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.
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
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
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