FOREWORD.
If
I’ll try to show what this book is, I’ll be putting myself between a rock and a
hard place, so instead I would rather show what this book is not.
First
and foremost is not a scientific compendium of elaborate formulae, footnotes
and referrals, theoretically discussing the fundamental laws and principles of
solid modeling.
Second,
it is not a step by step check-list taking the reader through all the
intricacies of Solid Modeling. Such a thing is feasible only for a specific
software package at a time, and we don’t want to be particular about any
package.
Third,
is not a compendium of “all things 3d”.
And in general, is not a book
you read in bed at the end of a long day at work.
On the other hand, it will surely
make you sleepy if you read it in bed!
OK, we saw what it isn’t.
Let
see what it is, or rather what is intended to be.
Is
supposed to be a guide into the field of solid modeling for people intending to
learn the ropes just right now as well as people who are already “in”, using it
(the 3d modeling software) but did not have the time to learn the ropes.
We
know that there are a lot of people in both these categories out there.
And
no blame is cast on any of them; we know too well that a lot of people in the
field were forced into using very complex tools (like solid modeling) without
having time to learn the fundamentals. The need to get to speed is always
prevalent in such cases.
From
his own experience, the author knows that a lot of people already using Solid
Modeling Software have gotten there without being asked. Somebody else made the
decision for them.
I
mean, if the “management” decided that Solid Modeling has to be implemented by
the end of the year, you got your share of headaches scrambling to learn it on
the fly. Unless you rather quit and go to a company that still uses drafting
boards.
Learning
on the fly gets you someplace, but is very probable that the basics were never
properly learned. Exactly like in math, if you didn’t grasp too well the
fractions, you’re bound to be lost in calculations when the “calculus” starts,
because you’re missing the fundaments.
This
book comes close to be a “take me by the hand” guide, but for very good reasons
doesn’t go totally there.
The
reasons are that –as we mentioned before- due to the specifics of each
commercial software dealing in this subject matter, it is impossible to get
into a unique step by step routine. Each software dealing with solid modeling
has its own set of tools and commands, each requires more or less steps to
accomplish a simple task like sketching, so, unless the author would have gone
mad and tabulated each step according to each software, like here:
Software Work plane Sketch Feature
XXX already set click to sketch Pick after sketch
YYY chose WP start after choosing feature chose before sketch
ZZZ chose and confirm chose 2d or 3d sketch after
sketch ready
orientation
… …. ….. ….
Besides,
more likely the author would have gotten in trouble with the software producers
for favoring one package against another.
For these reasons, this book
has taken the aspect of a brush-up guide for the fundaments of Computer Aided
Design with emphasis on 3D.
We tried very hard to explain for all levels
of knowledge on what foundation 3D resides, and what are the minimal
prerequisites to get to a good comfort level while working on a model.
To
return to the main thread, we tried here to brush up some forgotten (or never
well known) basic notions about elements of geometry as used in conjunction
with solid modeling: coordinates, position, point, planes, axes, and so on.
These are the fundaments.
They
should be enough to make the reader more comfortable when navigating through a
maze of work planes or when having to create a new one from scratch.
For
instance, if you knew that a plane could be defined by only three points or a
line and a point, you’ll get to create a custom plane in a jiffy, even if it is
skewed and offset like hell.
And
as we mentioned before, we can’t show in this book command by command or mouse
click after mouse click sequences needed to create a solid model. It will be as
large as an encyclopedia, and not universal, not two software have many things
in common.
We
did, however, went through a lot of trouble explaining how to create all the
features used in solid modeling, from sketch to the finished solid.
Here is what the reader will
find in this book:
Chapter one.
(16 illustrations)
a short practical introduction
to the basic geometric notions like:
point;
line;
origin;
position;
ordinates;
vectors;
systems
of coordinates;
planes;
projections;
axes.
Chapter 2.
(16 illustrations)
Another short and practical
brush-up for the following notions:
Work
plane;
Work
axis;
Sketching
tools;
Solidifying
tools;
Open
loop profiles;
Power
of smart dimensioning.
Chapter 3.
(72 illustrations)
Dedicated exclusively to “how
to” create Extrusions, with lots of
examples.
Chapter 4.
(47 illstrations)
Dedicated exclusively to “how
to” create Revolved features, with
lots of examples.
Chapter 5.
(34 illustrations)
Dedicated exclusively to “how
to” create Sweeps, with lots of
examples.
Chapter 6.
(23 illustrations)
Dedicated exclusively to “how
to” create Lofts, with examples.
Chapter 7.
(19 illustrations)
Dedicated exclusively to “how
to” create Shells, with examples.
Chapter 8.
(16 illustrations)
Also dedicated entirely to “how
to” create Helix features.
Chapter 9.
(25 illustrations)
Dedicated entirely
to the creation of Ribs in Solid
Modeling.
Chapter 10.
(35 illustrations)
This chapter will
be shared among lesser features as: Fillet,
Chamfer and Surface Draft.
Chapter 11.
(69 illustrations)
Here we put
everything together and create Assemblies.
Chapter 12.
(15 illustrations)
Here, we go back
from 3 dimensions to two: Drafting
from models.
Chapter 13.
(10 illustrations)
If you’re
superstitious, don’t touch it, it is mainly quizzes.
Chapter 14 (and last, thanks God)!
(7 illustrations)
Deals with
editing: how to edit sketches, features, part browsers.
CHAPTER ONE.
BASICS OF THE BASICS.
I’m
calling this chapter the “Basics of the basics” because in it we will cover the
first elements on which we will build our knowledge; these are elements
essential to the art of three dimensional design and drawing. And even beyond.
Some
will argue that nowadays, the software you will likely use to design in 3d does
not require you to know all these basic elements in detail. And that is true to
a point, but there are times when you have to solve a tricky situation to which
your software does not provide an easy solution. If you find yourself in such a
situation and you don’t know your basics, you will be in pain.
What
I’m conveying here is: it is not strictly necessary for you to know what the
definition of a point or a plane is in order to create a model; with modern
software you just pick your work plane and go. But, if you need to create an
out of ordinary work plane and you don’t know what defines a plane, you’ll wish
you knew the basics, or be left fishing.
On
the other hand, there will always be a lot of people out there craving to know
how to do solid modeling but not having the slightest idea about these
concepts. True, you can open the software and little by little, through trial
and error, you’ll succeed in creating a model, but your knowledge is very
shaky. If you are faced with a problem that involves the knowledge of the
fundamentals, you’re lost, because you never knew them.
In
any event, either you knew the fundamentals or you just want to know them, here
is the opportunity to brush up or to learn something new.
So, the
best place to start is the beginning, as though you never heard any of these
ideas before.
The
elements from which we build our solid modeling knowledge are, in no particular
order, the following geometric entities:
-point
-origin
-position
-ordinate
-vector
-projection
-work axis
-work plane
-sketch
-feature.
About the last entry, FEATURE, there are some fine points to
emphasize:
This word is used in 3D
modeling in three different situations, describing three things very tight
related, such as:
1) Feature
is the tool that allows the designer to transform a sketch into a simple solid
or a part of a more complex one.
For
instance, to obtain an extrusion, you have to use the feature (tool)
“extrusion” in order to obtain an extruded solid. This is also called a
“feature” if is only a part of a solid.
2) Feature
is also (as we just said above) an element of a model, obtained from a sketch
thru one of the features (tools for solidification) available.
3) Feature
is in the third place the name of the operation through any sketch is
transformed into a solid element.
To recap: using a feature
(tool) we obtain a feature (solid
element) through a feature
(operation).
Some
of these elements are used all the time, others are used only now and
then. But one way or another they are
used, and to brush up on them is not going to hurt anybody.
POINT.
The most minute of all, the point is an element of geometry we need to
know in order to be able to define other elements like: direction, distance,
line, center, and plane. One is inclined to say the point is the very base of
geometry.
The
point is defined in The Webster Dictionary as:
“An element in geometry having
only a position, but not size, shape, or extension”.
Let
try to find a few examples of points:
The
intersection of two or more lines creates a point, because it has a position
(at the intersection), but no other attributes.
The
center of a circle is also a point, positioned “at the center”.
The
intersection of three or more orthogonal planes is a point too.
The
beginning and the end of a line are each a point.
Hence, a line can be defined by two points.
And so we already covered the line as well.
ORIGIN.
The
word origin is taken here in the sense of the point of inception, the point
from which we define relations with other points.
The
origin can be situated anywhere in space, the only condition for it to exist is
a location.
The
center of the earth, the origin of spatial computations, has a unique location,
the center of the earth.
The
North Pole also has a definite location.
The
intersection of the Equator and the
No
confusion there, all these points are very precisely located.
Remember:
an origin is the starting point for a system that helps to define or locate
other points in space.
