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.
| Property Name | Description |
|---|---|
| (Name) | The unique name for this task. |
| Annotation Positions | A table of annotation positions. Columns must be: Sheet or View Name, Annotation Name, Axis, X Value and Y Value (in that order). |
As the table will mostly be dynamic we recommend using a Calculation Table.
| Sheet or View Name | Annotation Name | Axis | X Value | Y Value |
|---|---|---|---|---|
| Drawing View1@Sheet1 | RD1@Drawing View1@<DrawingName>.Drawing | YOnly | 0 | 115 |
| Drawing View1@Sheet1 | RD2@Drawing View1@<DrawingName>.Drawing | XOnly | -20 | 0 |
| Sheet2 | DetailItem126 | Both | 50 | 50 |
| Drawing View3@Sheet2 | D1@Distance1@<AssemblyName>.Assembly | YOnly | 0 | 115 |
| Drawing View3@Sheet2 | D1@Sketch1@<PartName>.Part | XOnly | -20 | 0 |
| Section View A-A@Sheet2 | RD3@Drawing View5@<DrawingName>.Drawing | XOnly | -10 | 0 |
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>
To find the Annotation Name you can use the DriveWorks Capture Pane inside SOLIDWORKS:
You do not need to Capture the Annotation to use the Set Annotation Position Generation Task.
The Axis property determines which of the X Value and Y Value properties are used to position the Annotation.
| Property Value | Result |
|---|---|
| Both | Will use both the X Value and the Y Value properties to position the Annotation. |
| XOnly | Will ignore the Y Value property and will only position the Annotation in the X Axis. |
| YOnly | Will 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.