Linking Sketch Blocks in SOLIDWORKS

TATA Technologies - James Keller | August 8, 2016 | Comment

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In the tutorial video above, we have an open sketch containing a single block.

The “3 Point Bracket” block is something we’ll want to be able to use in future designs, so we’re going to save the block to a central location. But first, we’ll want to change the color of the block so it stands out form other geometry when it’s used.

 

 

To do so, I’ll select it and then go to “Edit” > “Appearance” > “Sketch/Curve Color…” We’ll choose a green color, and then click OK, but when we do, the box still displays in black, denoting a fully defined sketch.

To display the sketch in color, we’ll first need to bring up the “Line Format” toolbar, under “Convert Entities,” and toggle the “Color Display Mode” button.

 

 

This switches sketch and edge geometry between system colors, an applied line or layer colors.

Now that we’ve got the block defined how we like, I can save it to file. We can now select the block and then click “Save Block,” from the “Blocks” toolbar.

Next, we’ll switch over to another example, where we want to insert a few instances of the three-point bracket. We’ll browse for the file to insert it and then relate each instance to the base bracket.

 

 

At this point, it’s important to know that the blocks can still be edited independently of the saved block. If we go back and edit the block definition and then resave it, instances like that in the image depicted above will still remain the same. This is because the block in the sketch is not linked to the saved block.

To link the block with its saved definition, I have to select an instance and then toggle the link icon in the property manager.

 

 

When we do this, all related instances will update to reflect the changes. Toggling the link icon again will break the connection, but does not return the block to its original definition. If we want to make sure blocks are linked to their saved definitions upon inserting them, we just need to make the “Create external reference to file” option is checked when inserting the block.

 

 

To find more tutorial videos like the one shown above, visit myigetit.com.

 

About the Author

 

James Keller has over seven years of CAD and instructional design experience, with a primary focus on SOLIDWORKS 3D design software. A strong design background allows him to wear both the hats of Engineer and Designer at once.