Design Studies in a Bottle

One of the questions I hear a number of times a year is, "How do I measure the volume of a container and what is the best way to monitor the volume while making changes?"

Let's take a closer look at the process. I might recommend using this small cosmetic bottle.

1. Cap the top of the bottle with some type of extrusion, merging the feature to the existing bottle.
2. Use what I call the Box-Extrude/Combine-Subtract method.  Extrude a large box around the entire bottle (add dimensions as you would like and make sure the box is large enough to accommodate any future changes you might make to the bottle) and make sure to NOT merge the box extrusion to the bottle (you should have two bodies now, a box and a capped bottle.)
3. Use the Combine command to subtract the bottle body from the box body (Insert-Features-Combine for those who may not have used this command before.) When prompted to choose which bodies to keep, only pick the inner body which is the fluid volume of the bottle. 
4. Mass Properties will now display the Volume of the fluid
5. Create a new Design Study in the model (right-click the Motion Study 1 tab in lower left corner of SolidWorks.)
6. Add Variables to the Design Study linking them to dimensions in the model you would like to adjust.
7. Set the variable information as needed (Range, Range with Step, Discrete Values.)
8. Add one or more constraints by adding Sensors in the model.  (For this bottle I added a Sensor to monitor volume and set the constraint to be between 99mL and 101mL because I want a 100mL bottle)
9. Hit RUN and watch the model adjust the dimensions through each scenario and based on your sensor the results view will give you a pass or fail. 
10. Weed through your results and find the scenarios that passed.  You can pick on the headers to have the model update to the dimensions from that particular scenario.
11. Pick your final dimensions or add more as variables and run again.  You can also choose to optimize the design which allows the addition of a goal and SolidWorks will then try and tell you what the best combination of dimensions is. 

For those that still may be a bit confused.  Here is a link to a YouTube video I created of the process.  I would love to hear your comments and suggestions for other tips for that you would like information on.

 

See more SolidWorks Videos on the Fisher/Unitech YouTube channel

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Brian VanderPloeg is an Applications Engineer at Fisher/Unitech, a SolidWorks Value Added Reseller with locations across the Midwestern and Northeastern United States. He is a regular contributor to the Fisher/Unitech blog.