C# SolidWorks 二次开发 API — 对象关系
参考老外的api网站,简单的弄了个,也当是自己再了解了解.
标签： 二次开发
C# SolidWorks 二次开发 API —dll插件如何让 winform 类似ShowDialog，但还能操作solidworks
C# SolidWorks 二次开发 API —dll插件如何让 winform 类似ShowDialog，但还能操作solidworks
这篇文章记录一下，这次看api帮助解决到的一个问题：
由于之前我都是先做好的exe独立开发，后来改成插件形式后遇到的问题。以前经常利用窗体的ShowDialog特性，让程序暂停，让用户进行对象的自定义选择操作，但是到了dll中出现了问题，因为dll和solidworks主进程是一个，所以当用了页面的ShowDialog之后，solidworks就再也无法操作了。这个问题之前花了一天多时间都没搞定，想了好多办法，最后利用的doevents解决的，但是效果不是特别好。
原来solidworks的帮助文件中已经有了解决方案： 只需要使用 Application.Run(winform)就可以了，我刚才进行了测试，很好用，至于还有没有别的问题，后面再测试一下。
参考链接：
posted @
2020-02-22 18:12
painezeng 阅读(
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C# SolidWorks 二次开发 API — 2018版 中文-完整版共享
C# SolidWorks 二次开发 API — 2018版 中文-完整版共享
由于还在湖北老家，暂时无法回去工作，休息期间我又把2018的api帮助文档看了一下，我把之前翻译的文件免费共享下，希望能对大家有所帮助。
https://download.csdn.net/download/zengqh0314/12170828
posted @
2020-02-19 12:56
painezeng 阅读(
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C# SolidWorks 二次开发 API — 实例：随机上色
C# SolidWorks 二次开发 API — 实例：随机上色
随机上色这个功能做起来不算复杂，但是要想做的比较完美也不简单。
这一篇文章我就只做随机给装配体中的零件上色。
上色前：
上色后：
简单的代码：
private void btn_setcolor_Click(object sender, EventArgs e)
{
ISldWorks swApp = Utility.ConnectToSolidWorks();
if (swApp != null)
{
ModelDoc2 swModel = (ModelDoc2)swApp.ActiveDoc;
Configuration swConf = swModel.GetActiveConfiguration();
Component2 swRootComp = swConf.GetRootComponent();
//遍历
Utility.TraverseCompXform(swRootComp, 0, true);
swModel.WindowRedraw();
swModel.EditRebuild3();
}
}
以下是上色代码：
//如果要设定颜色
if (setcolor == true)
{
double[] matPropVals = swModel.MaterialPropertyValues;
var tempC = GetRadomColor(System.IO.Path.GetFileNameWithoutExtension(swModel.GetPathName()));
matPropVals[0] = Convert.ToDouble(tempC.R) / 255;
matPropVals[1] = Convert.ToDouble(tempC.G) / 255;
matPropVals[2] = Convert.ToDouble(tempC.B) / 255;
swModel.MaterialPropertyValues = matPropVals;
swModel.WindowRedraw();
}
public static System.Drawing.Color GetRadomColor(string name)
{
Random rnd = new Random();
//这里可以根据需要指定颜色。
if (name.Contains("m1"))
{
return System.Drawing.Color.Red;
}
return System.Drawing.Color.FromArgb(
rnd.Next(0, 255), /*红色*/
rnd.Next(0, 255), /*绿色*/
rnd.Next(0, 255) /*蓝色*/ );
}具体代码见github或者码云，链接可以在之前的博文中找到。
posted @
2020-01-14 15:58
painezeng 阅读(
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C# SolidWorks 二次开发 API — 插入图块和属性块
C# SolidWorks 二次开发 API — 插入图块和属性块
在还没有取消所有2D图纸时，我们难免需要在图纸中插入一些标准图块，或者像AutoCAD那个的属性块。
如下图：
直接上代码：
private void btn_Insert_Block_Click(object sender, EventArgs e)
{
//连接到Solidworks
ISldWorks swApp = Utility.ConnectToSolidWorks();
ModelDoc2 swModel = (ModelDoc2)swApp.ActiveDoc;
DrawingDoc dc = (DrawingDoc)swModel;
// SelectionMgr selectionMgr = (SelectionMgr)swModel.SelectionManager;
double[] nPt = new double[3];
nPt[0] = 0;
nPt[1] = 0;
nPt[2] = 0;
MathUtility swMathUtil = swApp.GetMathUtility();
MathPoint swMathPoint = swMathUtil.CreatePoint(nPt);
double blockScale = 1;
string blockPath = @"D:\09_Study\CSharpAndSolidWorks\CSharpAndSolidWorks\TemplateModel\TestBlock.SLDBLK";
