Adding dimensions to your Sketches in SOLIDWORKS is one of the first things users learn to do. Dimensions, either driving or driven are critical to defining the shape of an object in SOLIDWORKS. In some cases though these dimensions provide information critical to the manufacturing process. Take for example the need to define, or get the overall length of a belt or chain. In some cases, you need to know how long the belt should be for ordering or manufacturing. In other cases, you need to work with a purchased or off-the-shelf component which has a pre-defined length.
The Path Length Dimension in SOLIDWORKS is a great way to capture this information while designing your parts and assemblies in SOLIDWORKS. To use Path Length Dimension, first expand the Dimension fly-out in the Command Manager (1). From that fly-out list, you will find the Path Length Dimension button (2).
SOLIDWORKS will then present you with with the Path Length Property Manager, including a selection box (3). Here, you can select any number of Sketch Entities to include in the Path Length Dimension. You can select these individually, however in the case of a belt or pulley, it might be easier to use Select Chain (4). Select Chain can be accessed from the right mouse click menu on any sketch entity. This is a great way to select a series of connected sketch entities; in this case the entire belt path. SOLIDWORKS will then add all of those sketch entities to the selection box in the Path Length Property Manager (3).
All that’s left is to choose the green check box (OK) button from either the Property Manager itself, the right mouse button menu, or the Confirmation Corner in the upper right hand corner. SOLIDWORKS, then does two things. It creates a path object from all of the selected geometry, and also adds the Path Length Dimension (5). This is like most other dimensions in SOLIDWORKS, in that it can be a driving or a driven dimension. In the example below, I’ve changed the dimension to 765mm. This value is now driving the overall length of the path; this can be seen by looking at the Reference Dimension I’ve also added (6). You can tell it’s a reference dimension because it’s both grey as opposed to black, and also less obvious is the very ‘uncommon’ value of 174.51mm. This is great for cases where you know the length of the belt or chain that you’re going to use in your design.
In some cases however, you might have strict location requirements for the pulleys or gears in a design, and instead need to determine the length of the belt perhaps. This is where changing the value from Driving to Driven really comes in handy. Within this sketch, you can right click on the Path Length Dimension (7) and choose Driven (8) from the right mouse click menu. When you do this, the dimension turns grey, and several sketch entities turn blue at the same time, letting you know they are now “Under Defined”. To “Re-define” the sketch, you will want to do the opposite for the dimension along the top (9). You will also notice, I’ve changed the dimension to a “real” number, in this case 175mm. In doing so, it has automatically updated the length of the Path Length Dimension (7) to 765.24mm. We could now take this value to the manufacturer to get the proper size belt made for this design if we so desired.
There is it, the Path Length Dimension in SOLIDWORKS, a very powerful tool that was introduced in SOLIDWORKS 2014. I’ve also provided a video below showing these same steps.
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