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.   Adding Custom Properties in Drawings
.   Add Your Logo to the Drawing
.   Add a Watermark to a Drawing
.   Tips and Tricks
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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.
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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.
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Note that your initials are automatically placed in the title block, the bottom right of your drawing.
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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.

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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.
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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.

 

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.


Just double click the image to open the Sketch Picture PropertyManager to make any changes.


If you want your company logo in the background of every drawing, you can insert the picture while in Edit Sheet Format mode and save it as a Drawing Template.

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
To embed a watermark directly from Microsoft Word into the sheet format, begin by opening a drawing.

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.

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Select any additional options that you want, and then click OK. In the Edit Picture" toolbar, click Close Picture.
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The watermark is imported into your drawing. Drag the watermark to place it where you want, as.

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
In a drawing, right click over the sheet and pick Edit Sheet Format. Pull down the "Insert" menu and pick Annotations – Note. Place the note on the drawing where you want the watermark to appear. Set the formatting, including the text angle and text color. Once you set the note the way that you want it, click the green check mark button in the Note PropertyManager. Next, right click on the note and pick Make Block, as shown.

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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
By default, SolidWorks uses a crinkled piece of paper for the sheet background of a new drawing document. The actual image file for the crinkled paper is located at SolidWorks Install Directory/data/Images/drawings/sheetbackground1.bmp. You can replace this bitmap file with something else. Before you do, just make sure to save the original file so that you can change it back at any time. Once you have the original sheetbackground1.bmp file backed up, simple save your new bmp file as sheetbackground1.bmp and place it in the drawings folder. Then, in SolidWorks, pull down the "Tools" menu and pick Options. In the System Options dialog box, pick Colors. In the bottom of the dialog, make sure that Use specified color for drawings paper color is not checked. If this option is checked, the color selected for Drawings, Paper Color will be used instead of the sheetbackground1.bmp file. Open a drawing and check out your new sheet background.


Remember, this is just for looks. In other words, the sheet background image will not print. If you want a picture to print in a drawing, pull down the "Insert" menu and pick Picture. Open the picture of your choice and use the Sketch Picture PropertyManager to adjust the picture.


TIPS AND TRICKS

  • The first component in an assembly is fixed by default. To move it right click on the component and select float.
  • You can crtl drag an assembly component from the feature manager design tree into the graphics window to create another instance of the same component in the assembly.
  • You can use tools, interference detection to make sure components in the assembly don't intersect one another.
  • You can use the view menu to toggle the display of various types of items planes, axis, origins etc.
  • You can specify the line font for many drawing items, including detail view borders. Click tools, options, document properties, line font.
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