CATIA V5 is the newest release of the
long-standing 3D CAD software from Dassault
Systemes. It is the first full release to be
available on the PC platform (NT). There are
many changes over the previous UNIX-based V4.
This quick demonstration will outline one basic
approach to 3D design.
1. Solid model creation of 3D objects has become much
easier. To begin with, we should use the 'Mechanical Design' Workbench.
We want to create an arc segment and a horizonal centerline for
revoltion surface later. As with CATIA V2 - V4, wireframe geometry
creation begins with the selection of a plane. We will select the ZX
plane for ourselves. Select the plane directly from the display or from
the Product tree. In both cases, the selected element should be
highlighted to indicate it has been selected.
2. The sketcher can be started on the selected plane
with the 'Sketcher' Workbench. The display will change to a 2D grid, and
the sketcher icons should apear on the toolbar. We want our arc segment
close to the axis, but stll fairly flat - 205mm Radius with centerpoint
200mm away from H axis..
3. We first draw our horizonal centerline for our later surface of
revolution. We draw a horizonatal line well under the (H)orizontal axis.
We may specify its distance from the H axis by using the CONSTRAINT
function and then selecting our line and (H)orizonal axis. A green
constraint dimension representing the distance should appear. Use the
left mouse button to fix it in position.
4. Double-click the new distance constraint. A dialogue box should
appear. Enter the Radius dimension "200"(millimeters).
Now we want to create our arc segment.
METHOD 1 (Using Trim):
One way to create an arc segment is to trim a
circle to endpoints. We create a circle with
the "CIRCLE" function. Using CONSTRAINT, we will specify a 410mm diameter
(R205mm), and a distrance of 200mm between the (H)orizonal axis and the circle's
We will create two vertical lines and use the "TRIM" function to create our
1. Create two vertical lines that intersect the circle above.
2. Constrain the distance a) between the two vertical trim lines and b)
between one of those two trim lines and the (V)ertical axis. Specify a distance
between the (V)ertical axis and one trim line at 25mm, and a
distance of 50 between the two trim lines themselves.
3. Click the TRIM icon, then the circle and one trim line.
Repeat process with the second one.
You must probably also constrain a distance of '0' between the
circle's centerpoint and the V axis.
METHOD 2 (Using ARC and SmartPick):
The above method was discussed so that
you would like the next mothod even more:-). Using the 'CTRL' key, many entities
may be selected at once for setting a constraint. This is the real key to
setting many SYMMETRICAL constraints.
1. You will have to find the ARC function (it might be hiding under the
CIRCLE sub-panel). We will select the left endpoint of our centerline
for our arc segment's centerpoint. Drag the mouse upward, above
the (H)orizontal axis, and click the left mouse button to create the arc
2. Add a radius constrain to the new arc segment
by selecting it and clicking the CONSTRAIN icon. Use the left mouse button to
fix the constraint's position.
3. Double-click the new radius constraint. A dialogue box should
appear. Enter the Radius dimension "205"(millimeters).
4. Select the CONSTRAIN function and the two endpoints of our
arc segment. After fixing the constraint's position in the workspace,
change its value to "50".
5. Using the CTRL key (or Strg), select both endpoints from the
arc segment again. While still holding the CTRL key, also select the
(V)ertical axis. Select the constraint function. A dialogue box listing
available constraints should appear. Select 'SYMMETRY'.
This quickly establishes exactly what we want: an R205 arc sement
with a horizontal length of 50, using the (V)ertical axis as our line of
You may exit SKETCHER using EXIT.