It is quite possible to create a blank part and drawing sheet with one click of a button. Yes, you are right, this can be done with the journal. This journal below is written in C sharp programming language.
Exactly how you either select a pre-defined template or custom apply a few settings on top of the existing template, the same can be done with writing a code inside the journal.
For example, part units, here millimeters units is applied. Template file name blank, this means no pre-defined template is used.
In NX Open, objects like features, geometries, and even drawing sheets are created using builder objects. These are nothing but create functions, also called factory objects.
using System;
using NXOpen;
public class blank_part_w_drawing_sheet
{
public static void Main(string[] args)
{
Session theSession = Session.GetSession();
FileNew objNewFile;
objNewFile = theSession.Parts.FileNew();
objNewFile.TemplateFileName = "Blank";
objNewFile.Application = FileNewApplication.Gateway;
objNewFile.Units = NXOpen.Part.Units.Millimeters;
objNewFile.NewFileName = @"C:\temp\test.prt";
objNewFile.UseBlankTemplate = true;
objNewFile.MakeDisplayedPart = true;
NXObject objNX1 = objNewFile.Commit();
objNewFile.Destroy();
Part workPart = theSession.Parts.Work;
Part displayPart = theSession.Parts.Display;
NXOpen.Drawings.DrawingSheet nullDrawings_DrawingSheet = null;
NXOpen.Drawings.DrawingSheetBuilder objDrawingSheetBuilder;
objDrawingSheetBuilder = workPart.DrawingSheets.DrawingSheetBuilder(nullDrawings_DrawingSheet);
objDrawingSheetBuilder.Option = NXOpen.Drawings.DrawingSheetBuilder.SheetOption.StandardSize;
objDrawingSheetBuilder.Units = NXOpen.Drawings.DrawingSheetBuilder.SheetUnits.Metric;
objDrawingSheetBuilder.StandardMetricScale = NXOpen.Drawings.DrawingSheetBuilder.SheetStandardMetricScale.S11;
objDrawingSheetBuilder.Height = 210.0;
objDrawingSheetBuilder.Length = 297.0;
objDrawingSheetBuilder.ProjectionAngle = NXOpen.Drawings.DrawingSheetBuilder.SheetProjectionAngle.First;
NXObject objNX2 = objDrawingSheetBuilder.Commit();
objDrawingSheetBuilder.Destroy();
// Application Switch will be performed AFTER program ends, see Docs.
UI.GetUI().MenuBarManager.ApplicationSwitchRequest("UG_APP_DRAFTING");
// Part is saved but Application is NOT Drafting yet!
displayPart.Save(BasePart.SaveComponents.False, BasePart.CloseAfterSave.False);
}
public static int GetUnloadOption(string dummy)
{
return (int)Session.LibraryUnloadOption.Immediately;
}
}
In this example, DrawingSheetBuilder is used to create a drawing sheet.
This builder is part of Drawings namespace. There are several things can be defined inside this builder, for example, sheet size (width and height), metric units, sheet scale, project angle (first angle method or third angle method).
ApplicationSwitchRequest which is UI function, can set the drafting application in newly created part.
You can simply copy the above code and get inside your NX CAD software to run it. You can even try doing small tweaks with little knowledge of C sharp programming.
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