//插入图块
var swBlockInst = InsertBlockReturnInst(swApp, swModel, swMathPoint, blockPath, blockScale);
// swModel.SketchManager.MakeSketchBlockFromFile(mathPoint, blockPath, false, blockScale, 0);
//修改块的属性(如果只是普通的图块，则无需要这一步。直接使用上面的一行插入图块即可)
swBlockInst.SetAttributeValue("Title1", "Paine");
}
/// <summary>
/// 插入并返回最后一个图块实例
/// </summary>
/// <param name="sldWorks"></param>
/// <param name="modelDoc2"></param>
/// <param name="mathPoint"></param>
/// <param name="blockPath"></param>
/// <param name="blockScale"></param>
/// <returns></returns>
private SketchBlockInstance InsertBlockReturnInst(ISldWorks sldWorks, ModelDoc2 modelDoc2, MathPoint mathPoint, String blockPath, double blockScale)
{
SketchBlockInstance swBlockInst;
List<String> NowBlockName = new List<String>();
var swModel = modelDoc2;
Boolean boolstatus = swModel.Extension.SelectByID2(System.IO.Path.GetFileNameWithoutExtension(blockPath), "SUBSKETCHDEF", 0, 0, 0, false, 0, null, 0);
if (boolstatus == true)
{
Feature swFeat = swModel.SelectionManager.GetSelectedObject6(1, 0);
var swSketchBlockDef = swFeat.GetSpecificFeature2();
var nbrBlockInst = swSketchBlockDef.GetInstanceCount;
if (nbrBlockInst > 0)
{
var vBlockInst = swSketchBlockDef.GetInstances();
for (int i = 0; i < nbrBlockInst; i++)
{
swBlockInst = vBlockInst[i];
NowBlockName.Add(swBlockInst.Name.ToString());
}
swModel.SketchManager.MakeSketchBlockFromFile(mathPoint, blockPath, false, blockScale, 0);
swModel.ClearSelection2(true);
boolstatus = swModel.Extension.SelectByID2(System.IO.Path.GetFileNameWithoutExtension(blockPath), "SUBSKETCHDEF", 0, 0, 0, false, 0, null, 0);
swFeat = swModel.SelectionManager.GetSelectedObject6(1, 0);
swSketchBlockDef = swFeat.GetSpecificFeature2();
nbrBlockInst = swSketchBlockDef.GetInstanceCount;
if (nbrBlockInst > 0)
{
vBlockInst = swSketchBlockDef.GetInstances();
for (int j = 0; j < nbrBlockInst; j++)
{
swBlockInst = vBlockInst[j];
if (!NowBlockName.Contains(swBlockInst.Name.ToString()))
{
swModel.Extension.SelectByID2(swBlockInst.Name, "SUBSKETCHINST", 0, 0, 0, false, 0, null, 0);
swBlockInst = GetSketchBlockInstanceFromSelection();
return swBlockInst;
}
}
}
return null;
}
else
{
return null;
}
}
else
{
var swSketchBlockDef = swModel.SketchManager.MakeSketchBlockFromFile(mathPoint, blockPath, false, blockScale, 0);
swBlockInst = swSketchBlockDef.GetInstances()[0];
return swBlockInst;
}
}
private SketchBlockInstance GetSketchBlockInstanceFromSelection()
{
ISldWorks swApp = Utility.ConnectToSolidWorks();
ModelDoc2 swModel;
ModelDocExtension swModelDocExt;
SketchBlockInstance SketchBlockInstance;
DateTime time = DateTime.Now;
try
{
swModel = swApp.ActiveDoc;
swModelDocExt = swModel.Extension;
SelectionMgr swSelectionMgr;
swSelectionMgr = swModel.SelectionManager;
string SelectByString = "";
string ObjectType = "";
int type;
double x;
double y;
double z;
if (swSelectionMgr.GetSelectedObjectCount2(-1) > 1)
{
// Return only a SketchblockInstance when only one is selected...
