Cad Guidebook: A Basic Manual for Understanding and Improving Computer-Aided Design (43 page)

Understanding how the perfectly tangent situation causes a problem for
stitching, the user could think ahead about this issue and deal with it accordingly.
Perhaps this part is going to have a shaft welded to the top of the block, so there
is really weld material between the two features. If the weld is actually modeled
(by adding some new 2-D sketch geometry with the circle), then the tangency
issue can be avoided. Refer to Figure 8.12. Understanding stitching is often the
key to knowing which method to use.

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FIGURE
8.12

Modeling as manufactured can avoid the tangent surface problem.

8.3.6.2 Joining Versus Adding

Earlier in this section, protruding was defined as an operation on a part that cre-
ated new volume for the part. It is the opposite of cutting. Note that it is assumed
that the protrude operation is going to force the CAD system to figure out how all
the surfaces stitch together (as was just discussed). When the system does suc-
cessfully calculate the stitched surfaces, the feature can be referred to as joined.
Although join seems to mean that it only applies to protruding, the need for
stitching surfaces also exists when the feature is a cutout.

However, some CAD systems may allow a new step in the part history, but
without the stitching process. This is sometimes referred to as adding (as opposed
to joining). In the add operation, the history of the part simply considers the new
volume of the new feature to be a step in the history, but the new feature has no
effect on any other area of the part. Clearly this is not a good idea in many cases
(interference is being ignored). For instance, the CAD system cannot reliably
calculate the volume of such a part (the 2 volumes might be interfering sig-
nificantly). On the other hand, if the user just wanted to show some 3-D geometry
as just a “reference” (such as weld material in the earlier example), then the add

Part Modeling 203

operation might be satisfactory. The part will look right, in this case, and per-
haps the weld is not supposed to calculated as part of the volume or weight of the
part anyway.

8.3.7 Summary: Creating New Features

At this point, the critical issue that the user needs to understand is that each time
a new sketch plane has been selected, one has started the process for creating a
new feature. And, if the process is completed, this feature is then going to be
shown in the part history data in some fashion. Also, it is essential to realize that
one has, at some point in the process, specified an operation (such as join, add,
cut, intersect, etc.) for how each new feature affects the state of the part model.

Realizing this, it is essential that the user somehow formulate a plan or
strategy for part modeling. A good plan of attack can make a part that replays
more quickly, and changes to features can be made more easily. With no plan-
ning, one can count on eventually having a rather frustrating experience trying to
rearrange or completely redrawing the part model.

8.4 SKETCH CONSTRAINTS

Constraints or constraining is somewhat of a point of contention between various
3-D CAD systems and their users. It is controversial since some CAD system
vendors insist this process is absolutely essential and any part not fully con-
strained is useless. On the other hand, some 3-D CAD systems do not have robust
constraint solving algorithms and their 3-D part models wind up being incapable
of being intelligently revised and re-used as designs evolve. This book assumes
that constraining is a very important feature of 3-D CAD systems, and they
should be used whenever it makes sense to do so.

8.4.1 What is Constraining?

As the name implies, constraining is a process of limiting or restricting the geom-
etry that is being created. The simplest example is showing a dimension in a
drawing. Imagine a drawing with a part that has a hole, and the drawing has a
dimension that indicates the diameter of the hole. This dimension fixes or re-
stricts the hole size. If a hole is shown without a dimension, one knows that it is a
circular feature, but the diameter could be anything. So, the diameter dimension
constrains the hole size, and this dimension can be referred to as a constraint.
Other types of constraints are more purely geometric. They would be constraints
such as parallelism (forcing 2 lines to be parallel), or coincidence (forcing one
line segment’s endpoint to be connected to another line segment’s endpoint).

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8.4.2 Dimensional Constraints

Referring to Figure 8.13, one can see that the hole has a dimension for its diame-
ter (15.00). Although the size of the hole can now be considered constrained,
there needs to be more information to fully define the sketch. In particular, there
needs to be an indication of where the hole would be located with respect to the
rest of the part. This can be accomplished by more dimensions such as the hori-
zontal dimension (45.00) and the vertical dimension (35.00) shown. These di-
mensions constrain the location of the hole, and again, these dimensions can be
considered constraints.

8.4.3 Geometric Constraints

Referring to Figure 8.14, the circular hole has now been replaced with a rectan-
gular-type of slot. Once again, dimensions can be shown on the sketch to con-
strain the size of the slot. However, notice that the horizontal and vertical
dimensions that position the slot (45.0 and 35.0) are to the center of one of the
arcs for the slot. It does appear, at first, that this would completely describe the
feature, and that anyone reading this information as a drawing would know how
to manufacture the part. But the problem is that there is no way to be sure that the
slot can not rotate about the center of that arc. The dimensions were to just a
central point. The slot can be imagined to be free to rotate about that point with
an axis of rotation sticking out from the page. There is nothing in the dimensions
that explicitly demands that the slot be parallel to the bottom edge of the plate.

