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This task shows you how to extrude
multiple profiles belonging to a same sketch using different length values.
The multi-pad capability lets you do this at one time. At the end of the
task you will see how to edit the resulting feature. |
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Open
the Pad1.CATPart document. |
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1. |
Click the Multi-Pad icon
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2. |
Select Sketch.2 that contains the
profiles to be extruded. Note that all profiles must be closed and must not intersect.
The Multi-Pad Definition dialog box appears and the profiles are
highlighted in green. For each of them, you can drag associated
manipulators to define the extrusion value. |
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The red arrow normal to the sketch indicates the proposed extrusion direction. To reverse it, you just
need to click it.
The Multi- Pad Definition dialog box displays the
number of domains to be extruded. In our example, the application has
detected seven extrusions to perform, as indicated in the Domains section. |
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3. |
Select Extrusion domain.1 from the dialog box.
Extrusion domain.1 now appears in blue in the geometry area. |
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4. |
Specify the length by entering a value. For
example, enter 10mm. |
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5. |
You need to repeat the operation for each extrusion
domain by entering the value of your choice. For example, select Extrusion
domain.2 and Extrusion domain.7 and enter 30mm and 40mm respectively. |
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For complex sketches, the Preview
button proves to be quite useful. |
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6. |
Note
that you can multi-select extrusion domains from the list before defining a
common length: multi-select Extrusion domain.3, Extrusion domain.4,
Extrusion domain.5 and Extrusion domain.6, then enter 50 as the common
length value. |
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One length value is now defined for
each profile of Sketch.2. |
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7. |
Click the More button to expand the dialog box. |
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8. |
In the Second Limit field, you can specify a
length value for the opposite direction. For example, select Extrusion
domain.1 and enter 40mm in the
length field.
Note that the Thickness section displays the sum of the two lengths.
Extrusion domain.1 's total length is 50 mm. |
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Unchecking the Normal to sketch option lets you
specify a new extrusion direction. Just select the geometry of your choice
to use it as a reference. |
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9. |
Click OK to create the multi-pad. The
multi-pad (identified as Multi-Pad.xxx) is added to the
specification tree. |
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Editing the Multi-Pad
The rest of the scenario shows you what happens when :
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Adding an Extrusion Domain
Example 1: the new profile is sketched outside existing extrusion
domains
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10. |
Double-click
Sketch.2 to edit it: for example,
sketch a closed profile outside Extrusion domain.1. |
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11. |
Quit the Sketcher. A warning message informs you that the application
has detected that the initial geometry has been modified. Close the window. |
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12. |
Double-click
MultiPad.1. The
Feature Definition Error window displays, providing the details of the
modification. |
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13. |
Click OK to close the window. The
Multi-Pocket Definition dialog box reappears.
The new extrusion domain "Extrusion domain.8" is indicated.
Select it and define the value of your choice. |
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14. |
Click OK to confirm.
Multi-pad.1 is
now composed of eight pads. |
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Example 2: the
new profile is sketched inside an existing extrusion domain |
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15. |
Double-click the sketch and for example,
add a closed profile inside Extrusion domain.2. |
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16. |
Quit the Sketcher. A warning message informs you that the application
has detected that the initial sketch has been modified. Close this window. |
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17. |
Double-click MultiPad.1. The
Feature Definition Error window displays, providing the details of the
modification. |
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When
sketching a profile inside an existing extrusion domain, the
application deletes that existing domain and replaces it with a new
one. This is why the message window displays :
-1 extrusion domain deleted (Extrusion domain.2)
-2 extrusion domains created (Extrusion domain.9, which replaces Extrusion
domain.2 and Extrusion domain.10) |
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18. |
Click OK to close the window.
The Multi-Pad Definition dialog box reappears. "Extrusion domain.2"
is no more displayed.
On the contrary, two new extrusion domains "Extrusion domain.9"
"Extrusion domain.10" are indicated with 0mm as their default
thickness. |
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19. |
Select "Extrusion domain.9"
if not already done and define
30mm as the length value. |
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20. |
Select "Extrusion domain.10",
that is the circle, and define 60mm as the length value. |
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21. |
Click OK to confirm. Multi-pad.1 is
now composed of nine pads. |
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Deleting an Extrusion Domain
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22. |
Double-click Sketch.2 and for example,
delete
Extrusion Domain.6. |
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23. |
Quit the Sketcher: the application
has detected that the initial sketch has been modified: |
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24. |
To tackle the problem, you can:
| edit or delete MultiPad.1. |
| or you can edit or delete Extrusion domain.6 |
Make sure that MultiPad.1 is selected and click the Edit button. The
Feature Definition Error window displays, providing the details of the
modification. |
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25. |
Click OK to close the window. The
Multi-Pad Definition dialog box reappears. Only eight extrusion domains
are indicated in the Domains category. |
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26. |
Click OK to confirm. The new multi-pad
feature is composed of eight pads. |
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