Create Joined Elements
You can assemble the elements by joining them.
Click Join
in the Operation toolbar (Join-Healing sub-toolbar).
The Join Definition dialog box appears.
In Part Design
workbench, the Join capability is available as a
contextual command named Create Join that you can access
from Sketch-based features dialog boxes.
Select the surfaces or curves to be joined.
You can edit the list
of elements to be joined:
Right-click the elements from the list and
select Check Selection.
This lets you check whether an element to be joined
presents any intersection (i.e. at least one common point) with other
elements prior to creating the joined surface. If this command is not launched, possible intersections will not
be detected. The Checker dialog box is displayed, containing the
list of domains (i.e. sets of connected cells) belonging to the
selected elements from the Elements To Join list.
Click Preview.
-
An information message is issued informing when no intersection
is found ("No topological problem found").
-
When an element is self-intersecting, or when several
elements intersect, a text is displayed on the geometry, where the
intersection is detected.
Click Cancel to return to the Join Definition box.
Right-click the
elements again and choose one of the options below to allow the selection
of elements of same dimension.
- Distance Propagation: the tolerance
corresponds to the Merging distance
value (as explained in step 14).
- Angular Propagation:
the tolerance corresponds to the Angular Threshold value, if defined (as explained in step 15). Otherwise, it corresponds
to the G1 tolerance value as defined in the part.
Each new element found by propagation of the selected
element(s) is highlighted and added to the Elements To Join
list.
Click Preview in the
Join Definition dialog box.
The joined element is previewed, and its orientation
displayed. Click the red arrow to invert it if needed.
The join is oriented according to the first element in
the list. If you change this element, the join's orientation is
automatically set to match the orientation of the new topmost element
in the list.
Select the Check
tangency check box to find out whether the elements to be joined are tangent.
If they are not, and the option is selected, an error message is issued
when you click Preview advising you to modify the selected
inputs. Elements in error are highlighted in the 3D geometry once you
have clicked OK in the Update
Error dialog box:
Select the Check connexity check box to find out
whether the elements to be joined are connex. If they are not, and the
option is selected, an error message is issued indicating the number of
connex domains in the resulting join and elements in error are
highlighted in the 3D geometry.
Select the Check
manifold check box to find out whether the resulting join is manifold.
Select the Simplify the result check
box to
allow the system to automatically reduce the number of elements (faces or
edges) in the resulting join whenever possible.
Select the Ignore erroneous elements
check box to let the system ignore surfaces and edges that
would not allow the join to be created.
You can also
set the tolerance at which two elements are considered as being only one
using the Merging distance.
Select the Angular Threshold
check box and specify the angle value below
which the elements are to be joined.
Click the Sub-Elements To Remove
tab to display the list of sub-elements in the join.
These sub-elements are elements making up
the elements selected to create the join, such as separate faces of a
surface for example, that are to be removed from the join currently
being created.
You can edit the sub-elements list as
described above (in step 3) for the list of elements to be
joined.
Select the Create join with sub-elements
check box to create a second join, made of all the sub-elements displayed in the
list, i.e. those that are not to be joined in the first join.
Click OK to create the joined
surface or curve.
The surface or curve (identified as Join.xxx) is added
to the specification tree.
Use the Federation Capability
The purpose of the federation is to regroup several elements making up
the joined surface or curve that will be detected together with the pointer
when selecting one of them.
This is especially useful when modifying linked
geometry to avoid re-specifying all the input elements.
Create the join as usual, selecting all elements to be
joined.
In the Join Definition dialog box, click the
Federation tab, then select one of the elements making up the
elements federation (providing the No federation and All
propagation modes are not selected).
You can edit the list of elements taking part in the federation
as described above (in step 3) for the list of elements to be
joined.
Select a propagation mode, the system automatically
selects the elements making up the federation, taking this propagation
mode into account.
- No federation: no element can be selected
- All: all elements belonging to the resulting joined
curve/surface are part of the federation. Therefore, no element can
be explicitly selected.
- Point continuity: all elements that present a point
continuity with the selected elements and the continuous elements
are selected.
- Tangent continuity: all the elements that
are tangent to the selected element, and the ones tangent to it, are
part of the federation.
Here, only the top faces of the joined surface are
detected, not the lateral faces.
- No propagation: only the
elements explicitly selected are part of the federation.
Select the Tangency continuity propagation
mode.
Move to the Part Design workbench, select the sketch and click
Pad
to create an up to surface pad, using the joined surface as
the limiting surface.
Select the front edge of the pad, click Edge Fillet
and create a 2mm fillet.
Double-click the sketch from the specification tree, then
double-click the constraint on the sketch to change it to 10mm from the
Constraint Definition dialog box.
Sketch prior to modification lying over two faces
Sketch after modification lying over one face only
Exit the sketcher
.
The up to surface pad is automatically recomputed even though it
does not lie over the same faces of the surface as before, because
these two faces belong to the same federation. This would not be the
case if the federation including all top faces would not have been
created, as shown below.
Double-click the joined surface to edit it, and
choose the No propagation mode.
Click OK in the Join Definition dialog box.
A warning message is issued, informing you that an edge no longer
is recognized on the pad.
Click OK.
The Update Diagnosis dialog box is displayed, allowing you to
re-enter the specifications for the edge, and its fillet.
You then need to edit the edge and re-do the fillet to obtain the
previous pad up to the joined surface.
Select the Edge.1 line, click the Edit button,
and re-select the pad's edge in the geometry.
Click OK in the Edit dialog box.
The fillet is recomputed based on the correct edge.
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