Understanding a problem like this rotating slot sketch is crucial to benefit-
ing from the constraining process. Almost anyone would assume from a drawing
that looked like Figure 8.14 that the slot is supposed to be parallel to the bottom

FIGURE
8.13

Example feature sketch with dimensions as constraints.

Part Modeling 205

FIGURE
8.14

Example feature sketch with some geometry-based constraints.

of the part. But, this is just an assumption or an impression. People who read
drawings make assumptions like this all the time. But 3-D CAD does not always
allow these assumptions. With the 3-D CAD system, the central idea is to not just
create a 3-D part, but rather to create a part MODEL that contains a mathematical
system that can change and evolve intelligently and predictably. Geometric con-
straints are an essential ingredient in this process.

So, to completely constrain the slot with the dimensions shown, new con-
straint information needs to be added. One possibility would be to indicate that
the slot is horizontal. Another possibility would be to indicate that the slot is par-
allel to the bottom edge of the part. Looking at Figure 8.14, one can see that there
is an H symbol near the bottom line of the slot. This symbol indicates to the de-
signer that the line is forced to be horizontal. The CAD system usually automati-
cally detects when lines are drawn in a horizontal position and adds the constraint
for a line automatically to be horizontal (or vertical, parallel, etc.), but users still
need to be aware of the meaning of these constraints. The H is shown on the bot-
tom line only, so that would only properly constrain the bottom line. Looking at
the top line of the slot, there is a parallelism symbol (2 short lines together). It has
a partner symbol on the bottom line. These 2 symbols form a pair and would be
identified as a single constraint. It indicates that the top line is parallel to the bot-
tom. The exact symbols and their meaning differ for the different CAD systems;
but these symbols are typical. These added geometric constraints should “fix” or
control the problem of rotating the feature about the dimensions to the point for
the arc.

With the horizontal and parallel constraints in place, the sketch is said to be
better constrained. One would now think that the sketch is fully defined and that
the geometry is under control. Unfortunately, there is still something missing.
The arcs at the ends of the slot are shown as “meeting” or “connecting with” the

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straight lines, but there is no certainty that the arcs are perfectly tangent to the
lines at the exact point where they connect. The tangency condition becomes a
necessary constraint to make certain the sketch shape is under full control.

8.4.4 Degrees of Freedom

It should be clear from the previous example that there can be a fair amount of
thought and planning required in creating a good system of constraints for even a
simple 2-D sketch. One way to analyze this situation is referred to as removing
degrees of freedom (DOFs). In any 2-D sketch, there are 3 degrees of freedom
available for each entity drawn. These degrees of freedom are translation in the
X-direction (sliding horizontally), translation in the Y-direction (sliding verti-
cally), and rotation about the Z-axis (as in the slot rotating example).

For each entity, then, the designer can try to imagine if that entity is free to
move in each of the 3 Degrees of Freedom. In other words asking, “can it move in
X?,” “can it move in Y?,” “can it rotate about Z?.” If it can move in one of these
ways, then constraints can be added to remove this degree of freedom.

8.4.5 “Inheriting” Constraints

Many times, when constraints are added to a sketch, the CAD system will auto-
matically include other constraints. In a sense, the sketch is inheriting the added
constraints since they are necessary to have a consistent network of constraints.
The simplest example is adding a linear dimension between two lines as shown in
Figure 8.15. Obviously, the dimension is between the two lines, but consider the
fact that this dimension is meaningless if the lines are not forced to be perfectly
parallel. If they are not parallel, then the lines will eventually cross (and the di-
mension becomes wrong). Therefore, when the linear dimension is added be-
tween the lines, if there isn’t already a parallel constraint present, the CAD
system will most likely add the parallelism automatically.

Unfortunately, it can take quite a while to become accustomed to how the
CAD system implements these inherited constraints. They usually are necessary,
but sometimes the reason they are needed can be rather subtle. Also, sometimes
the user applies constraints in a slightly different manner, and the system may
respond quite differently. For instance, in Figure 8.15, the linear dimension was
created by picking the two lines. The system applies the inherited parallel con-
straint. However, what if the dimension was created by picking one of the lines
and then an endpoint of the other line? Now, the system may figure that the user
wanted to allow the one line to be able to rotate about that endpoint. So, the di-
mension is applied (but it is only between a point and a line), and the system may
not create the inherited parallel constraint. This is a subtle difference when the
dimension is created, and the dimension may look the same to the user, but the
sketch may easily become scrambled since the line is free to rotate.

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FIGURE
8.15

Example of inheriting a geometric constraint.

It is not really possible to consider all the ways that the constraints are in-
herited or all the ways that simple mistakes in creating constraints can cause a
sketch to become unstable. It is usually simply a matter of practice and learning
from mistakes.