain &rarr; Equal Length.
    This is the same constraint that we used earlier when we were
    sketching our sections to extrude. (There's actually a small
    difference; within the workplane, the constraint worked on 2d length,
    projected into the workplane; but now, it's working on real 3d
    length. We can choose which version we want, by choosing Sketch
    &rarr; In Workplane or &rarr; Anywhere in 3d. By default, SolveSpace
    assumes that we want to sketch and constrain within a workplane when
    we're working with a sketch-in-workplane group, and in 3d when we're
    working with an extrusion. That's what we want here, so we don't need
    to do anything special.)
</p>
<div class="forimg">
    <img src="pics/tut-triangle-thickness.png">
</div>
<p>
    The constraint has now forced the gusset to have the same thickness
    as the angle. Try dragging the various points on the model. For
    example, dragging a point on the original profile of the angle (at
    the midpoint of the extruded angle) will change the
    thickness of the angle. It will also change the thickness of the
    gusset, since the constraint determines the thickness of the gusset
    in terms of the thickness of the angle. If something unexpected
    happens while dragging, then choose Edit &rarr; Undo.
</p>
<p>
    The part is now complete, except for the two mounting holes. We can
    draw those as another extrusion; except this extrusion, instead of
    adding material, should remove material to cut the holes. We must
    again create a new workplane, in which we will draw our section to
    extrude. (Most parts will have this structure of alternating sketches
    and extrusions.)
</p>
<p>
    Before, we created our new workplane in terms of a single point, and
    then we let SolveSpace infer the orientation of the plane from the
    orientation of our view. That worked because our desired orientation
    was parallel to one of the coordinate planes. In this case, our
    desired plane is not parallel to a coordinate plane, because the
    angle bracket is not (necessarily) ninety degrees. So in addition to
    the point for the origin, we specify two line segments; the workplane
    will be defined so that both of the line segments are parallel to
    that plane. So select a point and two (non-parallel) lines on the
    back of the extrusion, for example the point and two lines shown
    below. Then choose New Group &rarr; Sketch in New Workplane.
</p>
<div class="forimg">
    <img src="pics/tut-back-lines.png">
</div>
<p>
    The view is aligned to our new workplane, as usual. This time we want
    circles, so choose Sketch &rarr; Circle. Left-click to define the
    center of the circle, and then left-click again to define its radius.
    (To change the radius later, just left-drag the perimeter of the
    circle. And the center is a point that may be dragged like any other.)
    Repeat the process to draw a second circle.
</p>
<div class="forimg">
    <img src="pics/tut-circles.png">
</div>
<p>
    We want the circles to have the same radius/diameter, and to be
    placed symmetrically about the center of the part. Select each circle
    by hovering the mouse over it (so that it shows up highlighted in
    yellow) and then left-clicking. Then choose Constrain &rarr; Equal
    Radius. (Notice that the same menu item can be used to create many
    different kinds of constraint, depending on what is selected when we
    choose that menu item.)
</p>
<p>
    To place the circles symmetrically, select each circle's center. Then
    choose Constrain &rarr; Symmetric. The symmetry constraint is drawn
    as a pair of magenta arrows, pointing inwards.
</p>
<div class="forimg">
    <img src="pics/tut-circles-constrained.png">
</div>
<p>
    In this case, the points have been placed symmetrically about the
    vertical axis of the workplane (through the workplane's origin).
    Since no axis was specified with the constraint, SolveSpace inferred
    that we wanted either the horizontal or the vertical axis of the
    current workplane. Since the two circles' centers were initially
    drawn more horizontally than vertically, it inferred that we wanted
    the vertical axis. We could also have specified the axis explicitly,
    as a line segment or a plane, but it was not necessary for us to do
    so.
</p>
<p>
    The section is complete, so as usual choose New Group &rarr; Extrude.
    This creates two cylinders, as shown below.
</p>
<div class="forimg">
    <img src="pics/tut-circles-extruded.png">
</div>
<p>
    First, the extrusion is going in the wrong direction. We could fix
    that by dragging the end face of the extrusion to the other side. But
    once again, it's better to specify what we want exactly, using a
    constraint. Select the center of the circle on the extruded face. Then
    select the inside face of that leg of the angle, as shown below.
