I have created a title block that my company uses. I am trying to create attributes that I can change to suit my needs when I put information into the title block. How can I go about doing that?
There may be a better way to do this, but one way I can think of is to create some custom properties in the properties of the title block (File -> Properties) then you can use notes that have a custom link to each property and they will update when you change their value in the properties.
Robert, there are several Solidworks features for populating border information without having to manually edit text entities. Their respective usefulness is determined by the circumstances under which you wish to populate the data.
For border attributes like scale, sheet number, title and date information, it's best to let custom properties capture that information. If you're from an AutoCAD background, custom properties are similar to the Field Codes that were introduced in 2005.
Custom properties are document or configuration level metadata that are accessed through special codes that you include in annotations.
For example: including the text $PRSHEET:"Description" in a drawing note will retrieve from the model specified in Sheet Properties the description and display it in the note. $PRP:"SW-Total Sheets" will retrieve the sheet count for the drawing in which the annotation is placed.
You can populate custom properties from the File==>Properties Document information dialog box.
You can also create a custom property panel, which is a form that displays in the task manager area similar to the Attribute Edit Dialog box in AutoCAD. Entering values in the fields of the form will populate the custom properties of the current or selected model or drawing.
You can also create a title-block to modify static text or custom properties in your sheet format. This doesn't really have an equivalent in AutoCAD. Basically for each sheet, you can define a selection of annotation objects in the sheet format that are editable from the sheet. The user, double-clicks inside the title-block area of the border and the editable text objects highlight. Picking on one of them allows you to change the text value but not the location or other attributes. If the annotation is linked to a custom property, editing the text value this way will update that custom property. You can't use this with automatic properties like part mass or drawing sheet name.
If you're looking for something closer to the functionality of AutoCAD blocks with attributes, you can create a sketch block from a selection set of sketch entities in your drawing and like AutoCAD, you can specify an insertion point and designate the locations and text characteristics of editable attributes. There's no special entity type for an attribute in SolidWorks and the workflow is a little bit different to. What you do is create the block containing the annotations and sketch entities that you want and then edit the block definition and for the notes that you don't want to be editable attributes, you check the 'read only' checkbox:
When you exit out of the block editor, use the 'edit attributes' button in the property manager to display a form listing your available attributes. You can edit their values and add prompts to this form.
You can also edit the attributes by double-clicking on them-just like you can in AutoCAD. You can reposition an attribute without editing it's parent block definition, but the rest is pretty much the same. You can save the block to your design library and drag-n-drop it into your drawing. You can include custom properties in the annotations of blocks that will populate from the metadata stored in your drawings and models. If you export your drawing to AutoCAD, the block will export as an AutoCAD block insertion complete with attributes. I experimented with this back in 2006 when our engineering department insisted on finishing drawings in AutoCAD.
SolidWorks outfits don't typically use sketch blocks for border data, though. It's usually redundant to the functionality of the sheet format and not nearly as flexible.
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