Most
of the time, we use the word ORIGIN to indicate the intersection of the three
work axes (and planes too) at the left-bottom corner of our work sheet, but we
must be aware that this is only a convention and an origin can be situated
wherever we deem it necessary.
THE WORK AXES.
These
are the workhorses in our field, for they determine almost everything:
orientation of the work planes, direction of plus and minus, degrees of
freedom, even the ORIGIN, which is always located at their intersection.
Well,
depends on what we look at first, like the egg or the hen. Some people will
argue that the Origin determines the position of the three axes, which is also
true.
Better
let the Einstein-s of this world decide this one, for us, it works both ways.
And
we must thank whoever decided that only three of such elements are enough to do
our work. One more and everybody would have gone nuts.
By
universal convention, it is established that the three axes of the system are
intersecting perpendicularly on each other at the origin, and extend in both
sides of the origin.
A)
The X axis
goes towards the right (east) for positive values and left (west) for negative
values.
B)
The Y axis,
goes up (North) for positive values, down (South) for negative values
C)
The Z axis
goes away from the plane formed by x and y for positive values and stabs the
x-y plan for negative values.
Here,
a note has to be added:
If
the reader is more comfortable with indicating directions by using the dial of
a watch, then: 12 is North, 3 is East, 6 is South and 9 is West.
Also,
the above arrangement for the three axes is only one of many ways it is
conventionally represented, you may see them turned upside down and inside out,
and it doesn’t matter. This is the plain vanilla flavor.
This
is the most common representation of our basic system of coordinates.
Take
a look at Fig.1.1, and try to visualize and better, memorize, this concept
which in my humble opinion is the bible of 3D. If you don’t assimilate this
foundation block now, you’ll most likely suffer from an ulcer latter.
Fig.1.1 The three work axes.
PLANE.
A
plane, according again to our trusty Webster source, is:
“A flat surface that wholly
contains every straight line joining any two points on it”. Well, it’s like
scratching your left cheek with your right hand, very straightforward, isn’t
it? Anyway, it’s an earful.
Let
tray an easier approach;
A
PLANE is to be considered as a flat surface –like a flat sheet of paper- made
from infinity of lines glued parallel to each other. This is not to say that
the lines must be only parallel to each other, no, they can be intertwined or
interlaced as to create a fabric like surface, but without thickness. Since the
points don’t have any dimension, so do these infinite lines. Hence, the plane
is also
a-dimensional, A PLANE HAS NO THICKNESS, and
no boundaries, goes to infinity in all the directions.
What
are the ways of defining a plane, what makes a plane different from others?
A plane is uniquely defined by
any one of these:
-
3 points;
-
a line and a point;
-a
closed surface.
Let
ponder the first notion that a plane is defined by three points:
Take
a pencil and a small piece of cardboard and keeping the pencil with the point
up, try to make the cardboard stay put on it. If you have a lot of patience,
maybe you’ll find the center of gravity of the cardboard and succeed, but most
of the times you will need at least two other points to hold that cardboard in
position.
Now
take two pencils and try the same trick, the cardboard will tip one way or the
other and fall.
If
you now have three pencils standing tips up and lay the cardboard on all three
of them, the piece of cardboard will rest comfortably on these three points (it
may even thank you). This is why all the chairs and tables and cabinets, etc,
have at least 3 legs, it is the minimum required to obtain a supporting plane.
Now,
if you move just one of the resting points a tiny bit up or down, the plane
readjusts to lay on all three points again and in the process becomes a
different plane, defined by one new point and two old ones. Imagine how many
times you can do this without duplicating a plane? If you can imagine Infinity,
you’re good!
The
second way of defining a plane is by indicating a line and a point.
If we go back at our experiment
with the pencil and cardboard and try to balance the cardboard on the length of
a pencil this time, we’ll find that it is possible but tough. The 3d point is
not truly defined yet.
But if we lay the cardboard on
the pencil held horizontally and sustain one of its edges with a finger or
another pencil, the cardboard is happy again and won’t fall. The horizontal
pencil is our line, while the other is our point. A plane is defined by a line
and a point as I said before.
The
same idea with moving the point up and down applies here too, with the same
magic results; there is infinity of planes that can be created this way.
The
third way and the most obvious is the closed surface, like a circle, square,
rectangle, triangle, etc.
If
we take our tired cardboard and lay it on the mouth of our coffee mug, it will
happily stay there forever if we don’t remove it to drink the coffee.
Why? Because it lays on a
closed surface, the circle defined by the mouth of our mug. We said circle
because, from personal experience we saw that square mouthed mugs are very
rare.
Again,
the three ways to define a plane are: 3 points, a line and one point, and a
closed surface.
A
line and an angle will do the trick too, but is a duplicate of the second
axiom.
And
again, remember: the plane has no thickness, I can stuff a zillion planes in
the space of a thousand of an inch, maybe more if I get very motivated. And I’m
not different from him or you!
And the plane stretches to
infinity in all directions.
Don’t
forget these, please.
THE WORK PLANES.
These
are our workhorses, we use them constantly; as a mater of fact, you cannot
start working on a solid model until you do not select a work plane first.
They
follow the same principles established for planes in general; what make them
work planes is a simple convention, yet another one governing our field of mechanical
engineering, the one that establishes the three planes defining the Cartesian
system:
1) The x-y plane, also called the paper
plane is the plane lying flat on the drafting table and on which the top view
of a part must reside. Or, the surface of the screen on the computer running
your drafting software. This is the plane “you look at”, either because is laid
on the top of your desk, on the computer’s screen or hung on a wall like a map.
Maps
are conventional representations of geographical entities, and they also are
governed by conventions: North will be always on top of a map, south at the
bottom, east to your right and west to your left. Maps are also divided in
little squares of a grid, which facilitates the location of any point on the
map by the number of squares from south to north and west to east.
As
your x-y plane hangs from the wall, or lays flat on the table the origin is
located at the left-bottom corner of the grid.
This
is the universally accepted convention for an x-y work plane, it is the plane
you do your work on, having its origin on the left-bottom corner.
Take
a look at Fig. 1.2. You’ll see that the
XY plane is in fact stretching in all directions to infinity and the origin is
located somewhere arbitrarily in the middle of it. So, then, why say that the
origin of this plane is at the left-bottom corner? Because, in most usual
conditions, the only part of the XY plane we ever use and see is the positive
portion, bordered by the positive Y and positive X axis.
The reality is, as we said
before the plane stretches all the way to infinity in all directions.
Fig.
1.2 the X-Y plane.
2) The Y-Z plane, is defined by the y and z axis, as shown in Fig. 1.3
Fig.
1.3 the Y-Z plane.
3)
The X-Z plane is defined by the x and z axes and Fig. 1.4 depicts this
plane.
Fig.
1.4 the X-Z plane.
When added together in one picture, the three planes will
look like Fig.1.5 below. The picture doesn’t show the entire extent of the
planes for clarity, shows only the most used part of them, but remember, they
stretch all the way to infinity, wherever that is.
Fig.1.5 The 3 work planes.
To
get a clearer picture of this, you can imagine yourself standing in a room,
your feet on the X-Z plane, facing the X-Y plane, and having the Z-Y plane at
your left. Again, this is only one of the ways the 3 planes could be oriented
in relation to the World coordinate system.
Fig.
1.6 A more intuitive way to look at the work
planes.
SYSTEMS OF COORDINATES.
The
most frequently used system of coordinates is the Cartesian system.
The system is named after
Descartes, a renowned French mathematician who was the first to think that a
point in a plane could be defined by:
1)
a set of two
distances (ordinate) from a point called origin,
or
2)
a vector,
having a length from origin and an angle from a base.
To
locate a point in space, it is necessary to add a third ordinate, establishing
the distance from the base plane to the point, or a second angle for the
vector.
Extended
to the real world, for a point in space we need three ordinates, and the vector
must be guided by at least two angles.
In
order to define a point in the universe in relation to, say, the center of the Earth, one needs to know how
many miles high, how many miles to the East and how many miles to the North
that point is located. A system of three dimensions (lengths in our case) and
an origin is strictly necessary to find a spot in the universe. These three
values, together with the origin, are the COORDINATES of a point and are called
a “SYSTEM OF COORDINATES”.
Some
people prefer to call these Longitude, Latitude and Azimuth. These are
functionally the same thing, the only difference is that the origin of this
global system of coordinates is the intersection of the Equator and
To
exemplify, let say that we take the left-front corner on the floor of the room
as the origin and we want to give a precise location for the chair we sit on:,
3 feet to the right and 5 feet opposite the front wall. So, if someone takes a
ruler and measures 3 feet from the corner to the right and 5 feet from the
wall, our chair will be exactly there. Well, not exactly, only its legs will be
there, on the plane created by the floor. And we are still missing vital
information: what point on the chair did we just measure? Which of the four
legs?
