You can create a swept volume by sweeping out a closed
profile in planes normal to a spine curve while taking other user-defined parameters (such
as guide curves and reference elements) into account.
You can create a swept volume by sweeping out an explicit profile.
With reference surface
You can create a swept volume with explicit profile by defining reference surface and guide curve.
From the Volume section of the action bar, click Volume Sweep .
Click the Explicit profile type icon.
In the Subtype list, select With reference surface.
In the
Profile box, select a profile to be swept out.
In the Guide curve box, select a curve.
Select a surface
(by default, the reference surface is the mean plane of the spine) in
order to control the position of the profile during the sweep.
Note that in this case, the guiding curve must lie completely on this
reference surface, except if it is a plane. You can impose an angle
on this surface.
Click OK
to create the swept volume.
With two guide curves
You can create a swept volume with an explicit profile by defining two guide curves.
Click Volume Sweep
.
Click the Explicit Profile type icon.
In the Subtype list, select With reference surface.
In the
Profile box, select the profile to be swept out.
In the Guide curve 1 box, select a guide curve.
In the Guide curve 2 box, select a second guide curve.
You can also specify anchor points for each guide. These anchor points are
intersection points between the guides and the profile's plane or the profile
itself, through which the guiding curves will pass.
There are two anchoring types:
Two points: select anchor points on the profile that will
be matched respectively to guide curve 1 and 2. These points must belong to the
sweeping plane of the profile. If the profile is open, these points are optional
and the extremities of the profile are used.
Point and direction: select an anchor point on the
profile which will be matched onto guide curve 1 and an anchor direction.
If you do not explicitly select anchor points or anchor direction, they are
automatically computed if the profile is planar. Note that the selection is still
available. The anchor points are computed as follows:
For Anchor point 1: intersection between the profile
plane and Guide curve 1 (I1).
For Anchor point 2: intersection between the plane,
passing through Anchor point 1 and normal to the spine, with Guide curve 2
(I2).
For Anchor direction: line between I1 and I2.
Click OK to create the swept volume.
With pulling direction
You can create a swept volume with explicit profile by defining pulling direction
and guide curve.
The With pulling Direction subtype is equivalent to the With reference surface subtype
with a reference plane normal to the pulling direction.
Click VolumeSweep
.
The Swept Volume Definition dialog box appears.
Click the Explicit profile type icon.
In the Subtype list, select With pulling
direction.
In the Profile box, select the profile to be swept
out.
In the Guide curve box, select the curve.
In the Direction box, select a direction.
Click OK to create the swept volume.
Create a Swept Volume with a Linear Profile
You can create swept volume with a linear profile by defining guide curve and draft
direction.
Click Volume Sweep
.
The Swept Volume Definition dialog box appears.
Click the Line profile type icon.
The With draft direction sub-type is automatically
selected and grayed out.
In the Guide box, select a guide curve.
You can select a closed planar curve or any surface (planar or non-planar) as a
guide curve.
In the Draft direction box, select a draft direction
Draft direction can be a line, a plane or components.
Select the draft computation mode:
Square: a plane normal to the draft direction is used as
the reference surface and the projection of the guide curve onto this plane is used
as the spine.
Cone: envelop of cones defined along a given curve. In
order to have swept start and end planes similar as the square mode, the guide curve
needs to be extrapolated and the resulting volume Split.
Choose the angular definition:
Wholly defined: the angular value varies during the whole
sweeping operation.
G1-Constant: a different draft value for every G1 section
can be set; in this case, a relimiting plane is requested when defining
lengths.
Location values: on given points on the curve, angular
values can be defined.
Important:
This tab is only available for a square computation mode and
will work only on G1 curves.
Choose the length types:
From curve: the swept volume starts from the curve.
From/Up to: the length is computed by intersecting a plane
or a surface; a point can be selected: a plane parallel to the draft plane would be
computed.
From extremum: the lengths are defined along the draft
direction from an extremum plane; L1 corresponds to the "maximum plane" in the draft
direction, L2 corresponds to the "minimum plane" in the draft direction.
Click OK to create the swept volume.
Create a Swept Volume with a Circular Profile
You can create a swept volume with a circular profile by defining the center curves
and other parameters.
You can create a swept volume with circular profile by defining center and
reference curves.
Click VolumeSweep
.
The Swept Volume Definition dialog box appears.
Click the Circle profile icon.
In the Subtype list, select Center and reference
curve.
In the Center curve box, select a curve.
