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A Linear Pattern Design Library Feature – Unistrut Weldments

Wednesday May 7, 2014 at 4:52pm

SOLIDWORKS offers integrated Weldment Structure design tools at all levels of the product. Through the ‘SOLIDWORKS Content’ section of the design library, profiles for most types of structural member can be downloaded. The ‘Unistrut’ type is one of these and using it allows us to easily create structural members like the ones shown in the image below and left.

The Weldment tools speed up the creation of even the most complex structures. However, due to the way the system extrudes the profile along the path we sketched it can not construct additional detailing along the length of the structural member. The majority of Unistrut structural members include holes like the slotted ones shown in the image below and right.


Modelling these holes on every structural member would be fairly painful! To get around the problem we can create a fully automated design library feature. The feature will include a slotted cut and automatically determine the direction and number of instances needed to pattern it along our structural member.

Open a new part document and make a long and thin rectangular block (the dimensions of which are unimportant). On one of the faces draw the sketch shown in the image below. 

The position and size of the slot should be fully defined. The long blue line is sketched coincident to the ends of the block then a Dimension is added to it. When this dimension is added you will receive a message asking if you want it to be driven or to leave it driving, select ‘Make this dimension driven’ and that’s the sketch finished. Use the sketch for a cut extrude feature and set the end condition to ‘Up to next’, this will ensure that in our final part the cut goes all the way through the structural member but not anything behind it.

The next stage is to choose the Linear Pattern command from the features tab and select the long edge as the direction for the pattern. Set the pattern spacing to whatever value you wish although with most of the ‘Unistrut’ types the spacing should be 50mm. The number of pattern instances is driven by an equation so click in pattern instances field and type ‘= (‘, then click the driven dimension on the long line we sketched, then type ‘–‘ and click the dimension determining how far the slot is from the end of the block and close the brackets ), finally type ‘/50’ (to divide by the pattern spacing).

The finished equation should look like the one shown below. Where D1@Sketch3 is the 262.762mm dimension and ‘Short Edge Distance@Sketch3 is the 10mm dimension.

Accept the feature and use the Add to library button at the top of the design library. In the ‘Items to Add’ section, choose the ‘Cut Extrude’ and the ‘Linear Pattern’ but not the initial ‘Boss Extrude’ feature. Choose a location in your design library to save and click the green tick. Make a Test Weldment and drag your feature out from the saved location in the design library on to a face of the model. A window will appear asking you to select 3 edges (shown in the image below and left) once you click 3 similar edges on the test model the feature will insert itself (see image below and right).

By Peter Harkness

Applications Engineer


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