Anyway,
having two distances on two axes from an origin, you can find your destination
point with certainty, but it must reside in one plane. The two distances given from the
origin are our two planar ORDINATES, and only two of them are required to find
a point on a plane.
If
the point we want to find is located outside our plane, then a third coordinate
is necessary to find it, the height, thus a complete coordinate system involves
three ordinates, like in the geo-global system.
The same result in locating a point may be
achieved by a vector and an angle or a vector and one ordinate of the tip, for
instance the X ordinate. The value of the vector then can be calculated through
trigonometry if necessary. By tracing a vertical line on the X axis at the
indicated distance, the intersection with a line at the said angle is the tip
of the vector.
In
the following picture, our point is located at “dist. a” on the X axis and at
“dist. b” on Y axis from origin. Only one point can occupy this position,
because as we said before, the intersection of a two lines determines a point.
To determine the position of
the point, one has to walk the “a” distance parallel to the X axis, draw a
perpendicular on it at that point and climb the “b” distance; that will de
enough to determine the position of that particular point.
Fig.
1.7 Coordinates defining a point
in plane.
For
points outside our two-dimensional plane, ( in the real tree dimensional world)
we need a third ordinate, the one that tells at what distance above the
bi-dimensional plane our point hovers.
In
the following picture, we observe that a third dimension has been added to the
two we already know. The third distance, +2z, is the one establishing at what
distance from the “floor” plane the point resides.
The
three distances +7x, +3y and +2z, lead to an uniquely defined point in space,
no other point can claim to have the same exact ordinates, for the same reason
that it resides at the intersection of three lines .
Only one point can exist at the intersection of 3 lines, and
so, where all three coordinates intersect each other, is the destination, the
point we were looking to define.
Fig.
1.8. Defining a point in space
through three ordinates.
THE VECTOR.
A
vector can be assimilated to a line starting from an origin and extending a
certain distance (value or magnitude of the vector) at a certain angle.
The
point at the end of the vector is then uniquely determined.
This is exemplified in Fig.
1.9, where by specifying the length and the angle of the vector the position of
the point at which the vector is aimed is totally and unequivocally defined.
Fig.
1.9
Angle and value of a vector.
The
same result may be achieved by assigning an angle to the vector and one
ordinate of the tip, for instance the X ordinate. The value of the vector then
can be calculated through trigonometry or by tracing a vertical line on the X
axis at the indicated distance; the intersection with a line at the said angle
is the tip of the vector.
See this arrangement below in Fig. 1.10
Fig.
1.10
The ordinate and angle
definition of a point.
Yet
another method of determining a point in plane is through the value of the
vector and ordinate, like in the following picture:
Fig.
1.11
Vector value and ordinate
method.
All
methods for defining the position of a point through vectors shown until now
are only applicable for points lying in one plane, for two-dimensional
applications.
For
points in space, it is necessary to provide more information about where the
point resides, namely the distance from each plane must be given in order to
uniquely determine the position of the point.
This can be achieved by a vector starting from the origin,
having a certain length and by two of the three angles the vector creates with
each axis, like in Fig. 1.12.
Fig.1.12 Vector and angles for points in space.
POSITION.
While
discussing the Vector, we mentioned that the point at the tip of a vector is
“positioned”, by the fact that the vector has a value (distance from origin)
and at least an angle, thus assigning a unique position to that point.
Here
we intend to extend a bit the explanation of the word POSITION, to eliminate
any misunderstanding.
If
you find in your attic an old piece of parchment containing this magic text:
“The treasure is buried 12 paces north from the corner of the house”, don’t go
bananas just yet, you still have to find the treasure.
So, you grab the shovel,
measure 12 paces from the corner of the house due North and dig.
And
dig you do, until after a while, empty handed you start asking yourself: Yeah
right, but how deep? Do I have to dig until I reach
And
all this because the parchment you found gives you only the approximate
position of the treasure. You don’t know at what depth it is, and also which of
the four corners of the house is the origin of the 12 paces. Now, what do you
do, dig at 12 paces north from all 4 corners? No way, so you quit dreaming
about your new car and vacation in
To
establish a true position, you must know either: the origin, a direction
(angle) and a distance, or the origin and two distances. This, of course,
applies when dealing with points situated on the same plane.
For
points situated in space, that is to say points floating outside our two
dimensional default plane, we need to know either: the origin, the distance,
and at least two directions (angles) or all three ordinates of the point.
Because a picture is worth a
thousand words, take a look at Fig. 1.13.
Fig.1.13 Position of a point in space.
The
position of our point is uniquely defined by the three distances,
(x ordinate, y ordinate and z
ordinate), from Origin along the three axes, X,Y and Z.
In
the same time, it could also be defined by a distance (vector) starting from
Origin and inclined at an angle from plane xy (xy plane angle) and a different
angle from plane xz (xz plane angle). A third angle will only confuse things,
it is not required.
The
two methods are never used in the same time, there is no need to do this since
this would just be redundant.
How
can you get to that point?
Well, you can start flying from
origin a distance “Vector”, at an angle “φ” from the ground and an angle
“Ф” from the XY plane, or you can travel the “x ordinate” distance on the
+X axis, then turn 90° to right and travel the “z ordinate” distance and
finally “climb” the “y ordinate” distance to reach the point.
Or you can follow any of the
three projections and at their end, climb the “y ordinate” distance, you will
also get to the point.
The same method of ordinates or
vector applies for a point in the two-dimensional plane, as we have seen it
before when discussing vectors.
PROJECTION
The
projection of an object is its shadow laid directly perpendicular on the plane
of projection. This is the real projection, the geometrical projection. In the
same time, we have one other kind of projection, namely of sketches or geometrical elements of
sketches on planes, as we will see latter. These projections do not follow the basic rule of
projecting that dictates the shape of the projection to be the “shade” of the
projected element. For instance, in the
case of geometry projected on a skewed plane, the shape remains the same. As an
example, shown in Fig.1.13.1 below, the projection of a circle on a skewed
plane remains a circle.
Fig. 1.13.1 Projection of a circle on a skewed plane is another circle!
Returning
to the “real” projection, as seen on Fig. 1.13 further up, the “point” has
projections (named A, B and C) on each of the three planes. They
are situated at the bases of the three perpendicular lines traced from the
point to the three orthogonal planes.
The
“vector” connecting the point with the origin also has projections on each
plane, each projection of the vector connecting the origin with each projection
of the point. They are named xy
projection, xz projection and yz projection.
Unless
a geometrical figure is parallel to a plane, its projection on that plane is
not the real value of the figure. This is the meaning of “real” projection!
As
an example, in the same Fig. 1.13 the value of the XY projection is: (vector *
cosФ), the value of the XZ projection is (vector * cosω) and the ZY
projection is (vector * cosφ), where “vector” is the magnitude (value) of
the vector. The star (*) replaces the “X”, the multiplication sign. This
eliminates confusions with the unknown “x”, used in algebra.
To
make it even more evident, let take a tilted work plane and a line AB laid on
it, having a size=length and being parallel to XY plane, as in Fig. 1.14.
Fig
1.14.
Real value of a projection.
The
only projection of this line of equal value with the line itself resides on the
XY plane, because the work plane, by definition is perpendicular to XY, and
also by definition the line is parallel to the XY plane.
Now,
if we look at any of the two other projections, we see that they are smaller in
value than the vector itself, and a little trigonometry goes a long distance in
determining their real values.
The real value of the
projection of the vector on the XZ plane is:
XZprojection = (length * sin
β)
While the real value of the
projection on the YZ plane is:
YZprojection = (length * cos β).
As an example, if length = 2
and the β angle has a value of 25°, the value of XZprojection will be
(2 * 0.4226) = 0.845
while the value of YZprojection
will be
(2 * 0.906) = 1.812.
And
another point to remember: the shape of a projection is a deformed shape. The
projection of a circle on a tilted plane becomes an ellipse, a square becomes a
rectangle, and an ellipse may look like a circle and so on.
CONVENTIONS.
In
the design and drafting of mechanical parts, we are governed by a bunch of
conventions related to almost all aspects of our work, and we have to brush up
on them.
A)
COORDINATES.
According
to these conventions, there are three coordinate systems:
-The Global Coordinate System
-The World Coordinate System
-The User Coordinate System.
When
the origin is located in the center of the globe, this system is called a
Global Coordinate System.
When
the origin is located on a drawing, and the drawing is the main floor plane of
a factory depicting the layout of all the machines, the system is called a
World Coordinate System.
And
finally, when the origin is the center point of a wheel on one of the machines,
or any particular point in a drawing, the system having that origin point is
declared a User Coordinate system.
A
User Coordinate System may have any point as its origin and may be oriented any
which way the user desires, as long as it could be referred to the World
Coordinate System, WCS, and thus to the Global Coordinate System.
B)
ANGLES.
Another
convention we should be aware of is governing the way angles are measured:
-The
“zero” angle, meaning the base from which all angles are “growing” and measured
is the +X axis, or East.
-The
positive direction for angles is anticlockwise,
so that the +Y axis is situated at +90° or -270° from +X axis, the negative
X axis at ±180°, and negative Y at 270° or -90°. Take a look at Fig. 1.15, and imbed
this deep in your gray matter; it is mortally important.
Fig.
1.15
Convention governing angles.
The
same anticlockwise rule applies for all the planes, the positive branch of the
axes being the base from where the angles open.
Recapitulating,
let see, do we have what it takes to start cooking?
So far we brushed up on the
following definitions:
- point
- position
-origin
-vector
-projection
-work axis
-work plane
- plane
-coordinates
-systems of coordinates
-conventions
Seems to be all for now,
if anything I forgot pops up we’ll take it from there.
The
next chapter discusses the elements of 3 Dimensional design or solid modeling.
The words have the same meaning, only Solid Modeling sounds more sophisticated.
CHAPTER TWO.
ELEMENTS OF SOLID MODELING.
Because all the
companies making software for solid modeling are so competitive and don’t like
to share their secrets, each vendor has created his own set of tools and rules
for the use of their software.
This makes the idea of
writing a book about how to use specific software totally useless for the
public at large, since not two products have the same sets of commands or
tools.
What use would a book
describing solid modeling using “Alibre” have for a user of “Inventor?” These
are just two examples; any pair of commercial software on the market can be
taken as example. Furthermore, it is rare that two different products will name
an element the same name.
So, in no event would we
try here to show the commands or procedures used in certain software for solid
modeling. And if we do, we name that
software. What you’ll find here are the universal principles of 3 D modeling used
in order to create a solid model of a part or assembly.
In this book, you won’t
be taken by the hand and instructed: click on that, drag it there and then
click elsewhere. In this book you’ll learn instead what to do in order to
create models with the tools provided by your software, which is a prerequisite.
The ideas we will be brushing up on will be:
-the work planes
-the x,y,z axes (work axes)
-the sketching tool;
-the “solidifying” tool, a function that creates a solid
from your sketch;
Therefore, let start with the beginning.
THE WORK PLANE.
We discussed these
notions at the beginning, as part of the general conventions governing our
engineering work. Now we will discuss them as part of our “modeling” quest.
Each sketch must reside in a plane, and that plane is
usually called “THE work plane” (WP).
Not only that, but each new sketch you start
needs to reside in a plane. This plane
can be the same plane from a previous sketch, a new work plane, a surface of
the part, an offset plane, etc. Just remember, when you say “sketch,” the very
next thing you think is “plane.”
Sometimes what you need
doesn’t already exist. In this case, you
will have to create a new plane, and you should be prepared to do this a lot,
for you really will use a lot of these “custom” planes.
To create such a plane,
you have the luxury to:
-parallel-offset an
existing plane:
-offset an existing
plane at an angle:
-use points and lines
existent in a previous sketch to create a new one:
-chose an
existing face on the model as your new WP.
For
instance, you can very easy obtain a new plane tangent to two curves, or
tangent to a curve and an edge or a point, or between two lines.
Remember
the definition of a plane:
To exist, a
plane requires these minimal conditions:
-three
points;
-a line and a point;
-a closed curve, a polygon,
a surface, all of these is enough to create a WP.
A few examples of how to
create a custom plane will come in handy, so here we go.
We want to create a new
work plane, inclined at an angle of 35°
from the X axis.
If our software doesn’t
provide a direct way to create this plane, we shouldn’t consider suicide just
yet - we may be able to get around it.
We take our benign XY
plane, and create a parallel offset of it at some distance.
Fig. 2.1
The default (active) plane (blue) and the offset one (brown).
Then we draw a line at
35° on the default plane and
project it on the offset plane.
Fig. 2.2
The line (black) on the blue plane and its projection (blue
on the offset brown plane).
When we have both lines
ready, we “call” the tool that allows the creation of planes and by picking the
two lines, obtain a new plane exactly as we whished, tilted 35° from the X axis.
Now, we are ready to use this custom plane as we needed.
The general picture is like in Fig.2.3 below:
Fig. 2.3
The 35°
inclined work plane is ready for use.
When a work surface is
available, the task of creating a custom WP becomes a little easier. All we have to do is highlight an edge of
that surface and then the surface and indicate an angle for the offset, like
here:
Fig. 2.4
The edge we want
the offset plane to pivot on.
Fig. 2.5
The inclined plane
dialog box.
After highlighting the
surface, and deciding the angle, we see the preview of the new plane.
Fig. 2.6
The new inclined plane thus obtained.
The technique indicated
above belongs to a software package called Inventor, made by Autodesk.
Your package may act differently, so use caution!
At the beginning of this
chapter we said that sometimes you get lucky and your package puts you right on
the default plane, ready to sketch. This doesn’t imply that you are limited to
create only in this WP. On the contrary,
almost every sketch requires a different plane or existing face, so as we said
before, be prepared to change planes a lot more often than socks.
Some of the commercial
software packages take you directly to the default plane of XY, others display
all three of them and wait for you to pick the one you need. Again, how you get
to choose the work plane is your business.
When you pick a work
plane, remember that it dictates the direction in which your extrusion will
“grow”. For example, working on the most common plane, XY, your extrusion will
grow in the direction of the Z axis. This is like if you put the foundation of
your house in the XY plane, the house will grow its walls in the direction of
+Z, while the foundation will grow on Z negative.
Most of the time, for your
first feature you only need a default work plane, so you start on what is
available and build your custom planes from there.
Unless you have a specific need, always start to work on
your “ground” plane, X-Y.
THE
THREE WORK AXES.
As with the planes, the
work axes are also displayed by default by some packages and not by others. And
like with the planes, you can display or hide them, depending on your
intentions.
Again, like the work
planes, depending on what you intentions are, you need to pick the work axis
that suits you the best.
In case you need some
fancy axes, your software will let you create them one way or the other. This is usually accomplished by picking
points on known surfaces.
The main purpose of the
work axes is to show you what is the orientation of your model and also as
standard (default) revolution or sweep axes.
As I mentioned before,
the axes also indicate the direction in which an extrusion “grows.” If you sketch on the XY plane, the extrusion
will “grow” by default following the Z axis; if your sketch lies on the XZ
plane, the growth will follow the path of the Y; and it will grow in the
direction of the X axis for the YZ plane.
You don’t have to watch
the axis to find where the extrusion goes, the extruding tool in each software
package displays the presumptive direction and asks for your approval among
other questions. Remember the way it works so you won’t expect an extrusion on
the X axis if your sketch is not on the correct plane.
As a general rule, try to keep the origin of the three axes
as the center of your first sketch.
THE
WORK CYCLE.
Before
we go any further, we need to determine the “standard” work cycle, from start
to finish. This should be valid for most of the available commercial software
packages.
The first
step is the opening of your software, followed by the choice of “NEW PART”.
Once in the
“new part” environment, one will have to look for the tools of the trade, such
as: sketching, solidifying, and editing tools.
Once these are in place,
the next step is to choose “sketch”, a WP and the drawing tool that you need:
line, circle, polygon, and so on.
Armed with your choice
tool, draw the sketch of the feature you deem to be the main one, or the base
of your model
When the
sketch of the first element of the model is finished, by choosing the desired
“Feature” (extrusion, revolution, helix, loft, sweep, etc.) one gets to create
the initial element (also called feature) of the model. In rare occasions, the
model will be composed from just this one feature, and that means one can save
it and proceed with other chores. In most cases, after this first feature, a
lot more will follow, and a good advice is: save your work after each feature, you never know what lurks inside
your computer that can make it crash and make you lose your valuable work.
Even if the
computer doesn’t crash, is a good feeling to know that you can erase whatever
you goofed off after save, with the knowledge that somewhere in the guts of
your machine you still have the base of your model intact.
As
mentioned before, if our model is a simple one (a washer-like, a ball, a shaft)
that can e obtained from a single sketch and feature, then the model is ready
to be archived under a proper name or better yet, number.
If the
model is a little more complex (as in the vast majority of cases), then after
the first feature you will have to find a new WP, create a new sketch, solidify
it, save and go.
We will
take a very simple example: a flange with 4 bolt holes.
The initial sketch, 2 concentric circles, will create
(through extrusion) the base.
The second sketch, a circle of adequate diameter with 4
equidistant points on it will create (using the operation “HOLE”) the holes for
bolts.
The last operation doesn’t need a sketch. We’re talking
about “Chamfer”, a great way to bevel edges.
Fig. 2.6.1
below, depicts the three phases needed to obtain the flange and the “history”
box at the right of the picture lists the three features: extrusion1, hole1,
chamfer1. Just in case we need to edit one of them.
Fig.
2.6.1 Work cycle: The making of a flange.
Just to
ensure that this message goes through, this is the Work Cycle in a single pill:
-start with “New Part”
-choose “sketch”
-establish a WP
-draw the sketch of the first (main) element of the model
-invoke the adequate “feature” in order to “solidify” the
first element
-as soon as you declare it OK, SAVE!
-proceed to the next element and so on. But, first Christ’s
sake, SAVE each time you achieve something of importance. Better spend a mouse
click now than have a huge headache latter!
THE
SKETCHING TOOL.
When you start building
a model, the first thing you do is chose a work plane and create a sketch of
the first feature (the base) of your model.
So, to begin, reach for the “sketching mode,” or sketching tool. This
move, depending on the package you work with, may take a little longer to
complete.
We have to beat the nail
over the head here, meaning to establish what is what.
A “sketch” is a
collection of geometric elements (lines, circles, arcs, etc.) that establishes
usually the contour of a “feature”; this one, the “feature” could be a single
element of a model, or sometimes could be the model itself. In this case, the
model and feature are the same.
In order to create a
feature, one needs to create first a sketch; the sketch is then transformed
into a feature by one of the methods available (extrusion, revolution, sweeps,
etc.)
A collection of features
then will create the model.
For instance, some
models will require only extrusions, some will require extrusions, revolutions,
lofts, and so on in order to be complete.
No matter what, the
sequence you create a model is: work plane, sketch, feature and so on.
We’re going to repeat
that each package has its own way of starting a model. Some will simply display
the default work plane (XY most times) and will let you sketch right away. Others will ask you to pick a work plane, and
then click “sketch.” Some will even ask
you to pick a feature you intend to create and only after that you get to “sketch.”
Once you’re in sketch “mode” the screen will immediately show a work surface
(which is “on” your chosen work plane), eventually a grid and most likely at
least two work axes, the X and Y. Z is
usually invisible because it is orthogonal to the work plane.
We mentioned that the X
and Y axes would be visible since these are the axes bordering the chosen WP for most of our work, but, again, it
could be any of the three pairs.
And then, somewhere on
your screen, a “sketching menu” will become visible and usable, offering you a
choice of tools such as Line, circle, box, fillet, and so on.
To repeat, the sketching
tool is the first tool you use when creating a model and this process of
creation starts with a sketch on a plane. The sketch can then be transformed
into a solid by one of the available methods: extrusion, revolution, sweep,
loft, and their affiliates.
What is a sketch?
A sketch is the absolute
essential prerequisite in the process of creating a solid object.
For instance, when you
want to create a simple solid like a rectangular prism, you begin with drawing
the shape of the base of the prism, a rectangle. This way you “sketched” the
rectangular shape from which the software will extrude the prism.
Let’s look at a very
simple example: we need to create the model of a rectangular block having a
square base of 2 inches and a height of 3 inches.
Fig.2.7
The “sketch”, the backbone of a feature or a solid.
On our XY plane, starting from the origin, using either the “line” or
“box” sketching tools, we create a square and dimension it as required.
When the sketch is done,
we call up our “extrusion” tool and pick the sketch.
The software will show what it can do with this sketch by
highlighting it and the future feature resulting.
Fig.2.8
Highlighted sketch with the direction of extrusion shown
When we arrive at this
stage (previewed in Fig.2.8), if we agree with the direction of the extrusion,
all that is left to do is click OK, and the block is there. (See also NOTE).
Fig.2.9
Resulting
extrusion
And there it is, (Fig.2.9)
showing the work plane on which we started, and the three axis. Our block is
nicely centered on the Z axis, which will help later if we use it in an
assembly.
When creating a sketch,
it is good to remember to include all the features you can obtain from a single
extrusion, like holes in a flange or in a hollow pipe. And since you have the
ability to fillet and chamfer the solid latter, don’t be to fussy about fillets
and chamfers, consider only bevels or oblique shapes or arcs that represent big
chunks of material.
Generally speaking, the
way you start your sketch should be dictated by the feature you need to create.
The way you create a feature is limited by the available tools: extrusion,
revolution, sweep, loft, hole, shell, and rib, coil and so on.
And now, we’ll take our
sketching tools one by one and talk about them.
The most used sketching
tool should be by far “the line,”
where you pick one point to start and either stretch the line toward an end
point or just click it, the result is a straight line.
By connecting two or
many lines together, one could create very intricate shapes, and furthermore,
by combining lines with arcs, circles, and so on, the possibilities are
unlimited.
As in everything else,
the way each software package deals with lines is different, so it is no use to
make a rule about the use of “line.” You
must obey your software’s rules to play with it.
Some software packages
offer more than a straight line. The user has the luxury to use splines, curves
with nodes, and so on. These are handy when dealing with surfaces or with
objects that require free (artistic) forms.
The next most popular
tool should be “the circle,” used to
create holes or any round geometric elements. For instance, in order to create
a slot-like shape, you draw two circles at the desired distance, and then unite
them by two tangent lines. By trimming the parts of circle that are not
necessary you get the shape of your slot.
Oh, sure, there is some
software that let you start with a straight line and then curve it and
straighten it up again, but in case you don’t have it, you can use the above
method, the result will be the same.
Next in popularity
(based on usage) should be “the box.” This gives you the ability to create a square
or rectangle with only two clicks of the mouse instead of drawing four lines.
Next, the “arc” with all its options: three points,
start, end, center, etc. is also useful when creating complex shapes.
Again, some packages
will add the “hex” shape, some the triangle, depends on the package,
but these are immaterial. The hex tool is helpful for the creation of a screw’s
head.
Then we have the usual
array of helping tools like: offset,
that allows you to offset a profile at any distance from an existing one, thus
saving you the time of doing it over and over. There are also fillet, move, rotate, trim, erase, array, mirror, copy and lots of other
goodies that will prove invaluable to your work.
The number of little
tools that are available to you is very important. You don’t want a package that doesn’t offer
the “arc” for instance, but the most important tool when you create a sketch is
your own mind.
You ought to make
instant decisions about your work flow, your strategies on building the model
and the kind of sketch you ought to create, and use these decisions to choose
your tools.
So before you touch any
of the sketching tools, think twice about which work plane will be the best
suited for your needs, what feature will be the first (the base) to build on,
what will be the easiest way to create that feature (extrusion, sweep, loft,
revolved, etc.). Find a way to center or
align the base sketch to the origin and only then begin your sketching.
This way of starting a
sketch will give you a lot less headaches and/or ulcers in your career.
One of the finest points
of solid modeling software is the wonderful ability to sketch first and
dimension later. Gone are the days when you were measuring each line, tracing
points at “precise” distances and wasting time and gray matter galore.
With the 3D software of
today, we create a rough sketch and after that, we dimension it. The software
pulls each geometric element to its right place, at the correct dimension.
Here is an example of a
rough sketch:
Fig.2.10
An initial sketch, bearing some resemblance
to what is needed.
As soon as we call up
our dimensioning tool, we find out that the dimensions are out of whack.
Fig.2.11
Actual dimensions of the sketch.
They aren’t exactly what we wanted.
Fig.2.12
The sketch, brought
to the correct shape and size by the power of “dimension” tool.
Just by inputting the
right dimensions and adding the missing ones, courtesy of our software the
sketch looks now like a million bucks:
A good practice while
sketching is the use of “Constraints”.
Each software has a set of these, and they come in handy
when you need to:
-convince circles to be concentric;
- lines
to be parallel or perpendicular, vertical or horizontal;
- two
entities to be symmetric to a third;
-convince a line to be tangent to a curve;
-
something to be coincident to something else;
-
something to be collinear to something else;
-
something to be equal to something else;
-
something to stay putt, ground it or fixate it.
All these implements are
a big help while sketching, take a quick glance at how easy it is to convince
two lines to become tangent to two circles:
Fig.2.13
Lines intersecting circles before calling the “tangent”
constraint.
As
soon as the “tangent” constraint is put to work, the shape of the sketch
changes like magic and the rebel lines become instantly tangent.
Fig.2.14
Same lines, “very
tangent” after the
constraint was applied.
Among the multitude of helping tool
at sketch level, the “Trim” or “Scissors” one is very valuable when we need to
trim unwanted lines as is the case above, where after the lines became tangent
to the circles, the inner arcs of the circles are not necessary anymore. So, we
use the trimming tool, (whatever it is called) to clean our act as seen below:
Fig.2.15
The trimming tool at work.
As a reminder, dimension
and ground any entities you don’t want moved before you apply any constraint.
As a conclusion to our discussion
about sketch, remember: a sketch is a collection of geometrical objects - the
sketch geometry - that includes lines, points, rectangles, splines, fillets,
arcs, and curves like circles and ellipses. The sole purpose of the sketch is
to create the base for a “feature” that we will use to create a “solid”
object. The solid object will not
necessary be our “solid model” (that may take a lot more features to
accomplish), but we can go from a sketch to a solid nevertheless. In our
preceding example, from the sketch of a square we obtained a solid block of
material. This could be in itself our final objective or could be part of a
more complex model.
There is no need to
continue this discussion about sketching, unless we decide to show more
examples of sketches, and that would become a little boring.
Now, admitting that we know all about sketching, we ought to
look for ways to “solidify” those sketches.
WAYS TO “SOLIDIFY” A SKETCH.
For what we are
concerned, a “solid” is composed from at least one “feature”, and we have to
try to differentiate between features: feature
as tool and feature as part of the solid object.
Every software package
is different (you’ll be hearing this a lot in this book), even in the way they
call things, but there seems to be a consensus about calling a feature a
feature. And there is the confusion, too.
A feature, according
again to Webster Dictionary is “The make, shape form or appearance of a person
or a thing”
The way it is understood
and used in many packages is both THE TOOL THAT CREATES a shape or form and THE
RESULT of that action.
So, it’s like this: we
use the extrusion (as a feature) to create an extrusion (as a feature).
For these reasons, whenever we could, we will differentiate
between feature as the tool to create
a solid and the result, which is a solid
part of the integer model. So a tool will create a solid, but not the
model. It may take more solids, one on top of another to make a model.
The process of making a
solid goes like this:
-get hold of the best suited work plane for the base feature
and pick it for the first sketch;
-open your sketch tool and use whatever turns you on to draw
a rough sketch of the base solid;
-before you do any dimensioning, make sure that the main
elements are grounded, so they won’t move;
-dimension and constrain you sketch so it will look like
what you wanted;
-use one of the available “features” to create your first
chunk of solid;
-use faces of this first creation to sketch the next
feature, or use work planes derived from
these, or default work planes for the next sketch;
The most used methods
(some time called “features”) we use in our work to transform a sketch into
something solid and “3 dimensional” are:
-extrusion,
-revolution,
-sweep,
-loft,
- helix,
-shell
all of the above either add or to cut material (boss or
hole);
and
-edge
chamfer
-fillet
-hole
that allow only to subtract (remove) material.
There are a few other
features like: face draft, ribs and webs that are present in some packages
and absent in others. These are mostly “add material” type and we will discuss
some of them at the end of this chapter.
Conclusion: sketches are meant to be used as a base
for features. In turn, features create chunks of solids,
which in turn, added, make a model.
And since repetition
makes perfection, first you draw a sketch on a work plane or on a surface (if
is available) and then, using a feature you create something “solid”, either a
part of a model or the model itself (depending on its complexity). Many times
you go through a lot of features in order to finish a model (or part).
A sketch good for
extrusion will be good for all other features, as long as it is a closed loop
and resides in the right plane or surface.
The next chapters will take each of the above features and discuss them at length.
CHAPTER THREE
THE EXTRUSION.
The simplest way to
obtain a solid (feature) from a sketch and the most used is by far the
extrusion.
The meaning of the word
“extrusion”, according again to The Webster Dictionary is:
“to force material (metal, plastic, etc.) through a die or a
small hole to give it a certain shape, or “to protrude”.
In our case, the word
“protrusion” is the most adequate, since most of the time this is what we
create through extrusion, protrusions. We said “most of the time”, because
there are times when we need to create “voids”, to cut material from a solid,
to create “negative protrusions”. The word “protrusion” should be taken with
care, because, as we said, sometimes it means “void”, because the extrusion
works two ways, adding or subtracting material.
Knowing that a picture
is worth a thousand words, let’s take a very simple example of extrusion.
First, we sketch on the
XY plane a hexagon, and offset the shape with a small value like here in Fig.
3.1, to create a tubular hexagonal extrusion.
Fig. 3.1
Sketch of a hexagon, with an offset to create a wall.
Next step, we click on
the “extrusion” tool and highlight the sketch just created, choose the
“bidirectional” extrusion and “add material”, no draft. The result is a tubular
hex shape as seen below with the length we asked for, in this case 1.5 in,
equally spread in both sides of the Work Plane.
Fig. 3.2
We have extrusion!
Before we go any further
with examples of extrusions, we need to take a look at the many ways an object
or a feature can be achieved, not only by extrusion, but in general by any of
the available features of solid modeling.
In the next discussion
we will show that an identical rectangular prism can be crafted in at least 3
different ways, using the only method we “know” yet, the extrusion.
Let
start with the obvious: on work plane XY, sketch a box, dimension it to be 2 by
2, extrude it 3 on +Z and is done once (All dimensions are inches or whatever).
Fig. 3.3
First of three extrusions to create a similar object.
Now,
pick the XZ plane as work plane, new sketch, draw a rectangle 2 by 3 and
extrude it 2 towards +Y. Done twice, we have a 2 by 2 by 3 inches prism.
Fig.3.4
Second way to create the same object.
Last, pick the XZ plane,
sketch another rectangle 2 by 3 and extrude it 2 in both directions of Y, just
for fun. Done #3. We also have a 2 by 2 by 3 thing.
Fig.3.5
Third
way to achieve the same.
In Fig. 3.6 we gathered
all three contraptions together to create a visual icon of what is all about.
We created three
identical prisms, by extruding a sketch (not always the same) from three
different work planes.
It should be recognized
here that, although you could use the same identical sketch in
all three cases, at first look the prism will show to be
different. In any case, it will be differently oriented. We wanted to convey
the idea of “identical object and position, as in fig 3.6, thus having to
create sketches different from case to case.
If you look at Fig. 3.6,
you will recognize the three work planes and three work axes, although not
exactly in the default position.
And also you’ll notice
that the origin resides at one corner of the first extrusion, which is good
practice. Even better, the origin should have been the center of the sketch, as
we show in figs. 3.3, 3.4 and 3.5.
The drawing has been
rotated to provide a better view, so it doesn’t look like the familiar default.
This rotation tool is
another huge help and from what it was a few years ago is a piece of cake to
twist and turn your model nowadays.
Fig. 3.6
Three ways to
create the same thing.
The “solids” created
this way are identical, the only difference between them being the fact that
they reside on different planes. And
another thing, very important: all three
of them constitute one solid model made
out of three features! Any attempt to separate them (other than deleting
the respective feature) will fail, because as we said, this is a solid made
from three identical elements situated in three different planes.
The real meaning of the
above example is to make the reader use his/her mind and become inventive when
it comes to creating a solid, there are a lot of ways to do the same thing.
Let’s take another
little example, by creating the model of a dice, the kind used in the game of
backgammon or other athletic performances like “crap”.
We will do it from
scratch starting with:
-the creation of a sketch on our default XY plane,
-extrusion of a square block by “adding” material,
-picking a new work plane on the surface of the just created
dice,
-creating a sketch for the 4 spots (the number 4),
-extruding the 4 spots by subtracting material,
-picking another surface, for the 2 spots,
-creating a sketch for the 2 spots,
-extruding the 2 spots by cutting in the material.
And we can go like this until we finish all 6 faces of the
dice.
We will stop here though, the rest is absolutely the same
over and over again, we would not learn anything we don’t know already.
Step 1:
The very first move, create a sketch of a 0.5 inches square on the XY plane.
Fig. 3.7
The sketch of the dice and preview of the extrusion.
Step 2:
Extrude in direction of +Z at a height of 0.5, to obtain a little cube like the
one below.
Fig. 3.8
First extrusion of the dice.
Step 3:
Create a new sketch whit 4 circles equally distant from the center, using a
surface of the dice as the new work plane
Fig.3.9
Sketch for the 4 dots.
Step 4:
Apply “extrusion with removal of material” to “cut” the four little dots
Fig.3.10
Second extrusion, we have “drilled” four dots.
Step 5:
Draw two circles equidistant from the center of the cube, on the face of the
dice perpendicular to the front.
Fig.3.11
New sketch, for the
two dots.
Step 6:
Extrude the 2 new dots, and by now our dice should proudly display a 4 and a 2,
exactly as we see in the picture.
Fig.3.12
Third extrusion, we have our two dots.
Doesn’t make any sense
to continue playing with this dice, the rest is repetitive.
A note: Instead of
sketching circles and taking the pain to dimension them, we could have used the
“Hole” feature. It requires only the position of the center of the hole, the
diameter and depth are set in the feature at extrusion time. Since is a feature
on itself, we’ll talk about it when the time is ripe.
Extrusion, example 3.
Let’s take another
example of extrusion: a hollow box, some sort of a housing, having a hole
through the top and 4 bolt holes at the 4 corners. The far side is hollow, as
you can see from the second picture where the object was rotated to show the
hollow.
The exercise is to make
the reader think a strategy through which this object could be created with the
least amount of work; we all know that work is not paid as it should, so why
break a sweat when you can do it simple and elegant. As we saw before, there
are at least three ways to extrude a rectangular shape like this.
Since our object has
some rounded corners it is preferable to create them from the start, by
sketching them for the first extrusion.
Sure, the big hole on
the top could be added to the first sketch (thus saving same latter work), but
then the opportunity to demonstrate how to create a hole would have been
missed.
Fig. 3.13
The box we want to “recreate”
This is the task: create
the box shown above. How?
We start with a simple
“boss” extrusion to create the body and the 4 holes, since the holes have the
same height as the body.
The
sketch defines the contour of the box with corners rounded and the 4 bolt holes
as in the following picture
Fig.3.14
Sketch of the first extrusion of the box.
Next step, extrusion of
the box.
To do that, we highlight
our sketch, choose a “height” and the software does the rest.
Fig.3.15
The feature (extrusion) of the box is done.
And here it is, extruded
and with the 4 holes already through it.
Next, we need to create
the void inside the box, so we choose the bottom of the box as WP and draw our
sketch there as below in fig. 3.16:
Fig.3.16
Sketch for the “void” on the back of the box.
Now, by extruding this
sketch with removal of material (cut boss in some software, subtract material
in others), we will get the hollow in the box:
Fig.3.17
The box now has a hollowed out bottom.
Not bad, so far we got
almost every feature except for the big hole and its rim
We’ll
create a new sketch on the top surface to depict the rim:
Fig.3.18
Sketch on the top face for the next feature, the rim.
The
extrusion, on which we added a “draft” of 10°,
will look like below:
Fig.3.19
After another
extrusion, the rim on top is added to the box.
And now, for the last
feature, we have to sketch the big hole on the top of the box.
We pick the top surface as work plane and draw a circle of
appropriate diameter, like so:
Fig.3.20
Last sketch, a circle
for a future hole.
And we again invoke a
“cut extrusion” to remove the material inside the circle.
The reason of all this
trouble, as we explained, is to familiarize the reader with the notion of
“drilling” holes through extrusions with removal of material.
As we said before, this
is not the only method to create holes in a solid, there is the “hole” tool
that will achieve the same result by just indicating a point for the center and
choosing the shape and size for the hole.
We
didn’t use this one either, for the same reasons, but will revue it when it’s
time will come.
Fig. 3.21
Our box is
finished.
And there it is our box, ready to fly (or whatever).
Extrusion, example 4.
Yet another way to use
the extrusion tool as a cutting tool is to carve or shape solids in order to
obtain for instance flat faces on a cylindrical object.
Assume “The Boss” wants
us to create a part like this one:
Fig.3.22
This is the part we
want to recreate, using only “extrusion”.
What will be the best
way to make such a thing?
First, the way
it shouldn’t be done.
We can go crazy and
start with the extrusion of a disk like below:
Fig.3.23
First extrusion
of a bad idea.
Then create a
sketch on one end and extrude two protrusions like these:
Fig.3.24
Second extrusion of a
bad idea.
and finally, add on the other side the last extrusion:
Fig.3.25
The part looks OK,
but we spent too much energy on it.
A better way to do the
same thing would be to extrude a cylinder, then
sketch a rectangle on one of the end surfaces and cut-extrude it.
Fig.3.26.
Sketch the shape
of the void on the end of cylinder.
You see it here
highlighted and previewed.
Approving the preview creates
the first cut on the cylinder.
Fig. 3.27
The cylinder with the first cut.
Then, on the opposite
end, sketch another rectangle, dimension it and extrude with “cut” to carve
another piece of the cylinder like here:
Fig.3.28
Sketch for the last cut on
this part.
Fig.3.29
The final result is
good, but not the best.
And
now, we will show you yet another way to do the same thing, but cheaper.
We
take a cylinder and on a plane through the center of it create the two cutting
sketches:
Fig.3.30
Best way of doing it.
We create the two
cutting sketches on the median WP, at both ends of the cylinder.
Then we highlight both
sketches and request a “cut” in both directions:
Fig. 3.31
Highlighted sketches
and preview of the extrusion.
Green represents the
sketches, red the future extrusion.
Fig. 3.32
The part with two cuts, obtained
from one extrusion.
Now our part is ready
from only two sketches and two extrusions, one to create the base and one to
cut the voids in it.
Extrusion,
example 5.
Here is another way one
can flatten parts of a cylindrical object:
(The discussion is based only on extrusions, since we don’t
yet know other forms of “expression”).
First, we sketch a
circle and extrude it as long as we want. The result is a cylinder, as seen
below:
Fig.3.33
Extruded cylinder,
ready to be carved.
Next, on the end surface of the shaft, we create a sketch,
two boxes at a distance of .38 from each other and centered about the axis of
the shaft. The boxes don’t need any other dimension, as you see here:
Fig.3.34
Sketch for the first
two “flats” at one end of cylinder.
With our “removing
material extrusion”, we highlight both sketches and indicate a depth of about
1.5 inches and a direction “into the plane”, and the software will carve two
nice flat faces off of your shaft:
Fig. 3.35
The freshly cut flats.
Taking this idea a
little further, what if we needed a flat surface terminated by a round edge at
the other end of the shaft? You know, the kind of surface obtained by an end
mill cutting on a cylindrical object?
Draw a sketch
representing the shape you want, on the proper work plane, like here:
Fig.3.36
Sketch for rounded end flat.
Since the sketch is on
the WP (work plane) passing thru the center of the shaft, extrude it in both
directions and choose “remove material”.
You must obtain a beauty
like the one at the right end in this picture:
Fig.3.37
Rounded edge flat at
the other end.
Yes, but what if now we
want to add a bevel at this end of the shaft, opposite from the flat?
OK, this shouldn’t be
any problem, let sketch what we want, on the plane passing through the center
(whenever possible):
Fig.3.38
Sketch for the bevel,
on the center WP.
We
are again ready to use the “extrude with
cut” tool, and again we must use the bidirectional option, because we did
the sketch on a median WP.
The final result is this:
Fig.3.39
One bevel
extruded!
Our bevel is quite
visible, makes you believe you’re looking at the mouth piece of a clarinet. Is
only a resemblance, nobody ever intended to design a musical instrument here.
Finally, since we went
through almost all the aspects of extrusion and are about to become experts in
it, I would like to share with you one or two more things one can do by using
the right tool with the right set of options.
For instance, by using
the sketch of a simple rectangle and extruding it with a stiff draft, one can
obtain a beveled plaque on which, by sketching a few letters and cut-extruding
them also with a stiff draft, a nice name-plate can be obtained,
For this demo, I chose
the word “3DIM4U”, mainly because is the name of my web site and my own name is
a lot longer and would have taken a lot more sketching than this.
And since my software allowed me to choose a
material, I picked-up chrome, because shines brighter than other materials.
Fig. 3.40
A nice nameplate obtained through cut extrusion with a lot
of draft.
The second demo, is the
letter M, obtained (according to my software list of materials) from pure gold
by boss-extruding the contour of the “M”, also with a lot of draft (30°) which gives it a nice look.
Fig.3.41
A nice gold monogram
obtained by boss-extruding an M shaped sketch wit a 30°
draft. Try your own!
Extrusion example 6.
And now, ladies and
gentlemen, we present the crusher, the real McCoy, the genuine extrusion
article, a part you must duplicate in its totality, using similar shapes and
approximate dimensions. For the real dimensions, check the “DRAFTING” chapter.
Fig.3.42
A nice part to be
recreated using only “EXTRUSION”.
Step one: we start with the
heaviest chunk, the extrusion of the body:
Fig.3.43
Step one: first
sketch and feature.
The sketch is the blue line, the extrusion is the golden
solid.
Please note that no
dimension whatsoever is visible, but this is only for clarity.
The reader must believe
that the entire sketch is properly dimensioned, as it should be for precise
modeling.
Step two: two circles on the top
surface, to create two bearing nests.
Fig.3.44
Sketch and extrusion number two.
Again, the blue is the
sketch, the gold is the solid. We show both the sketch and the result in one
shot.
Step three: on the opposite
surface, project the two circles for two more bearing nests:
Fig.3.45
Bearing
nests on the “back” surface.
Same here, we show the
intention and the result in one shot.
Step four: on the left side
bevel, sketch a circle for a pivot hole and chop off some material.
