SolidWorks Tips and Tricks
Automatically Fill in Your Title Block
Every time that you create a drawing document, you need to fill in the title block, including your name and the date that you created it. However, it gets repetitive if you have to do this every time. SolidWorks provides you the ability to do this automatically whenever you start a new drawing document. Let’s see how to automatically fill in the drawn by and created date information.
Open a new drawing document. Note that you’ll need to do this for each of the different sheet formats that you use. For this tip, in the Sheet Format/Size dialog box, make sure that the Standard sheet size radio button is selected and pick A – Landscape from the menu. Right below the menu is the name of the template, a – landscape.slddrt. If it’s not, browse to that file. Make sure that Display sheet format is checked and click OK.
In the Model View PropertyManager, click the Cancel button. You should see a blank piece of paper with a border and title block.
Pull down the “File” menu and pick Properties. In the Summary Information dialog box, on the Custom tab, click in the box below Property Name and pull down the “Property Name” menu and pick DrawnBy. Click in the Value / Text Expression box and type your initials. Note that what you type is exactly what will appear in the title block. Click OK.
Note that your initials are automatically placed in the title block, the bottom right of your drawing.
Now, to automatically fill in the date, right click on the sheet and pick Edit Sheet Format. As you may notice, the lines turn blue and a few custom properties of parts or assemblies are already linked to fields in the system sheet formats. That’s what the $PRPSHEET means. Place the cursor in the middle of the Drawn/Date box where the date should appear. When the $PRP:“DrawnDate” flyout appears, click the left mouse button as shown below. A little green box will appear where you click.
In the Note PropertyManager, under Text Format, click the Link to Property button.
In the Link to Property dialog box, pick the Current document radio button. Then, pull down the menu and pick SW-Created Date. Below that, pull down the menu and pick Short Date. Uncheck the Show Time check box. This will place the current date in to the title block of your drawing. If you wanted the date the model was created in your drawing, pick the Model in view specified in sheet properties radio button. Finally, click OK to close the dialog box.
You should now see the current date in your title block. Right click on the date and pick Edit Text in Window. (For SolidWorks 2007 and before, right click on the date and pick Properties). Delete $PRP:”DrawnDate” as shown below and click OK.
Press the Escape key and then right click on the sheet and pick Edit Sheet. The lines on the title block turn gray, indicating that the drawing sheet is now active. Remember that SW-Created Date is static. In other words, when you create a new drawing document, the current date will be inserted. But thereafter, when you reopen any of your saved drawing documents, the date remains the date the document was created, not changing to the current date.
To make this work for future drawing documents, you’ll have to save it. You can replace the existing sheet format or save it as a new one. To do this, pull down the “File” menu and pick Save Sheet Format. In the Save Sheet Format dialog box, under File name, rename the file to ‘a – landscape_date.slddrt‘ and click Save. Finally, open a new drawing document. In the Sheet Format/Size dialog box, pick a – landscape_date from the list of available sheet formats, as shown below. Click OK.
In the Model View PropertyManager, click the Cancel button. In you title block, you should see that your initials and the created date are already filled in for you. So, every time that you use this new customized sheet format, you don’t have to worry about filling out your name and the date the drawing was created. SolidWorks automatically does it for you. Look around the title block for other fields that you may want to have filled in automatically.
Customizing SolidWorks For Greater Productivity shows you how to format and create your own linked notes, how to set the detailing options and layers, and how to save the custom template for future use. By creating a custom drawing format, you can set up things once and then not have to worry about them ever again.
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