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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:

  • Extrude

  • Revolve

  • Sweep

  • Loft

  • Thicken

 

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:

  • GetFeatureScopeBodiesCount

  • IGetFeatureScopeBodies

  • ISetFeatureScopeBodies

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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