Fig.3.46
The pivot hole on the
left side bevel
We hope you did it the
right way, first by picking the bevel’s face as WP, then sketching a circle
with the hole’s dimension and extruding it with removal of material.
Step five: choose the right side bevel as WP and sketch
a circle for a second pivot hole, on the opposite bevel. Chop another hole.
Fig.3.47
The pivot hole on the right side bevel
Step six: create a new sketch on
the top surface for a new protrusion.
Fig.3.48
A new protrusion sprang on the top surface.
Step seven: this is tricky folks,
you have to create a work plane tangent to the two rounded corners of the last
protrusion created and on this tilted plane to create a sketch (a circle) for
the extrusion of a hole dug in the meat of the curved portion of the last boss.
Maybe you can do it by drawing
a construction line tangent to the two fillets and from then create the plane,
maybe you can offset a centerline plane to the correct angle, depends on the
power of your software. All we can say is: do it!
In Fig.3.49 below, the plane has a brownish shade while the
sketch is blue, as usual.
Fig.3.49
Plane tangent to two
rounded corners and the hole extruded.
Step eight. Same hairdo, different
Janet: do the same on the opposite side of the boss.
Fig.3.50
Sketch and hole on
the other side of the boss.
This time both the work
plane and the sketch are bluish, while the preceding WP is still brown. Just
don’t ask why, will you?
Step nine: time to cut a deep
rectangular hole through the whole thing, by sketching on the topmost surface
(or the back, for crying out loud) and using “cut extrusion”.
Fig.3.51
The deep, “thru” extrusion with removal of material.
Step 10:
Creation of two circular grooves of
triangular profile around the top bearing nests.
Fig.3.52
Using extrusion, we created two grooves having a triangular profile.
We start with two
circles each around the nests, and then extrude about 0.2 deep, with removal of
material and a draft of -45°
to obtain the triangular shape of the groove as seen in the next picture:
Fig.3.53
Detail showing the triangular profile of the groove we did
as the previous feature.
Step eleven: with a sketch on the
frontal surface and a cut extrusion, we obtain this guide slot in our solid. It
could be done also by sketching on the initial surface of the solid and
cut-extruding “on reverse”.
Fig.3.54
The slot cut
through the boss.
Step twelve (and last):
creation of a conical bearing surface on the “top” of the model.
Fig.3.55
A conical extrusion?
Why not!
We did it by using a
cut-extrusion with a stiff draft again, from an initial circle sketched on the
appropriate surface.
By working with this
model, we learned a few new tricks, like the use of draft to create conical
surfaces, and the use of custom work planes.
This last one, the
custom work plane is going to be an almost every day occurrence in your life as
a solid modeler, together with the omnipresent extrusion.
Extrusion,
example 7.
Now is time for us to
talk a bit about extrusion with an open profile.
If you ever try to
extrude a profile that is not a closed loop (like an enclosed area), you don’t
get an error message, instead you obtain only a surface, not a solid. Is like
instead of a body, you get only the skin!
Let’s take a look at
what happens when you extrude a simple profile like this in Fig. 3.56.
Fig.3.56
A simple curve, not a closed
profile.
When you extrude it, the
result is this: a surface, not a solid
Fig.3.57
Surface obtained after
the extrusion of an open profile.
Just
for kicks, let see what happens when the profile is closed by a simple line.
Fig.3.58
Closing the profile by adding a line at the base of sketch.
By adding the line at the base of the
profile, from an open loop the sketch becomes a closed one, describing a closed
profile that can be made into a solid by the extrusion operation.
Thus, an extrusion of this closed loop
profile will result in a solid object,
as it should:
Fig. 3.59
Solid extruded from a closed profile.
Extrusion, example 8.
We will go over just another example of a part made using only
extrusions, this one with plenty of custom planes.
This is what we want to create:
Fig.3.60
A contraption with two tilted wings and some cylindrical slots on one
wing, some triangular shaped ones on the other wing.
We must start with the easiest sketch, the “flat” body with the 3
holes and the slot through the center.
Here is the sketch, complete with all the holes and the slot, so we will
save some extruding time and effort: the picture shows also the extrusion.
Fig. 3.61
The sketch and
extrusion of the first feature, the body.
Now, we want to create a work plane which must be tilted at the angle
of the first wing, let say 38°.
For this we create an angle-offset plane from an existing surface like
in the next figure, Fig.3.62
Fig. 3.62
An inclined work
plane has been created using an existing surface on the model.
Next step will be
the sketching of the profile for the wing on the newly created plane and the
extrusion to an appropriate length. Will see this next, in Fig. 3.62a below.
Fig. 3.62a
Sketch (red) for
the next feature.
For visibility,
the previous feature has been reduced to a wire frame; the tilted plane (brown)
and the new sketch (red) are visible now.
Fig. 3.63
The tilted wing
attached to our initial body.
The
sketch that created this wing is a simple rectangle on the custom WP we just
created.
In the next move, we will create a similarly tilted work plane on the
other side of the body.
Fig.
3.64
New tilted work plane on the opposite side of
the body.
Next, the new extrusion should take place to complete the new wing.
Fig.3.65
The second extruded wing in place.
To create the cylindrical grooves in one of the two wings, we pick as
work plane the end surface of the wing and sketch the 5 circles that will cut
into the wing to create the semicircular grooves.
Fig.3.66
Sketch for cutting the semicircular grooves.
Next, using extrusion with removal of material and the option “through
all”, we obtain the five semicircular grooves like below:
Fig.
3.67 The five cylindrical
cuts through one wing.
A note is required here: we could have made only one cut and used
“pattern” for the rest, but we don’t yet know that!
What follows must be the creation of a sketch that will allow the
removal of material that will carve the triangular shaped grooves.
Fig. 3.68
The sketch that
will create the triangular cuts. The preview of the action is also visible.
The above note about patterns applies here too!
Last step, approving the preview to get the cuts in the wing, we got
what we were looking for, four triangular shaped grooves.
Fig.3.69
Final aspect of our part.
Before we end our discussion about extrusion, I would like to return to the above example
and try a different approach for the creation of the wings.
We will take only one of the wings, the
second being just a copy of the procedure.
Starting with a view from the South of
the part, we will create an offset plane that will reside at the precise
beginning of the wing, at the end of the fillet.
Fig.3.71 Sketch and preview of the new way of
obtaining the wing.
As it can be seen in the picture, we
have the parallel-offset WP (brown) on which we sketched the profile of the
wing (green). Also visible are the dimensions and the preview of the extrusion.
After the extrusion, we get the same
wing as previously, just waiting for someone to chop the grooves. See the
following illustration, Fig.3.72.
Fig.3.72
The ”new” wing attached to our part.
The idea here, is again to emphasize the
variety of ways a designer has when dealing with modeling.
This concludes our review of the extruding feature.
We went through
almost all aspects of this feature, the rest of your knowledge has now to come
from working and using your mind on finding answers to all challenges
encountered.
Whenever you don’t know how it works, experiment, you won’t hurt
anything (well, maybe your pride will suffer a bit), the software won’t mind
and you’ll learn very valuable things. Plus the boss will see you busy and
…maybe give you a bigger screen or more memory for your system.
CHAPTER FOUR
REVOLVING
FEATURES.
It is time to attack the
problem of revolved surfaces or surfaces of revolution or rather the art of
obtaining solids using the revolving feature.
Maybe a word or two
about this feature are necessary here at the beginning.
We say “revolving
surfaces” but in fact, we mean “revolving solids”; both of these two terms are
valid in solid modeling. By revolving an open
profile, what we obtain is a revolving
surface.
By revolving a closed profile, we obtain a revolved feature, which is in fact a
solid.
A revolving feature is created by revolving (rotating) a
sketch around a line.
The sketch becomes our profile to be revolved, while the
line becomes the pivot, the axis of revolution.
In order to work, a
revolving feature must have both the sketch and the axis in the same plane.
In the picture shown
below, we revolved the same circular profile once around the X axis and once
around the Y axis, just to demonstrate this idea.
On looking to use the Z
axis for the same purpose, one gets an error message, the software can not do
it, Z is perpendicular to the profile.
A note of precaution
must be issued here: be careful when revolving a sketch around different axis
of rotation, the resulting shape varies.
In the example below, because the profile is a symmetrical
one (a circle), the results are similar.
Fig.4.1
How many revolutions
in one plane?
A note: the
two rings depicted above make one single solid, as we explained before.
They are the result of two revolutions (features) and thus
they make a solid with two features.
So, only two revolved
solids can be obtained from a sketch (profile) belonging in the XY plane: one
around the X axis and the other around the Y axis. Both are identical, because
both axes are bordering the plane, thus being parallel to the profile, and the
profile is symmetrical.
Is this true?
No, it is not!
Have a look at this:
We start with a sketch
(profile) and four lines in the same plane:
