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SolidWorks Technical Tips & Techniques

» How to set up a property to calculate shipping weight

With this tech tip, we are going to look at putting shipping weight in a template or part so the property will show on the drawing.

First a couple questions to think about:
   1. Do you put shipping weight on your drawing?
   2. Is the calculated shipping weight a percentage of the actual weight?

We will show you that SolidWorks, can accomplish these calculations and output the results very easily. Our goal for this tech tip is that you will understand how to do this on both a part and a template.

Step by step instructions listed below video & SolidWorks eDrawings links

Click here to watch this Flash SolidWorks Tech Tip video  
Press F11 if you cannot see all of the video while watching

Click here to download the SolidWorks model & drawing files

The first thing we must understand is how do we define Shipping Weight. Usually Shipping Weight is calculated as a percent added to the actual weight. This is to account for non-modeled items that are shipped with the item.

1. Open a part, or a blank template.
2. To start with, lets take a look at the actual weight of the model so we have a good idea what our
    starting point will be.
          a. We can do this easily by going to the "Evaluate" tab and choosing "Mass Properties".
          b. Notice all the information about this model we get from this dialog.  We are most interested
              in the mass of model at this time.  You will notice that the actual mass is 196.66 pounds.
3. Net lets add an equation that calculates the Shipping Weight based on the actual weight.
          a. Our equation will simply be: Shipping Weight = "The mass" times 1.10
4. In order to do this we will need to use the "Equations" dialog in SolidWorks.
          a. Add a new Equation, by clicking Tools ~ Equations ~ Add.
          b. Using the equations dialog, create a variable called "Shipping Weight", by typing Shipping
              Weight in quotations and then put an equals sign.
          c. At the bottom of the equations dialog box there is a chevron.  Click this and it will expand
              the inputs box.  This area calls any SolidWorks Properties and any custom properties.
          d. Click SW-MASS, which is the SolidWorks Property for Mass, this will add the proper callout
              to the right side of the equal sign.
          e. Now finish the "Shipping Weight" variable by adding the text "*1.10"
          f. The value entered is the percentage over 1 that you want to calculate.  In our example
              we want to calculate plus 10%
          g. Double check the variable.  It should read "Shipping Weight"= "SW-MASS" * 1.10
5. Click OK to create the variable
6. Click OK to dismiss the equations dialog.
7. Next lets add a custom property that will be used in the drawing to link to the equation
    previously created.  To create a custom property we will need to click File ~ Properties. 
          a. Add a new configuration specific custom property called "Shipping Weight".
          b. Use the drop down arrow to select our previously created variable.
8. The last step is to create a note in the drawing that links to the property "Shipping Weight".  Alternatively, you could actually put this in a BOM at the assembly level.  Or you could do both.  The custom property will automatically update to any design changes to the model.

As you can see from this tech tip, using SolidWorks Custom Properties and Equations allows for leveraging data from your design accurately.  This also provides a time savings be removing repetitive manual calculation.

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