Adding Custom Properties in Drawings
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.
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.
Add Your Logo to the Drawing
A lot of companies like to have the company logo on their blueprints. The first step is to prepare your company logo. SolidWorks allows you to insert the following image types into a drawing: .bmp, .gif, .jpg, .jpeg, .tif, .wmf, .png, and .psd. Once your logo is ready to go, all you have to do is use the Sketch Picture command on the "Sketch" toolbar to easily insert your image file into a drawing.
To do this, open the drawing that you want to insert your picture in.
Then, pull down the "Insert" menu and pick Picture, or pick Sketch Picture from the "Sketch" toolbar.
In the Open dialog box, browse to an image file, then click Open.
Note that the inserted image is inserted in the lower left corner of the drawing, the (0,0) position. You can just drag and resize the images in the graphics area to any desired location.
In the Sketch Picture PropertyManager, pick the position, size, rotation, and transparency settings of your choice, and then, click the green OK check mark.
Add a Watermark to a Drawing
At times, a watermark such as "CONFIDENTIAL" is required on a drawing print. Unfortunately, SolidWorks does not have a watermark feature. There are a few workarounds that are available, though.
Embed a Microsoft Word Watermark
Right click over the sheet and pick Edit Sheet Format,
Then, pull down the "Insert" menu and pick Object.
In the Insert Object dialog box, under Object Type, pick Microsoft Word Picture, as shown in Figure 2. Then, click OK,
A Word document will open. In the Word document, pull down the "Format" menu and pick Background – Printed Watermark.
To insert a text watermark, click the Text watermark radio button. Then, pick the text you want from the pull down. Note that you can also type in any text that you want, as shown in the Figure. To insert a picture as a watermark, click the Picture Watermark radio button, and then select your picture.
Select any additional options that you want, and then click OK. In the Edit Picture" toolbar, click Close Picture.
Finally, right click over the sheet again and pick Edit Sheet to exit out of the sheet format. Remember that you can use this technique to create the watermark as part of a Drawing Document Template.
Manually Add a Watermark
Right click over the sheet again and pick Edit Sheet to exit out of the sheet format. You watermark is now underneath everything on your drawing. Note that you can save your block for use on multiple drawings or for use on a Drawing Document Template.
Change the Drawing Paper Image in SolidWorks
TIPS AND TRICKS