How to add Sheet metal Properties to Drawings
How to add Sheet Metal Properties to Drawings
SOLIDWORKS Sheet Metal Properties can be added to Drawings using a predefined annotation or selectively using standard annotation property mapping syntax.
The secret is the annotation MUST be attached to the Flat Pattern view. Right-click inside the border of a drawing’s Flat Pattern view and then select Annotation > Cut List Properties. Finally, place the predefined annotation on the drawing.
The predefined annotation can then be edited by right-clicking the annotation and then selecting the option ‘Edit Text in Window’.
The property units are linked to drawing’s document properties in Tools > Options > Document Properties > Units, Length (Decimals).
To create your own custom annotations mapped to specific Sheet Metal Properties, create an annotation within the Flat Pattern view’s border, and then add the property names accordingly. For example, to map the outer cut length, create an annotation and enter the text $PRPWLD:”Cutting Length-Outer“
To speed up the process, you can copy and paste properties from the list below:
$PRPWLD:”Bounding Box Length”
$PRPWLD:”Bounding Box Width”
$PRPWLD:”Sheet Metal Thickness”
$PRPWLD:”Bounding Box Area”
$PRPWLD:”Bounding Box Area-Blank”
$PRPWLD:”Cutting Length-Outer”
$PRPWLD:”Cutting Length-Inner”
$PRPWLD:”Cut Outs”
$PRPWLD:”Bends”
$PRPWLD:”Bend Allowance”
$PRPWLD:”MATERIAL”
$PRPWLD:”Mass”
$PRPWLD:”Description”
$PRPWLD:”Bend Radius”
$PRPWLD:”Surface Treatment”
$PRPWLD:”Cost-TotalCost”
$PRPWLD:”QUANTITY”
A final note on this topic, you may consider adding any customized annotations to your design library to easily drag and drop the annotation from the design library onto other drawings. To add an annotation to the design library, simply right-click the annotation and then select ‘Add to Library’ from the menu.