Modeling Challenge – Calculate Internal Volume

Continuing the modeling challenge theme I started with my last post, I’d like to review a few different ways to calculate the internal volume of an open container. There’s something to be learned from each method, but thanks to recent enhancements in SOLIDWORKS, some are much easier than others. Feel free to try this out for yourself on this 2015 SOLIDWORKS model, and don’t hesitate to comment if you discover an even better method.

Modeling Challenge - Calculate Internal Volume

 

Surfacing (8 Steps)

Surface modeling provides the most flexible and creative modeling workflows in SOLIDWORKS since we’re not confined to the typical constraints of the solid modeling environment (i.e. the constant necessity of water-tight faces).  Though surfacing can often provide convenient modeling shortcuts, in this case, it’s the most manual process.

  1. Right click an internal face of the container and choose the ‘Select Tangency’ option
  2. Copy all of the selected faces by using the ‘Offset Surface’ command with a value of 0 (note: the command name in the PropertyManager will change from ‘Offset Surface’ to ‘Copy Surface’ as soon as the offset value is modified)
  3. CTRL+Drag the ‘Top Plane’ to create an offset plane representing the liquid level
  4. Sketch a rectangle on that plane
  5. Create a ‘Planar Surface’ from that sketch
  6. Hide the solid body of the container to isolate the view of the two surfaces
  7. Remove the extraneous portions of the surfaces using the ‘Mutual’ mode of the ‘Trim Surface’ command
  8. Apply the ‘Thicken’ command to the leftover surface model with the ‘Create solid from enclosed volume’ option activated

Multibody (5 Steps)

Multibody modeling allows us to create assembly-like designs within a single part file.  This environment enables us to model static in-context assemblies without the responsibility of managing external file references, but there are many more modeling tricks the multibody environment can be used for.  In this case, we’re utilizing some multibody features to perform Boolean operations – leaving us with a single body.

  1. Sketch a rectangle on the ‘Top Plane’
  2. Use this sketch to ‘Extrude’ to a height representing the liquid level with the ‘Merge Result’ option deactivated
  3. Make a copy of the bottle’s solid body using the ‘Move/Copy Bodies’ command
  4. Use the ‘Subtract’ mode of the ‘Combine’ command to subtract the copied bottle body from the extruded block
  5. Choose to only keep solid body representing the internal volume

Intersect (2 Steps)

The Intersect command (introduced in 2013) is an underutilized feature that combines the power of the Split, Replace Face, Trim, Knit, and Combine features into a single easy-to-use interface. There are many more cases to use the Intersect command, but this example clearly illustrates the time savings it provides.

  1. CTRL+Drag the ‘Top Plane’ to create an offset plane representing the liquid level
  2. Use the ‘Intersect’ command to generate a solid body in the theoretical water-tight volume created by the bottle’s body and the recently created plane

Is this the first time you’ve heard of the Intersect feature?  If so, read more about it in our online help documentation, and don’t forget to check our What’s New documentation after each upgrade.

Still not fast enough? Stay tuned for updates in SOLIDWORKS 2016. Make sure to follow the SOLIDWORKS 2016 Sneak Peek blog posts to see what awaits in our next release.

Jordan Tadic

Jordan Tadic

Territory Technical Manager - NA East at SOLIDWORKS
Jordan has been serving the SOLIDWORKS community for over 10 years. He’s a mechanical engineer by day and a wannabe artist by night, so he’s at his best when he’s forced to use both sides of his brain to solve complex modeling challenges. If you have one for him, don’t hesitate to share it. His specialties are surface modeling, industrial design, cloud solutions, and technical communications.
Jordan Tadic