Surfaces
A surface is a sheet of solid material
with no thickness. It is a feature, just like other solid features or Datum
Planes; however, since it has no thickness, it has no volume or mass.
There are three primary reasons to use surfaces when constructing
solid geometry:
· To create surface geometry that you cannot
create using solid creation methods.
· Your preferred construction technique
involves creating a set of surfaces before you make the solid. In other words,
the solid is created in two steps, where step one is making the surfaces and
step two is constructing the solid geometry.
· Creating a surface first allows you to
verify that the desired geometry is created before you commit to adding
it to your existing part.
For example, you can create a Solid Protrusion by
generating a Sweep of a section. You can also create a Surface
by generating a similar Sweep. The difference between the
resulting features is that creating a Solid Protrusion results in
a closed, solid mass, whereas creating a Surface generates a sheet
with no enclosed mass.
In Pro/ENGINEER, a Surface is
a single entity, developed with one operation on a single entity - for example:
extruding or revolving a straight line. A Quilt is a feature made
up of a patchwork of Surfaces. Both of these Surface features were created
using a single sketch; the single Surface section contains only a single swept
line, while the surface Quilt section contains multiple swept entities. Appart
from standard creation techniques for Surfaces and Quilts with which you are
already familiar when building solid features, there exist additional methods
to create surface features. The list includes the following tools:
Boundary Blend, Style, Warp
Surface and Quilt features (generically referred to as surface features)
may be joined together using the Merge function and they may be subdivided using the Trim function. Surface
features can be used further to construct solid or thin protrusions, or to modify
existing solid features.
Surfaces are created as features, just
like any other entity in Pro/ENGINEER. As such, they may be
redefined, patterned, copied, or deleted exactly like any other feature.
Surfaces may be created prior to creating the first solid feature, by
referencing the Default Datums, or any preexisting Datum Curves.
As
an example we will construct surfaces with the Boundary Blend tool,
but
first we use fetch_proe
surf.prt to
get a copy of the example file.
Once the Surf.prt is
loaded into Pro/E we will build a surface using the two existing datum
curves. See Fig 1.
·
Select 
the Boundary Blend tool.
|
Figure 1 |
Figure 2 |
·
Select one datum
curve and with the CTRL-key depressed select the second datum curve. To
complete the feature click on the Check-icon in the dash board. See Fig 2.
This surface is built with no specific constraints on
its edges. One is able to specify explicit constraints. We will specify that
the edges shall be normal to both datum planes. Select Edit Definition
and set the Constraints to
·
Now Mirror the
surface around the FRONT
datum plane to create Blend2. First select Blend1
and the 
- icon, next
click on datum plane. See Fig 4 below.
|
Figure 3 |
Figure 4 |
·
Next Mirror Blend1 and Blend2 about RIGHT datum plane to cretae Blend3 and Blend4.
·
Now Merge 
Blend1 and Blend2 to create Merge1.
·
Next Merge Blend3 and Blend4 into Merge2.
·
Next we Merge Merge1 and
Merge2 to create Merge3.
Only now have our surfaces become a single connected Quilt, which can be converted into a Solid.
·
We create a solid
by clicking on Merge3 and selecting Edit –
Solidify. See Fig 5 for the completed
model tree and Fig 6 for the finished model.
|
Figure
5 - Model Tree |
Figure
6 – Finished Model |
