The SOLIDWORKS sensor tool allows a user to set parameters within
a model or assembly that can then be monitored by SOLIDWORKS as your design is
developed. If a design change you make results in a deviation outside the
limits you specify, then the software will alert you, allowing for the
appropriate action to be taken.
The sensors folder can normally be found in the feature
If you don’t have it, you can set it to show in your system
options. (see below)
demonstrate a sensor, we will take a look at an example from the SOLIDWORKS
Assembly modelling course.
this design we want to monitor the clearance between the outer face of the main
body and the inside face of the retaining plates, so as to ensure product can
be easily assembled.
will use a sensor to monitor the amount of clearance in this area. To do this
we must first add a reference dimension. This dimension is what the sensor will
To add a reference dimension, select the smart dimension tool from
the sketch toolbar (you don’t need to be in a sketch).
Add the reference
dimension between the outside face of the main body and the inside face of the
retaining plate (the dimension should be shown in grey, denoting it as a
add a new sensor, right click on the sensor folder in the tree and select “add
sensor” from the menu.
The sensor property manager will open (as below). We will
now take a look at the parameters which can be set for Sensor types, Properties
There are a number of sensor types to choose from including
Simulation Data, Mass properties, Dimension and Measurement. A description of
each type of sensor is shown below. (Taken from SOLIDWORKS help) For our
example we are going to choose dimension from the list of sensor types.
There are a whole list of properties available for
selection. Each sensor type has specific properties relating to it (there are
lots of options, so take some time to see exactly what’s available). In our example
we will be using a dimension sensor. For the property we simply need to select
the reference dimension we added earlier. The value of the selected dimension
If we wish for SOLIDWORKS to make us aware of any changes
made to the dimension we are monitoring then we must tick the alert check box. In
here we can choose as to when we wish to be alerted of any changes. In our
example we want to be alerted if the value of our reference dimension falls
below 0.5mm (see settings in image below).
With all the settings made, close the sensor property
manager using the green tick and continue with the design. Notice that the
sensor folder in the feature tree contains the dimension sensor we just configured.
Open up the retaining plate part and modify the recess from
2mm to 2.6mm. Exit the sketch and update the model.
Return to the assembly to review the effects. You will
notice that there is now and error in the feature tree.
The sensor has been triggered due to the design change made,
resulting in a warning in the feature tree that we can now react to. Relevant
changes can then made to ensure the design is in keeping with the sensor
More information on sensors can be found in the SOLIDWORKS online help documentation
If you would like to try this example for yourself you can
download the training files here.