Solidworks二次开发-05-装配体中插入零部件

Solidworks二次开发--装配体中插入零部件

在往装配体中插入零部件时,我们使用 addcomponent 函数。如果需要选定零部件的配置,则需要使用 addcomponent4 。

先学习下语法:

addcomponent4 :

** retval = AssemblyDoc.AddComponent4 ( compName, configName, x, y, z)

**

Input: (BSTR) compName Path name of a loaded part or assembly to add as a component

Input: (BSTR) configName Name of the configuration from which to load the component

Input: (double) x X coordinate of the component center

Input: (double) y Y coordinate of the component center

Input: (double) z Z coordinate of the component center

Output: (LPCOMPONENT2) retval Pointer to the Component2 object

需要注意的是:参数 1 为文件的全名(包括路径);参数 2 为文件的配置名称;当函数执行成功购返回一个指向该零件的指针。

于是我们可以如下写一个小程序,用来给装配体中插零件:

‘filename:insertPart.swp

‘write by arden 2005-4-4

‘this function add a part called “ 零件 1.SLDPRT” in CurrentWorkingDirectory

‘precondition is there has a part document called “ 零件 1.SLDPRT” in CurrentWorkingDirectory

‘and it has a configuration called “ 配置 1”

Dim swApp As SldWorks.SldWorks

Dim Model As ModelDoc2

Dim pth As String

Dim strpath As String

Sub insertPart()

Set swApp = Application.SldWorks

strpath = swApp.GetCurrentWorkingDirectory ‘ 当前工作路径

Set Model = swApp.ActiveDoc

pth = strpath & " 零件 1.SLDPRT" ‘ 得到文件的 FULLPATH 全名

Model.AddComponent4 pth, " 配置 1", 0, 0, 0 ‘ 添加零部件

End Sub

然而,这个程序比不是想象中那么好用。为什么呢??回头看 addcomponent4 的 remark ,上面这样写:

The specified file must be loaded in memory. A file is loaded into memory when you load the file in your

SolidWorks session ( SldWorks::OpenDoc6 ) or open an assembly that already contains the file.

就是说你想指定的插入的文件必须在调用函数之前已经在内存中加载了。

不习惯,你就不能直接打开多简单,没办法,我还没有找到好的方法,只能按人家的来:

看看下面的函数 Opendoc6 ,它打开一个文档:

Opendoc6 :

** retval = SldWorks.OpenDoc6 ( filename, type, options, configuration, &Errors, &Warnings )

**

Input: (BSTR) Filename Document name or full path if not in current directory, including extension

Input: (long) Type Document type as defined in swDocumentTypes_e

Input: (long) Options Mode in which to open the document as defined in swOpenDocOptions_e

Input: (BSTR) Configuration Model configuration in which to open this document :

Applies to parts and assemblies, not drawings

If this argument is empty or the specified configuration is not present in the model,

the model is opened in the last-used configuration.

Output: (long) Errors Load errors as defined in swFileLoadError_e

Output: (long) Warnings Warnings or extra information generated during the open operation as defined in swFileLoadWarning_e

Return: (LPDISPATCH) retval Pointer to a Dispatch object, the newly loaded ModelDoc2 , or NULL if failed to open

这个函数参数 1 就是文档的全名,参数 2 是要插入的类型描述,其中 0123 分别表示:

0 swDocNONE :不是 sw 文件

1 swDocPART :零件

2 swDocASSEMBLY :装配体

3 swDocDRAWING :工程图

如果想使用 swDocNONE,需要定义:

Public Enum swDocumentTypes_e

swDocNONE = 0

swDocPART= 1

swDocASSEMBLY = 2

swDocDRAWING=3

End Enum

参数 3 是打开文档的模式,一般我们就选择 swOpenDocOptions_Silent 用 0 表示,当然还有只读、只看等选项

参数 4 是打开选项,一般置空

后面是两个 OutPut ,用来显示错误打开时的提示

函数返回一个指向打开文件的指针。

按照上面的要求我们在向装配体中插入一个零部件时,需要这样步骤:

1 、得到装配体

2 、使用 opendoc6 打开需要插入的零件

3 、使用 addcomponent4 插入零件到装配体

我们上面的程序需要这样来修改一下,添加了一个打开文档的函数:

' ******************************************************************************

' insertpart 03/21/05 by arden

' 插入零件 1

' 前提条件:在装配体所在文件夹中有零件“零件 1 ” 存在,并且零件 1 有配置“配置 1 ”

' ******************************************************************************

Dim swApp As SldWorks.SldWorks

Dim Model As ModelDoc2

Dim YSBmodel As ModelDoc2

Dim pth As String

Dim strpath As String

Dim nErrors As Long

Dim nWarnings As Long

Sub insertpart()

Set swApp = Application.SldWorks

strpath = swApp.GetCurrentWorkingDirectory

Set Model = swApp.ActiveDoc

pth = strpath & " 零件 1.SLDPRT"

openYSB (pth) ‘ 在添加零部件之前,先打开它

Model.AddComponent4 pth, " 配置 1", 0, 0, 0

End Sub

' 这个函数打开零件 1

Sub openpart(ByVal pth As String)

Dim path As String

Dim newswapp As SldWorks.SldWorks

Set newswapp = Application.SldWorks

path = pth

Set YSBmodel = newswapp.OpenDoc6(path, 1, swOpenDocOPtions_Silent, "", nErrors, nWarnings)

YSBmodel.Visible = False ‘ 我不想看到零件 1

End Sub

这样的做法我感觉比较笨 ~ 为了赶工程进度我没有再去寻找好的方法,如果您知道有好的方法请告知我,万分感谢。

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