Drafts are defined on molded parts to
make them easier to remove from molds. |
The characteristic elements are: |
| pulling direction: this direction corresponds to the reference from
which the draft faces are defined. |
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| draft angle: this is the angle that the draft faces make with the
pulling direction. This angle may be defined for each face. |
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| parting element: this plane, face or surface cuts the part in two and
each portion is drafted according to its previously defined direction. For an example,
please refer to Draft with Parting Element. |
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| neutral element: this element defines a neutral curve on which the
drafted face will lie. This element will remain the same during the draft. The neutral
element and parting element may be the same element, as shown in Draft
with Parting Element. |
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There are two ways of determining the
objects to draft. Either by explicitly selecting the object or by selecting the neutral
element, which makes CATIA detect the appropriate faces to use. This task shows you how
to create a basic draft by selecting the neutral element. |
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Open the Draft2.CATPart document. |
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1. |
Click the Draft Angle icon . |
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The Draft Definition dialog box is displayed and an arrow
appears on a plane, indicating the default pulling direction. |
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This dialog box displays the constant angle
draft option as activated. If you click the icon to the right, you then
access the command for creating variable angle
drafts. |
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2.
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Check the Selection by neutral face option to
determine the selection mode. |
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3. |
Select the upper face as the neutral element. This
selection allows CATIA to detect the face to be drafted.
The neutral element is now displayed in blue, the neutral curve is in pink. The faces
to be drafted are in dark red.
The Propagation option can be set to:
| None: there is no propagation |
| Smooth: the application integrates the faces propagated in tangency onto the neutral
face to define the neutral element. |
For more about the neutral element, refer to A Few
Notes about Drafts. |
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The pulling direction is now
displayed on top of the part. It is normal to the neutral face.
The
Controlled by reference option is now activated, meaning that whenever you
will edit the element defining the pulling direction, you will modify the
draft accordingly. |
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Note that when using the other selection mode
(explicit selection), the selected objects are displayed in dark pink. |
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4. |
The default angle value is 5. Enter
7 degrees as the new angle value. The application displays the new angle value in the geometry. |
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5. |
Click Preview
to see the draft to be created. It appears in blue. |
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6. |
Click the More button to access
additional options.
To know how to use the options "Parting Element" and
"Draft Form", refer to Draft with Parting Element. |
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7. |
Click the
Limiting element(s) field. While drafting a face, you can limit it by
selecting one or more faces or planes that intersect it completely. |
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8. |
Select Plane.1 as the limiting element.
The arrow points to the portion of material to be kept to perform the
operation. |
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9. |
Select Plane.2 as the
second limiting element.
Note that the number of limiting elements you select is indicated in
the dialog box, just in front of the Limiting Elements field.
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10. |
Click the arrow to
reverse its direction, and therefore retain the opposite side of the
feature. |
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When using several limiting
elements, make sure that they do not intersect on the face to be drafted. |
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11. |
Click OK to confirm the operation. The
faces are drafted but the part areas included between both limiting planes
have not been modified, as specified through the limiting element option. |
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Editing Drafts
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If you edit the sketch used for defining the
initial pad, CATIA integrates this modification and computes the draft again. In the
following example, a chamfer was added to the profile. |
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You can now transform a
constant angle draft into a variable angle draft. To do so, double-click
your draft, then click the variable angle draft option in the dialog box
to access the appropriate options. For more, refer to Variable
Angle Draft. |
Neutral Elements
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It is possible to select several
faces to define the neutral element. By default,
the pulling direction is given by the first face you select. This is an
example of what you can get: |
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Draft Definition |
Result |
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You
can use neutral elements that do not intersect the faces to be
drafted. This is an example of what you can get: |
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Draft Definition |
Result |
Methodology
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If you need to draft several faces
using a pulling direction normal to the neutral element, keep in mind the following
operating mode that will facilitate your design: Click and first select the neutral
element of your choice. The pulling direction that appears is then normal to the neutral
element. Select the face to be drafted and click OK to create your first draft.
Now, to create the other drafts in the same CATPart document, note that by default the
application uses the same pulling direction as the one specified for creating your first
draft. As designers usually use a unique pulling direction, you do not need to redefine
your pulling direction. |
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If you
perform a difficult drafting, for example if you obtain twisted faces, use
the Deactivate and Extract Geometry commands to
solve your difficulties. For more information, refer to Extracting
Geometry. |
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