DriveWorks Pro 18: Set Annotation Positions [send feedback...]

Set Annotation Positions

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

We recommend applying this task in Post-Drive Tasks, Generation Sequence.

This ensures all views are resized and positioned before the Annotations are driven.

Properties

Property NameDescription
(Name)The unique name for this task.
Annotation PositionsA table of annotation positions. Columns must be: Sheet or View Name, Annotation Name, Axis, X Value and Y Value (in that order).

Example Annotation Positions Table

As the table will mostly be dynamic we recommend using a Calculation Table.

Sheet or View NameAnnotation NameAxisX ValueY Value
Drawing View1@Sheet1RD1@Drawing View1@<DrawingName>.DrawingYOnly0115
Drawing View1@Sheet1RD2@Drawing View1@<DrawingName>.DrawingXOnly-200
Sheet2DetailItem126Both5050
Drawing View3@Sheet2D1@Distance1@<AssemblyName>.AssemblyYOnly0115
Drawing View3@Sheet2D1@Sketch1@<PartName>.PartXOnly-200
Section View A-A@Sheet2RD3@Drawing View5@<DrawingName>.DrawingXOnly-100

Sheet or View Name

When an annotation is attached to a view the format is:

<ViewName>@<SheetName>

For Detail or Section Views the <ViewName> is the name displayed in the SOLIDWORKS Feature Manager. (These views are given a different name when capturing a Reference Dimension attached to the view.)

When an annotation is on the sheet (not attached to a view) the format is:

<SheetName>

Annotation Name

When an annotation is a Model Dimension from an Assembly the format is:

<Annotation Reference>@<Feature Reference>@<AssemblyName>.Assembly

When an annotation is a Model Dimension from a Part the format is:

<Annotation Reference>@<Feature Reference>@<PartName>.Part

When an annotation is a Reference Dimension attached to a view the format is:

<Annotation Reference>@<ViewName>@<DrawingName>.Drawing

When an annotation is a Reference Dimension attached to a sheet the format is:

<Annotation Reference>

How To Find The Annotation Name

To find the Annotation Name 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.

Positioning The Annotation

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.

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