I’ve been writing these tutorials on making an object in popular 3D modeling programs for a while now, and each week I’ve put out a call for what software I should do next. There is one constant in all those comment threads: FreeCAD. I don’t know if these suggestions reflect the popularity
or difficulty of FreeCAD nevermind, it’s totally the difficulty.
FreeCAD is an amazing tool that, if used correctly, can be used to make just about any part, and do it in a manufacturing context. If you need a bauble that’s three times the size of the original, FreeCAD’s parametric modeling makes it easy to scale it up. If you’re designing a thumbscrew and want the head larger while keeping the threads the same, FreeCAD is for you. Basically, you can think of this as a graphical extension of the Thingiverse Customizer. Very powerful, very cool, and unlike a lot of CAD packages out there, free.
Our in-house, overpaid SEO expert (he’s really just a monkey someone trained to use a bullwhip) demands I link to the previous ‘Making a Thing’ tutorials:
The tutorial for FreeCAD continues below.
We won’t be copying this thing exactly - there’s a small taper on the tab with the counterbored hole – but we’ll get close enough so our finished model should be functionally equivalent.
Starting Up, And An Overview
To use FreeCAD, you might want to download FreeCAD. It’s available for Windows, Linux, and OS X in 32 or 64-bit varieties. Pick your poison. After downloading and installing, you’ll end up with a “start center” that looks something like this:
FreeCAD is unique among 3D design programs in that it has many different workbenches, or modes, to draw and model in. For most of our thing we’ll be using the Part Design workbench. Under the Start A New Project tab in the start page, click on the Part Design button. Hit Create Sketch, Choose the XY-Plane, and marvel at your drawing grid.
Before you begin, you might as well change the grid size to 1mm and turn on grid snap.
A word of note: While the grid size says millimeters, FreeCAD doesn’t really have units. Well, it has units, where one FreeCAD unit is equal to one FreeCAD unit. This is fine, because now we can design our part in eighths of an inch, where one eighth of an inch is one unit. It’s simpler, and to print out a correctly sized part we’ll need to multiply anyway…
If you read nothing else, read these two paragraphs
FreeCAD is a parametric modeler. This means all lines, figures, and subassemblies are defined by parameters and constraints. parameters are pieces of information that define a property of a part – a 10cm cube would have a parameter for the X, Y, and Z axes equal to 10cm. Constraints define the relationship between parts of an object. Two lines can be constrained to being parallel; move one vertex of a line, and a vertex of the constrained line will move as well.
Modeling an object parametrically is how companies can design many similar, but differently sized objects. A company that makes shoes may have only one model for every size of shoe. With parametric models, fabricating the parts for a run of size 6 and size 10 shoes may be as simple as changing a single number – the length from toe to heel.
For most of our modeling, we’ll be working with two toolbars. They are the geometries and constraints toolbars:
The Geometries toolbar is what you would find in just about any CAD or drawing package. You have buttons for creating a point, an arc, a circle, lines and polylines, and even fillet and trim buttons.
The Constraints toolbar has buttons for locking an object (a line, circle, polyline, or what have you) onto the vertical axis and horizontal axis. In addition, lines can be made parallel, perpendicular, on a tangent to an arc, and the vertical, horizontal distances of a line, as well as the total length of a line or the radius of a circle may be constrained as well.
The first part of our ‘thing’ we’ll draw is the largest circle. Using the grid snap (or by pressing CTRL while moving the cursor around), draw a circle at 0,0 on the grid. This circle will have a radius of 9.5. We’re doing our units in eighths of an inch, and since the largest circle has a diameter of 2 3/8″, or 19/8″, the radius will be 9.5 units. Also add another circle with a radius of 4.
You can use the Geometries button to make these circles roughly to size, then use the radius constraint to make the circles the required sizes.
After you’ve drawn and constrained these circles, you should have something that looks like this:
Now for some detailing
There’s still a lot to add to our ‘thing’. Let’s start with the 3/8″ wide slot. Start by drawing two lines roughly going from the center of the circles through the larger circle. Constrain them to be parallel, and the angle of one (the far right button on the Constrain toolbar) to be 45 degrees.
Using the Trim tool on the geometry toolbar, trim off all the excess – the ends of both lines, and the cutout on both of the circles. Now you should have something that looks like the letter C.
With the “Fix a length” constraint tool, make the distance between both of the 45 degree lines to be 3. Finally, lock the upper, outer vertex of the slot with the ‘Lock’ constraint. You should have something that looks like the pic to the right. You’ll also notice on the left-hand toolbar of FreeCAD the “Solver messages” says it’s a fully constrained sketch.
This means we’ve done this properly. Well, in this case that’s a bit of a lie (we haven’t guaranteed the slot is lined up with the center of the circles), but it’s close enough. In FreeCAD, the object is to have a fully constrained object. That’s what we’ve done here.
Since I like to keep these tutorials down to about 1000 words, I’m going to end this here. In the next installment of this tutorial, we’re going to add the flanges on this washer-type part, extrude it into the third dimension, and add the bit with the countersunk hole.
To be continued, and I’ll probably put a link to Part II right here.