Programming Multibody Parts
This topic provides information about programming multibody
parts using the SolidWorks API. Click a link to read that section.
Obsoleted methods and their replacements
When programming multibody parts:
|
Do not use... |
Instead, use... |
Because... |
|
IFeature::GetBody |
IFeature::GetFaces
IFace2::GetBody |
A feature can affect more than one body. Therefore, getting the faces
created by a feature and getting the bodies to which the faces belong
is a better way to get a feature's body or bodies. |
|
IPartDoc::Body
IPartDoc::IBodyObject2 |
|
It no longer makes sense to get the body of a part if it contains multiple
bodies. In a single-body part, IPartDoc::Body and IPartDoc::IBodyObject2
still return the body, but in a multibody part, they return NULL. |
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Changes to base features
Most of the methods for creating base features (cut and boss, including
thin features) belong to IFeatureManager:
These methods may include any of the following parameters that support
multibody parts:
|
If this parameter... |
Is set to... |
Then... |
|
merge |
TRUE |
Merging occurs and feature scope applies. |
|
|
FALSE |
Merging does not occur and feature scope does not apply. |
|
useFeatScope |
TRUE |
All currently selected bodies are affected. |
|
|
FALSE |
All applicable bodies are affected . |
|
UseAutoSelect |
TRUE |
All applicable bodies are added to the selection list, which the user
can edit. |
|
|
FALSE |
User must select bodies. |
NOTES:
The merge parameter
applies to bosses, but not to cuts.
When the UseFeatScope
parameter is set to FALSE, it applies to all bodies including new bodies
placed before the feature in the FeatureManager design tree.
The UseAutoSelect
parameter applies to the existing bodies only.
Examples
IModelDoc2.IFeatureManager.IFeatureExtrusion(sd
As Boolean, flip As Boolean, dir
As Boolean, t1 As Long, t2 As Long, d1 As Double, d2 As Double, dchk1
As Boolean, dchk2 As Boolean, ddir1 As Boolean, ddir2 As Boolean, dang1
As Double, dang2 As Double, offsetReverse1 As Boolean, offsetReverse2
As Boolean, translateSurface1 As Boolean, translateSurface2 As Boolean,
merge As Boolean, useFeatScope As Boolean,
useAutoSelect As Boolean) As feature
ModelDoc2.FeatureManager.FeatureCut(sd As
Boolean, flip As Boolean, dir
As Boolean, t1 As Long, t2 As Long, d1 As Double, d2 As Double, dchk1
As Boolean, dchk2 As Boolean, ddir1 As Boolean, ddir2 As Boolean, dang1
As Double, dang2 As Double, offsetReverse1 As Boolean, offsetReverse2
As Boolean, translateSurface1 As Boolean, translateSurface2 As Boolean,
normalCut As
Boolean, useFeatScope As Boolean, useAutoSelect
As Boolean) As feature
In the following example, three solid bodies exist: Extrude1, Extrude2,
and Extrude3. To create a through-all cut through Extrude1 and Extrude3,
you could do something like the following. Notice the use of the mark
parameter.
Part.ModelDocExtension.SelectByID2 "Sketch5",
"SKETCH", 0, 0, 0, 1, 0, Nothing, swSelectOptionDefault 'cut
profile
Part.ModelDocExtension.SelectByID2 "Extrude3",
"SOLIDBODY",
0, 0, 0, 1, 1, Nothing, swSelectOptionDefault 'body
to affect
Part.ModelDocExtension.SelectByID2 "Extrude1",
"SOLIDBODY",
0, 0, 0, 1, 1, Nothing, swSelectOptionDefault 'body
to affect
Part.FeatureManager.FeatureCut
1, 0, 0, 1, 0, 0.058, 0.058, 0, 0, 0, 0, 0.01, 0.01, 0, 0, 0, 0, 0, 1, 0 'use feature scope, do not use
Autoselect
You can observe this by recording a macro and playing it back.
In the following example, again three solid bodies exist: Extrude1,
Extrude2, and Extrude. However, in this example, a through-all extrusion
boss is created and merges with Extrude1 and Extrude3. Notice the use
of the mark parameter and that merge is set to TRUE.
Part.ModelDocExtension.SelectByID2 "Sketch4",
"SKETCH", 0, 0, 0, 1, 0, Nothing, swSelectOptionDefault boss
profile
Part.ModelDocExtension.SelectByID2 "Extrude3",
"SOLIDBODY",
0, 0, 0, 1, 1, Nothing, swSelectOptionDefault 'body
to affect
Part.ModelDocExtension.SelectByID2 "Extrude1",
"SOLIDBODY",
0,0,0, 1, 1, Nothing, swSelectOptionDefault 'body
to affect
Part.FeatureManager.FeatureExtrusion
1, 0, 1, 1, 0, 0.047, 0.047, 0, 0, 0, 0, 0.01, 0.01, 0, 0, 0, 0, 1, 1, 0 'merge, use feature scope, do
not use Autoselect
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Modifying the definition of solid features that
use feature scope
The IExtrudeFeatureData2,
ILoftFeatureData,
IRevolveFeatureData2,
ISweepFeatureData,
and IThickenFeatureData
have methods and properties that support multibody parts:
|
Methods: |
|
|
Properties: |
AutoSelect
(VARIANT_BOOL) FeatureScope
(VARIANT_BOOL) FeatureScopeBodies
(VARIANT array of bodies) |
When you get or set FeatureScopeBodies,
that feature then affects all bodies in that array. Make sure that any
bodies that you set in this array exist and that IBody2
objects are valid when the feature is in its rolled-back state (after
AccessSelections
is called). If the bodies are not available, then you might have to reorder
features in the FeatureManager design tree to achieve the desired result.
Also, if FeatureScope
is set to false or merge is set to true, then GetFeatureScopeBodiesCount
returns 0 and FeatureScopeBodies
is an empty array.
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