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Thursday, June 16, 2016

Finding Internal Volumes Using Autodesk Fusion 360 - A Nice Little Trick!

Just this week, I had to figure out how to find the internal volume of a hollow structure.

Liquid in a bottle is the typical example.  And I'm using a bottle in my example, but I threw a bit of a twist on it. 

I mad the bottle a little crazy.  You know, for fun! 

Here's a shape to get the internal volume for! 
Finding internal volumes can be a bit of a feat sometimes.  Many hollow vessels have stiffeners, valves, risers, or some other nook or cranny that doesn't make this a simple task.

Here's how I was able to crack this particular nut in Fusion 360. 

1) Seal up the volume. 

The first step, is to close up the volume and make it "watertight".  In other words, you have to make sure that there are no gaps in the envelope defining fluid volume.

Looking at the bottle, the neck is an opening, so that has to be closed.  You can close with a solid, with a surface, or in this case, I'm using a workplane. 

The workplane is added. 

2) Fire up the Boundary Fill tool

Step 1 defined the boundary, now it's time to fill it!  The Boundary Fill tool will be the one that will help us fill the boundary we will define.

You'll find that under the Create pulldown menu. 

Filing up the Boundary Fill command

3) Start picking what to fill! 

Now comes the trick! When the dialog box for Boundary Fill appears, pick the lower half of the bottle and the workplane that defines the fluid level in the bottle with the Select Tools options highlighted.

Selecting the boundaries of the volume.  Only the work plane
is selected in this picture.
Once you have the lower part and the bottle selected, choose the Select Cells option and choose the volume you want to fill.  

You do this by selecting the check box that corresponds to the volume you want to fill.

Selecting the volume to fill.
Once you have it, choose OK!

4) Verify the solid you just created! 

If you check the browser, you should see an additional body in the browser.

The volume highlighted.  I've turned the visibility of the workplane
off to make the solid easier to see.

You can toggle the visibility of the bottle, leaving just the body representing the volume of the fluid inside.

The volume created by the boundary fill command.
5) Check the volume! 

All that's left to do, is locate the body in the browser, and choose Properties.

Locate the body and select properties.

Search through the options and find the volume, and your set!

In Conclusion

This tool can be a great addition to your arsenal.  I've used it a couple of times, and it's been a nice asset for me.

One thing I will say, is give it a little practice.  It takes a little time to get the process down pat.  But don't worry!  It's not too hard to get the hang of.

Do make sure to give it a try!  I think you'll find it's well worth it!

Tuesday, June 07, 2016

Fusion 360 - Learning to Create Drawings.

Even as the CAD world steams at flank speed toward the "Land of 3D", many of us, even most of us, still need to generate a 2D drawing.

As I created a design to take me through the process of creating parts and assemblies, I have at last reached the point of creating drawings.

So how does Fusion 360 create drawings?

It all starts with the model that you want to create the drawings from.  In this example, I'm going to use the end table I used in my last post.

Revisiting the this coffee table.
To create a drawing, choose the File icon and choose New Drawing.  You'll have the option to create a new drawing From Design or From Animation.  In my example, I'm going to use the Design.  Mostly because I haven't had a chance to try out animations yet!

Creating the Drawing
The next screen will give you options to choose from to create the drawing.

 From the top, the options are:

  • A check box allowing you to create a drawing from the Full Assembly
  • A pulldown allowing you to choose American Society of Mechanical Engineers  (ASME) or International Organization for Standardization (ISO) standards for your drawing.
  • The units for your drawing (inches vs millimeters)
  • The size for your drawing, A,thourgh E for ASME, and A0 through A4 for ISO
Clicking OK will create the drawing.  And you can be off creating your assembly drawing! 

The drawing getting created.

Choose your options to place your view. A quick summary of the options are: 
  • A pulldown allowing you to choose the view orientation you want (Top, Bottom, Left, Right, etc.)  
  •  A pulldown with line styles (visible edges, visible and hidden edges, shaded with visible edges, shaded with visible and hidden edges) 
  • A Tangent Edge pulldown allowing you to show full length tangent edges, foreshortened tangent edges, or turn them off. 
  • A pulldown to turn interference edges on or off. 
  • A pulldown to turn thread display on or off
Clicking OK will place the view, and get you started.  Now your off and running with a drawing! 

But what about creating drawings of just the components?   What if you want piece part drawings? 

That's where we can return to the Create Drawing dialog box, you can uncheck the Full Assembly option to create drawings of individual components.  You'll have an option to select the component, or components, you want to create the drawing from. 

Creating a drawing of piece parts.
Note two components are selected.
So there you are!  Creating drawings from assemblies and components  

But there is one, last final tip.  You can also create a drawing from a component, by right clicking on it in the browser, and choosing Create New Drawing

It's another neat little trick to get started creating drawings!

Have fun, and enjoy!