    Faces can be selected, in the same way that points or lines can be
    selected. Hover the mouse over the face, and it will appear
    highlighted in yellow. Left-click, and it will appear highlighted in
    red.
</p>
<p>
    In order to select both the face and that point, it may be necessary
    to rotate our view of the part. This is not a problem.
</p>
<div class="forimg">
    <img src="pics/tut-circles-pt-on-face.png">
</div>
<p>
    Then choose Constrain &rarr; On Plane. This places the point on the
    plane, which sets the extrude depth and direction as desired.
</p>
<p>
    In the
    Property Browser, modify the extrusion so that it is merged as
    "difference" instead of "union". This means that instead of adding
    material, this extrusion removes material. So the extrusion cuts two
    holes, and we're done.
</p>
<div class="forimg">
    <img src="pics/tut-finished.png">
</div>
<p>
    Try dragging each point on the model, to see which degrees of freedom
    it manipulates. Some points cannot be dragged, because the
    constraints that we have specified completely determine their
    position. But we have not fully constrained the sketch, so most of
    the points can be dragged to change some parameter of the part.
</p>
<p>
    Also, try going back and making some change to earlier sketches in
    the part.  In the Property Browser, choose "home" (from the link at the top
    left of the Property Browser), or press Escape until we see a list like
    the one below.
</p>
<div class="forimg">
    <img src="pics/tut-group-list.png">
</div>
<p>
    Each entry in the list corresponds to a group in the part. The first
    group is the references; that includes things like the XY plane and
    the origin. The references are created automatically, and cannot be
    modified. The first real group is g002-sketch-in-plane; when we
    started drawing, we were drawing in g002. This is a
    sketch-in-workplane group, where that workplane is parallel to the XY
    plane and centered at the origin.
</p>
<p>
    We had then extruded g002 to form g003, an extrusion. We drew the
    gusset section in g004, and extruded it in g005. We drew the mounting
    hole section in g006, and extruded it in g007. SolveSpace maintains a
    history of the features with which we created our part, and allows us
    to modify them. If we modify something in an earlier group, then that
    change will automatically propagate into later groups, according to
    the constraints and other rules that we have specified.
</p>
<p>
    For example, click the radio button in the "active" column for g004. We now see
    the section that we had drawn for the gusset. Choose View &rarr; Align View to
    Workplane to orient the view back on to that workplane, and make some
    change that sketch (by dragging the points, or dimensioning the
    length of one of the lines, or even adding some new geometry). Then
    click the radio button in the "active" column for g007, to see the finished
    part. Whatever changes we made to g004 have propagated through.
</p>
<p>
    The current view of the part is rather cluttered. SolveSpace will
    generate many extra lines and points, because they might be useful to
    constrain against. To hide those, choose "hide all" on the Property
    Browser home screen. We now see only the lines and curves that
    actually form the edges of the solid model.
</p>
<div class="forimg">
    <img src="pics/tut-finished-all-hidden.png">
</div>
<p>
    This solid model can be used in several different ways. We could just
    look at it, or export a screenshot using File &rarr; Export Bitmap.
    Or we could export a hidden-line-removed vector drawing, using File
    &rarr; Export 2d View. We could export a section of the solid by
    selecting a face of the model (to define the section plane), and
    then choosing File &rarr; Export 2d Section.
</p>
<p>
    We also could export the three-dimensional solid model itself, either
    as a triangle mesh or as a STEP file. Most CAM or rapid prototyping
    software expects some type of solid model as input. It's generally
    better to use STEP files when possible, since they represent curves
    and curved surfaces exactly (vs. triangle meshes, which are only an
    approximation).
</p>
<p>
    This tutorial has covered only the basics of SolveSpace. Many other
    features exist, including a wide range of entities and constraints,
    2d and 3d parametric assembly, and various analysis and export
    functionality. See the reference manual for more information, or the
    other tutorials.
</p>
</p>
<p>The part drawn in this tutorial is available for download:</p>
<ul>
    <li><b><a href="dl/bracket.slvs">bracket.slvs</a></b></li>
</ul>

EOT
);