DriveWorks Pro 15: Set Annotation Position [send feedback...]

Set Annotation Position

The Set Annotation Position Generation Task sets the XY position of an annotation.

Properties

Property NameDescription
(Name)The unique name for this task.
Annotation NameThe name of the annotation to position.
AxisSpecifies which axis to drive the annotation along. For example, specifying XOnly will only position the annotation along the X-axis and maintain the annotation's current Y position.
Sheet or View NameThe name of the sheet (or view) the annotation belongs to.
X ValueThe new position of the annotation along the X axis (expressed as a percentage).
Y ValueThe new position of the annotation along the Y axis (expressed as a percentage).

Example Property Values

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

(1) 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.

To find out the ‘Annotation 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 position
  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 Set Annotation Position 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).

Creating Rules for the Annotation Name Property

The Part names in the Annotation Name Property need to be the final generated models file names, not the Master file names.

For example:

By default, DriveWorks gives each model the File Name Rule DWSpecification meaning that your models will generate with the following naming structure;

MasterName ProjectName 9999.SLDPRT

This means the Rule for the Annotation Name property would be;

"D1@Sketch1@MasterName " & DWSpecification &".Part"

The following are two further examples of potential Annotation Name property rules in combination with the related Model File Name Rules:

Example 1

Model File Name Rule => "*PartName-" & OrderNumberReturn

Annotation Name Property Rule => "D1@Sketch1@PartName-" & OrderNumberReturn &".Part"

Example 2

Model File Name Rule => "*" & DWSpecificationId & "*"

Annotation Name Property Rule => "D1@Sketch1@" & DWSpecificationId & " MasterName.Part"

For more information on Model File Name Rules: Concept: File Naming

Annotation Name Property Accepted Values

The following is a description of DriveWorks behaviour for each ‘Annotation Name’ Property value possibility.

Example 1

Annotation Name Property Rule Result = D1@Sketch1@{Model File Name Result}.Part

DriveWorks will use the full result to select the required Annotation.

Example 2

Annotation Name Property Rule Result = DetailItem110

DriveWorks will use the full result to select the required Annotation.

Example 3

Annotation Name Property Rule Result = RD1

DriveWorks will compare this with the name component of the address to select the required Annotation.

Example 4

Annotation Name Property Rule Result = RD1@Drawing View1@{Drawing File Name Result}.Drawing

DriveWorks will use the full result to select the required Annotation.

Positioning The Annotation

Once you have defined which Annotation you wish to position, you will need to define where to position the Annotation on the generated Drawing. You define this using the ‘X Value’ and the ‘Y Value’ properties.

The ‘Axis’ property determines which of the ‘X Value’ and ‘Y Value’ properties are used to position the Annotation.

Property ValueResult
BothWill use both the ‘X Value’ and the ‘Y Value’ properties to position the Annotation
XOnlyWill ignore the ‘Y Value’ property and will only position the Annotation in the X Axis
YOnlyWill ignore the ‘X Value’ property and will only position the Annotation in the Y Axis

The ‘X Value’ and ‘Y Value’ are expressed as percentages. For example, X Value = 50, this will position the Annotation half way along the Drawing View or Sheet.

The ‘X Value’ and ‘Y Value’ properties accept negative values and values greater than 100.

If an Annotation is not attached to a Drawing View, the ‘X Value’ and ‘Y Value’ are in relation to the entire sheet.

If an Annotation is attached to a Drawing View the ‘X Value’ and ‘Y Value’ are in relation to the Bounding box of the Drawing View.

X Value = 0, Y Value = 0, is the bottom left hand corner of the Sheet or View.

Set Annotation Position works best when placed in Post-Drive Tasks. All views will have been resized and repositioned before the Annotations are positioned.

There is a Tech Tip example Project that can be downloaded from the Tech Tip Portal on the DriveWorks Community Website.

This Tech Tip can be used as a reference for using the Set Annotation Position Generation Task.

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