DriveWorks Pro 16: Delete Annotation from Drawing [send feedback...]

Delete Annotation From Drawing - SOLIDWORKS PowerPack

The Delete Annotation from Drawing Generation Task will delete a given annotation from the given View or Sheet.

Properties

Property NameDescription
(Name)The unique name for this task.
Annotation NameThe name of the annotation.
Sheet or View NameThe name of the sheet or view.

Examples

The following table shows examples of the ‘Annotation Name’ and ‘Sheet or View Name’ Properties for a range of possible SOLIDWORKS Drawing Annotations.

TypeSOLIDWORKS Address StyleDriveWorks 'Annotation Name' PropertyDriveWorks 'Sheet or View Name' Property
Model Dimension (1)D1@Sketch1@PartName.PartD1@Sketch1@{Model File Name Result}.PartDrawing View1@Sheet1
Reference Dimension (Model)RD1@Annotations@PartName.PartRD1@Annotations@{Model File Name Result}.PartDrawing View1@Sheet1
Reference Dimension (Drawing)RD1@Drawing View1@DrawingName.DrawingRD1@Drawing View1@{Drawing File Name Result}.DrawingDrawing View1@Sheet1
BalloonDetailItem120DetailItem120Drawing View1@Sheet1
Balloon on a Magnetic LineDetailItem120DetailItem120Drawing View1@Sheet1
Note (Attached to View)DetailItem140DetailItem140Drawing View1@Sheet1
Note (Not Attached to View)DetailItem140DetailItem140Sheet1
Note (Model)DetailItem140DetailItem140Drawing View1@Sheet1
Weld Symbol (Drawing)DetailItem150DetailItem150Drawing View1@Sheet1
Weld Symbol (Model)DetailItem150DetailItem150Drawing View1@Sheet1
Hole Callout (Drawing)RD1@Drawing View1@DrawingName.DrawingRD1@Drawing View1@{Drawing File Name Result}.DrawingDrawing View1@Sheet1
Geometric Tolerance (Drawing)DetailItem160DetailItem160Drawing View1@Sheet1
Geometric Tolerance (Model)DetailItem160DetailItem160Drawing View1@Sheet1
Datum Feature (Drawing)DetailItem170DetailItem170Drawing View1@Sheet1
Datum Feature (Model)DetailItem170DetailItem170Drawing View1@Sheet1
Surface Finish (Drawing)DetailItem180DetailItem180Drawing View1@Sheet1
Surface Finish (Model)DetailItem180DetailItem180Drawing View1@Sheet1
Datum Target (Drawing)DetailItem190DetailItem190Drawing View1@Sheet1
Datum Target (Model)DetailItem190DetailItem190Drawing View1@Sheet1
Revision SymbolDetailItem200DetailItem200Drawing View1@Sheet1
Location LabelDetailItem210DetailItem210Drawing View1@Sheet1

The SOLIDWORKS Address Style for Model Dimensions linked to Assemblies will take the form D1@Distance1@AssemblyName.Assembly.

The PartName or AssemblyName in this address refers to the file name of the part or subassembly that contains the Model Dimension.

When Annotations are linked to a section or detail view you will need to use the Section or Detail View Name E.g. Section View A-A (not the drawing view name in the SOLIDWORKS Address)

The above examples of the ‘Annotation Name’ and ‘Sheet or View Name’ Properties will work for single sheet or multi sheet SOLIDWORKS Drawings.

Determine The Annotation Name

To find out the Name of an Annotation you can use the DriveWorks Capture Pane inside SOLIDWORKS;

  1. Open the captured Master Drawing file in SOLIDWORKS
  2. Switch to the ‘Annotation Text’ tab of the DriveWorks Task Pane
  3. Select the Annotation you want to Delete
  4. The dimension address will appear in the ‘Address’ field of the DriveWorks Task Pane
  5. You can copy and paste this into DriveWorks for use in rules

You do not need to Capture the Annotation to use the Delete Annotation from Drawing Generation Task

The Annotation Name Property can also end in .Assembly (if the Annotation is an Assembly dimension, such as a Distance Mate value) or .Drawing (if the annotation is a Reference Dimension).

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