// modify if you want return more than one (or only the first) selected Sketchblockinstance
return null;
}
swSelectionMgr.GetSelectionSpecification(1, out SelectByString, out ObjectType, out type, out x, out y, out z);
Debug.WriteLine(SelectByString + " " + ObjectType + " " + type);
if (type == (int)swSelectType_e.swSelSUBSKETCHINST)
{
SketchBlockInstance = swSelectionMgr.GetSelectedObject6(1, -1);
Debug.WriteLine("Found:" + SketchBlockInstance.Name);
return SketchBlockInstance;
}
else if (type == (int)swSelectType_e.swSelSKETCHSEGS | type == (int)swSelectType_e.swSelSKETCHPOINTS)
{
// Show if a sketchblockinstance has the same name
SketchManager SwSketchMgr;
SwSketchMgr = swModel.SketchManager;
object[] blockDefinitions = (object[])SwSketchMgr.GetSketchBlockDefinitions();
foreach (SketchBlockDefinition blockDef in blockDefinitions)
{
foreach (SketchBlockInstance blockInstance in blockDef.GetInstances())
{
if (SelectByString.EndsWith(blockInstance.Name))
{
Debug.WriteLine("Found:" + blockInstance.Name);
return blockInstance;
}
}
}
}
else
{
return null;
}
}
catch (Exception ex)
{
}
finally
{
Debug.WriteLine(DateTime.Now.Subtract(time).Milliseconds);
}
return null;
}
posted @
2020-01-06 13:30
painezeng 阅读(
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C# SolidWorks 二次开发 API — 把零件中的坐标点转换到总装配中
C# SolidWorks 二次开发 API — 把零件中的坐标点转换到总装配中
今天我们来看下solidworks中的坐标矩阵转换，这个例子是把子零件中的一个基准轴的两个端点读出来，并转换到总装配的坐标系中，得到在总装配体坐标系的位置，可以进一步判断轴的真实安装方向。
直接上代码：
private void btn_Transform_PartToAsm_Click(object sender, EventArgs e)
{
//连接到Solidworks
//这个例子是把零件中的一个基准轴 的两个点的坐标转换到装配体中
//请打开装配体，并在某个零件下选择一下基准轴
ISldWorks swApp = Utility.ConnectToSolidWorks();
ModelDoc2 swModel = (ModelDoc2)swApp.ActiveDoc;
SelectionMgr swSelMgr = swModel.ISelectionManager;
Feature swFeat = (Feature)swSelMgr.GetSelectedObject6(1, 0);
String sAxisName = swFeat.Name;
RefAxis RefAxis = swFeat.GetSpecificFeature2();
var vParam = RefAxis.GetRefAxisParams();
Component2 inletPart = swSelMgr.GetSelectedObjectsComponent4(1, 0);
double[] nPt = new double[3];
double[] nPt2 = new double[3];
object vPt;
object vPt2;
nPt[0] = vParam[0]; nPt[1] = vParam[1]; nPt[2] = vParam[2];
nPt2[0] = vParam[3]; nPt2[1] = vParam[4]; nPt2[2] = vParam[5];
vPt = nPt;
vPt2 = nPt2;
MathUtility swMathUtil = (MathUtility)swApp.GetMathUtility();
MathTransform mathTransform = inletPart.Transform2;
MathTransform swXform = (MathTransform)mathTransform;
MathPoint swMathPt = (MathPoint)swMathUtil.CreatePoint((vPt));
MathPoint swMathPt2 = (MathPoint)swMathUtil.CreatePoint((vPt2));
//swXform.Inverse(); 反转的话就是把装配体中的点坐标转到零件对应的坐标系统中
swMathPt = (MathPoint)swMathPt.MultiplyTransform(swXform);
swMathPt2 = (MathPoint)swMathPt2.MultiplyTransform(swXform);
var x = swMathPt.ArrayData[0];
var y = swMathPt.ArrayData[1];
var z = swMathPt.ArrayData[2];
var x2 = swMathPt2.ArrayData[0];
var y2 = swMathPt2.ArrayData[1];
var z2 = swMathPt2.ArrayData[2];
var v1 = x2 - x;
var v2 = y2 - y;
var v3 = z2 - z;
if (Math.Round(v3, 4) != 0 && Math.Round(v1, 4) == 0 && Math.Round(v2, 4) == 0)
{
MessageBox.Show("此轴在Z方向上");
}
}比较全的关于矩阵转换的一篇文章：
posted @
2019-12-31 10:12
painezeng 阅读(
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