I first learned CAD – Computer Aided Design – a little over 26 years ago, and yet I still find digital modeling to very challenging at times.
While I’m in no position to teach others, I thought I’d share the main steps I took to model a basic project enclosure half-box that I use to test 3D printers and CNC desktop mills.
I have used many 3D modeling programs over the years. Familiarity comes from repetition.
Switching programs can mean having to learn entirely new ways of doing things, but most modern 3D modeling and engineering software packages and apps tend to have similar tools.
The basics remain the same.
Note: 3D modeling pros, please don’t yell at me until you get to the end of the post.
How I Modeled the Box in Solidworks
For this model, I started with a sketch – it’s a rectangular box measuring 2″ x 3″.
Next, I used the extrude/boss tool to make the 2D shape into a 3D part. I gave it a height of 0.60″.
Some apps call this extrude/cut, push/pull, or similar. It basically transforms a 2D shape into a 3D object.
I then used a “shell” tool to hollow out the rectangle, setting the thickness of the side walls and bottom.
In other software, I would have sketched a rectangle on the top face and then extruded downwards.
Then I added fillets to the corners, with a 0.18″ radius.
I found it a lot easier to sketch a rectangle, extrude it, use the shell tool to hollow it out, and then add fillets to the corners to round them, than to extruded a rounded-corner rectangle.
And because the corner fillets are not locked into the initial sketch, I can more easily modify them later.
There are different ways to make the same shapes, with some easier than others.
I used construction lines to define center points, and then sketched circles on the top plane, also with 0.18″ radius. This is for unthreaded screw bosses that will match the outer radius created by the corner fillets.
Extruding downwards to the top of the bottom wall gave us this shape.
I then sketched smaller circles, with a 0.12″ radius, on the top plane, working from the same center points as before.
Using the cut/extrude tool hollowed out the holes to a set depth.
Summary: I made a rectangle, then turned it into a box. Used the shell command to hollow out the box. Fillets rounded the external corners. Added a circle to each corner, then extruded them into cylinders. Added smaller circles and then cut-extruded them into unthreaded holes.
The reason I reopened this file is because I want to modify the dimensions so that I can use it to test desktop CNC mills. I also want to make smaller parts in 3D printer filament tests, to save on materials.
I Repeated the 3D Modeling in Fusion 360
Different modeling platforms have different nuances.
For example, I used a multi-thickness option in Solidworks to create walls (0.15″) and a bottom layer (0.10″) of different thicknesses. In Fusion 360, to do similar I need to create a shell with 0.15″ walls and then offset the bottom by 0.05″ to get the same 0.10″ thickness.
There’s an “offset face” tool in Fusion 360 to lower the bottom to the correct depth. For this shape, extruding it with a negative value would have also worked.
I modeled similar in Fusion 360 just now. The tools are mostly similar, but the interface is completely different.
Fusion also shows dimensions differently. I could see dimensions for sketched components, but not extruded unless I used the inspection tool.
I inspected a cross section to ensure the bottom wall was a different thickness than the side walls.
And yes, I goofed – extruded the corner bosses to 0.45″ instead of 0.50″, forgetting that the bottom wall was set to 0.10″ from the extruded height of 0.60″. There’s a 0.05″ gap.
There, I fixed it.
Fixing Beginner Mistakes
Everything I did makes sense, and it works. But it’s not the best way to do things.
Here’s what happened when I dropped the 3″ side to 2″.
Here’s what happened if I instead expanded the 2″ side to 3″.
I did not properly define the relationships between the different parts and features, and so the model is not responding predictably.
If I shorten the extrusion height, everything looks as expected, except the stopped holes are now through holes.
I’ll be recreating the part with properly-defined constraints and relationships between the features relative to each other, so that I can modify the part to suit different testing needs and material dimensions.
This is what it looks like if I go back in Fusion and modify the original 2″ x 3″ sketch to 2.5″ x 2.5″.
It’s what happens when you don’t pay attention to constraints.
In modeling software, a common adage works just as well as in programming – don’t repeat the same task any more than is necessary.
How exactly do we want to define the corner extrusions? Instead of a set dimension, we can extrude it to an object – the bottom face. This way, if we make the box taller, shorter, or with a thicker bottom, everything will still work.
Okay, so this is what my revised model looks like in Fusion 360.
Earlier Model
They look the same. But they’re not.
Let’s go back and change the dimensions from 2″ x 3″.
Here, I modified both dimensions to 2.5″ x 2.5″.
Here it is with taller height and longer length. It looks as expected.
What did I do differently?
It all has to do with how the circles are referenced in their sketches.
Instead of drawing 4 circles at 4 corners, we start with 4 circles of whatever diameters. I set one circle’s dimension (top left) to 0.36″ (diameter). Then I constrained all 4 circles to be equal to each other.
I started off my creating a horizontal line from midpoint to midpoint before setting it as a construction line. I did the same for a vertical line.
I set the center of top right circle to be positioned 0.18″ away from the top edge, and and same for the center from the right edge. I then selected the centers of the top left and right circles and selected symmetry constraint about the vertical line.
Then I used symmetrical constraint for top left and bottom left circles. I followed up by doing the same with the bottom left and bottom right circles. Or, I could have done the same with top right and bottom right.
It’s a little different in Solidworks.
Here, I found it easier to sketch a single circle and set it to 0.36″ diameter. I then created construction lines in both directions, across the midpoints.
Then, I used mirror-copy to duplicate the circle. First I mirror-copied the top left circle to the top right, and then selected both circles on the top and mirror-copied then about the horizontal midpoint line. Construction centerlines would have also worked.
I could have also set their constraints from the edges. It all depends on if and how you might be modifying the model.
I’m sure there are other or simpler ways to do this.
This looks the same as the model at the start of the post, doesn’t it.
But with this one we can make changes with greater predictability.
How you reference your dimensions and part features makes a huge difference.
It also helps to pay attention to the types of tools you use, and the order in which you add features to a part.
Again, because the rounded corners were created with fillets, I can change them much more easily than if they were created as part of the first sketch with the starting rectangle.
Sometimes even just a hole size needs to be changed, and it’s easier to change all at once than one by one.
What if you don’t plan on making any changes or modifications to a design?
Well, simpler and direct reference points and construction lines can still work. But going back to programming principles, it’s often slower and less effective to make the same definitions over and over.
It’s tedious to get the hang of constraints and relations, but they’ll often save you time in the end. If you need to make changes, designing a part with best practices is quicker and easier than having to start over, or fix relations that fail with changes.
Let’s say we have to change hole sizes very slightly. It’s easy to miss one of the change is small and each hole needs to be selected and changes. If they’re all supposed to be the same, and set to be equal, it will be better to change the one dimension all the holes are set to.
I tend to put off modeling because each part presents a stubborn learning curve. But lessons do stack and make things easier.
