Set Body for View Example (C#)
This example shows how to show just one body of a multibody part in
a drawing view.
//------------------------------
// Preconditions:
// 1. In SolidWorks, interactively open:
// <SolidWorks_install_dir>\samples\tutorial\multibody\multi_inter.sldprt
// 2. In SolidWorks, save the part document as a drawing
document:
// a.
Select File > Make Drawing from Part.
// b.
Click OK on the Sheet Format/Size
dialog.
// c.
Drag the *Isometric view from
the View Palette onto
// the
drawing sheet.
// 3. Run the macro.
//
// Postconditions: The drawing view shows one body of
the multibody part.
//
// NOTE: Because the part document is used by a
// SolidWorks online tutorial, do not save
// any changes when closing the document.
//------------------------------
using SolidWorks.Interop.sldworks;
using SolidWorks.Interop.swconst;
using System;
using System.Diagnostics;
using System.Runtime.InteropServices;
using System.Windows.Forms;
namespace BodiesViewCSharp.csproj
{
partial
class SolidWorksMacro
{
public
void Main()
{
ModelDoc2
swModel = default(ModelDoc2);
SelectionMgr
swSelMgr = default(SelectionMgr);
SolidWorks.Interop.sldworks.View
swView = default(SolidWorks.Interop.sldworks.View);
int
nbrBodies = 0;
object[]
arrBody = null;
Body2
swBody = default(Body2);
Face2
swFace = default(Face2);
Entity
swEnt = default(Entity);
SelectData
swSelData = default(SelectData);
PartDoc
swPart = default(PartDoc);
bool
status = false;
DispatchWrapper[]
arrBodiesIn = new DispatchWrapper[1];
object[]
Bodies = new object[1];
int
i = 0;
int
objType = 0;
swModel
= (ModelDoc2)swApp.ActiveDoc;
swSelMgr
= (SelectionMgr)swModel.SelectionManager;
swView
= (SolidWorks.Interop.sldworks.View)swSelMgr.GetSelectedObject6(1,
-1);
if
((swView == null))
{
MessageBox.Show("View
not selected.");
return;
}
nbrBodies
= swView.GetBodiesCount();
Debug.Print("Number
of bodies: " + nbrBodies);
if
((nbrBodies < 1))
{
MessageBox.Show("No
bodies in selected view.");
return;
}
arrBody
= (object[])swView.Bodies;
for
(i = 0; i < arrBody.Length; i++)
{
swBody
= (Body2)arrBody[i];
swSelData
= (SelectData)swSelMgr.CreateSelectData();
swSelData.View = swView;
status
= swBody.Select2(false, swSelData);
//
Object type 76 is a solid body
objType
= swSelMgr.GetSelectedObjectType3(1,
-1);
if
((objType == 76))
{
Debug.Print("
Object type: solid body");
}
if
((!((int)swSelectType_e.swSelSOLIDBODIES == swSelMgr.GetSelectedObjectType3(1,
-1))))
{
MessageBox.Show("Solid
body not found.");
}
swFace
= (Face2)swBody.GetFirstFace();
while
((swFace != null))
{
swEnt
= (Entity)swFace;
//
Select using IEntity
status
= swEnt.Select4(true, swSelData);
Debug.Assert(status);
swFace
= (Face2)swFace.GetNextFace();
}
Debug.Print("
Name of body: " + swBody.GetSelectionId());
}
System.Diagnostics.Debugger.Break();
swModel.ClearSelection2(true);
//
Get the bodies from referenced model
swModel
= (ModelDoc2)swView.ReferencedDocument;
swPart
= (PartDoc)swModel;
arrBody
= (object[])swPart.GetBodies2((int)swBodyType_e.swSolidBody,
true);
if
((nbrBodies == 1))
{
swView.Bodies = (arrBody);
}
else
{
//
Set the body to include in the drawing view
Bodies[0]
= arrBody[0];
arrBodiesIn[0]
= new DispatchWrapper(Bodies[0]);
swView.Bodies = (arrBodiesIn);
}
swModel.ClearSelection2(true);
}
///
<summary>
///
The SldWorks swApp variable is pre-assigned for you.
///
</summary>
public
SldWorks swApp;
}
}