In the Reference curve, select a reference curve.
Optional:
Select the Use fixed radius check box and enter the value of
the fixed radius.
Click OK to create the swept volume.
Center and radius
You can create a swept volume with circular profile by defining center curve and
radius.
Click VolumeSweep
.
The Swept Volume Definition dialog box
appears.
Click the Circle profile icon.
In the Subtype list, select Center and
radius.
In the Center curve box, select a curve.
Here we selected DemoCurve2.
In the Radius box, enter the value or use the arrows to
change the value.
Here we entered radius value as 10mm.
Click OK to create the swept volume.
Preview the Angular Value
You can preview the various solutions you can get after completion of
operation.
Important:
This option is available with:
Explicit profile: With reference surface and With pulling
direction sub-types.
Linear profile: With draft direction sub-type.
When creating a swept volume, you are now able to preview the four solutions based
on the values given for the Angle and
Lengths. The first solution corresponds to Angle, Length1 and
Length2 values, the second solution to -Angle, Length1 and Length2
values, the third solution to Angle, Length2 and Length1 values, and the
fourth solution to -Angle, Length2 and Length1 values.
The orange arrow corresponds to the current solution.
Click on any arrow then on Preview or
OK to recompute the swept volume. You can also use the
Previous or Next buttons or enter a
solution number in the Angular sector box:
Define Relimiters
You can define relimiters to get expected swept volume.
Relimiters can be selected on a closed curve (curve, spine, or default spine). In that
case, you are advised to define points as relimiters, as plane selection may lead to
unexpected results due to multi-intersection.
You can relimit the default spine, thus avoiding to split it to create the swept
volume.
Select a relimiter in the Relimiter 1 and/or the
Relimiter 2 boxes.
Below is an example with a plane as Relimiter 1:
Smooth
You can define the smoothing parameters on the swept volumes.
Select the Angular correction check box to smooth the
sweeping motion along the reference surface. This may be necessary when small
discontinuities are detected with regards to the spine tangency or the reference
surface's normal. The smoothing is done for any discontinuity which angular deviation
is smaller than 0.5 degree, and therefore helps generating better quality for the
resulting swept volume. By default, the angular correction is set to 0.5 degree.
Check Deviation from guide(s) to smooth the sweeping motion
by deviating from the guide curve(s). A curve
smooth is performed using correction default parameters in tangency and
curvature. This option is unavailable for with tangency surface subtype.
Remove Twisted Areas
During creation or edition, you can generate swept surfaces that have a twisted
area by delimiting the portions of the swept surface to be kept.
The generated surface is therefore composed of several unconnected portions.
Select the Remove cutters on Preview check box to remove the
twisted areas management each time you click on Preview. This
option is selected by default.
Use the Setback slider to define a distance to move all the
cutters from the twisted areas. It is defined as a percentage of the guide length from
0 to 20%. Its default value is 2%.
Select the Fill twisted areas check box to fill the twisted
zones. It is activated by default.
Important:
When you select this check box, the Setback slider
affects only the cutters that have not been previously moved.
If you have not manually moved any cutter, and if you replace the main guide
of the sweep, the twisted areas are filled with the defined setback.
Select the Compute C0 vertices as twisted areas check box to
fill the C0 vertices areas taking into account the setback value.
It is activated by default.
Note:
This option is unavailable with the With tangency surface
and With two tangency surfaces subtypes of the linear
profile, and One guide and tangency surface subtype of the
circular profile.
Use the Connection strategy list to choose the connection
mode for the filled areas. The three options are:
Automatic: this mode chooses the best connection strategy
depending on the geometry.
Standard: this mode maintains the sweep profile.
Similar to guide: this mode maintains the point
continuity.
Important:
These modes force the chosen connection.
If Similar to guide fails, then the
Standard connection strategy is applied. If this
mode also fails, no connection strategy is applied.
Click the Add cutter button allows you to create cutters on
the main guide of the sweep.
Important:
If the Fill twisted areas check box is
selected, while the Add cutter button is clicked, the
created cutters define a filled area. Otherwise, the cutters define a cutting
zone.
Detect Canonical Shapes
You can detect the canonical shapes if they exist in the swept surface.
Select the Canonical Shape Detection check box to
automatically compute regular shapes such as cylinders, cones and spheres. Moreover,
it can automatically detect planar surfaces if they exist in the swept surface.
By default, this option is not selected.
Important:
This capability is unavailable with explicit profile.