Brian has graciously allowed me to hop on the 3D Printering bandwagon to write a brief intro to the wonderful world of Solidworks. We’ll be making the same ‘thing’ as done in the previous ‘Making a Thing’ tutorials:
- AutoCAD Part I
- AutoCAD Part II
- Blender Part I
- Blender Part II
- Autodesk 123D
- FreeCAD Part I
- FreeCAD Part II
Admittedly, most Hackaday readers probably don’t have Solidworks as it is a very expensive program. The main reason we are posting this tutorial is so that you can understand the work flow and compare it to some of the free/open packages out there.
As Brian has touched on in his FreeCAD post, the part features of parametric models can be modified at any time. For example, let’s say I made a solid block, then added a specific size hole in the center of one face. Later, if I wanted to change the size or shape of the block, the hole would stay the same size and stay in the center of that face no matter the other changes to the object. See the graphic below, all that was changed was the size of the block, the hole stayed the same size and position (center of the face). This is different than if you were to ‘scale’ the entire object as the hole would also become stretched along with the block.
Between school and work, I’ve had the opportunity to use several professional parametric modeling softwares, including ProE (now called Creo), NX (was Unigraphics) and, of course, Solidworks. They are all similar in work flow. If you remember these 4 steps, you’ll do ok: Plane, Sketch, Dimension, Extrude.
There are 2 main tabs we’ll be using in this example, the Feature and Sketch Tabs. They have all the tools we’ll need to make the sample part.
Let’s create a new part, File then New. A window will pop up asking what file type to make. We are just making a single part so we’ll pick ‘Part’.
You’ll start with a screen showing empty space, this is where the object will be created. There are 3 planes, in the graphic below I have clicked on the Top Plane to select it. Why? Because ‘Plane’ is our first of 4 steps! We are selecting the plane (or surface) that the sketch will be drawn on.
With the Plane still selected, click on the Sketch Tab and then select Sketch. The view will move to be perpendicular with the Top Plane. We are now in Sketch Mode and will be able to make a sketch of a portion of the part. I have decided to sketch the bottom portion of the part first, the one with the hole and slot. It is just as easy to start with the back portion of the part.
The best part about sketching in a parametric program is that you can just sketch it without worrying about size or proportion. We will dimension the sketch after it is complete. To show you what I mean, I am going to intentionally make a really out-of-proportion sketch.
All of the tools we need for the sketch are on the sketch tab. For this sketch I’ll be using the line, centerline, circle, trim and fillet commands. Sketching at this point is very similar to any 2D CAD software with the exception that you don’t have to worry about the dimensions at this time. Just make it look close.
Well, isn’t that one ugly part! Ugly but totally acceptable. Notice that I intentionally left the inside and outside fillets off the bottom right leg of the part. I did this so we can add them after the part is extruded into a solid, just to show another way of doing something. Also notice that I made the circular features concentric with the intersection of the Front and Right Planes. This is a personal preference but I think it makes dimensioning a little easier as I can dimension features in relation to both of those planes, which also happens to be to the center of the circles. The dashed line coming from the center of the hole is a centerline and will define the angle of the slot. The centerline won’t become a feature of the part, it is just a reference. Later, I will make the slot edges parallel to this centerline, a certain distance away.
You can see a bunch of little green boxes all over the sketch. These are the relations of each feature. Each symbol means something. The vertical lines mean that the adjacent feature will always be vertical. The circle with a line means the arc is tangent to the line and will always be. Two lines and a red dot means that the two adjacent lines share an end or mid-point.
Our sketch now needs dimensions. On the Sketch Tab there is a tool called Smart Dimension. Select this to start dimensioning the part features. Here’s how you do it:
- To specify a distance between 2 parallel lines, click on one line, then the other line. A dimension will appear, move the mouse to where you want the dimension label and click to place it. Enter the distance in the dialog box that pops up and the lines will move to satisfy the new dimensional requirement.
- To specify a radius of an arc or diameter of a circle, click on the curve and place the dimension. Then type the value.
- To specify and angle between two non-parallel lines, click on one line, then the other. Place the dimension and enter the desired angle value.
- To add a relation, like specifying the slot edges to be parallel with the centerline, select one of the slot edges, then select the centerline while holding SHIFT. The Add Relations option will show up on the left of the screen. Select Parallel. You can see all of the available relation options. Notice after completing the command that the two lines are now parallel as well as two green parallel relation indicator boxes showed up. FYI, you can not be in the Smart Dimension function when adding relations.
Keep going with the dimensioning and you’ll end up with something like the below graphic. Notice that some of the sketch lines were blue but are now black. A black line means that it is fully defined regarding its location and size. This is a good thing and prevents unexpected and inadvertent geometry changes in the future. A completely black sketch can be referred to as ‘fully constrained’.
The sketch is done. Click Exit Sketch on the Sketch Tab.
This is the fun part. You can now see the sketch on the top plane and a new line item in the Model Tree on the left called Sketch1. If we need to change anything on this sketch (even after the model is created) we can do that by going back and editing Sketch1.
Click on Sketch1 in the Model Tree to select the sketch. Then on the Feature Tab, select Extruded Boss/Base. A dialog box will pop up asking how much to extrude the sketch. Enter the desired amount and click the green check mark.
Done Deal! ….for this portion at least. In Part 2 (not yet published) we’ll get going on the rest.
If you would like to waste 4 minutes of your life, here’s a video: