A Bit of Intro
One of my recently acquired hobbies is 3D design. Once I got a 3D printer, I wanted to know how to design my own things. At first, I started with SketchUp.
This is a simple program that you can use to design all sorts of simple objects. But then I soon realized that the lack of features was slowing me down. So I then went on to Tinkercad, which allowed me to improve some of my models. But it was still not enough. I finally ended up using Solidworks. After some time, I also discovered Fusion 360 from Autodesk, which works in a similar fashion.
In this small how-to, we’ll walk through designing a mounted coat hanger. It uses two wood screws and is easy to mount anywhere.
While there are better ways to design this, I will walk you through a simple process. It should be easy to understand.
We’ll start by clicking File / New / Part and then OK.
We're now in the design environment, so we’ll select the Front Plane with the left mouse click. On the small contextual menu that appears, we’ll click on the first option: Sketch. The camera will reorient itself. We’ll be looking straight down on the front plane, with the sketch tools active.
Finding The Line Tool
So we’ll begin with adding a line that starts at the point of origin (the red dot with arrows).
To do this, we either select the Line tool from the sketch toolbar or hit the “L” key on the keyboard. You can also hold the right-click anywhere on the work-space. Then navigate left in the contextual menu that appears.
Drawing the Line
With the line tool active, I’ll start a horizontal line beginning at the origin. To do this I click the starting point (the origin) and the end point of the line. You'll notice that Solidworks snaps to certain points/edges by default. This makes drawing easier.
It doesn’t matter how long the line is at this point since the next step is to dimension it. While dragging the line, you should notice a yellow square next to your pointer. This indicates that you’re drawing a horizontal line.
Adding Dimensions to the Line
After we draw the line, we’ll move onto adding a dimension to it. To do this, we’ll use the Smart Dimension tool. You can find this tool in the sketch toolbar. Or you can hold the right mouse button in the work-space and navigate up to select the Smart Dimension tool. Once the tool is active, we’ll click on the line we drew earlier.
You should notice the dimension following the mouse. We can place this dimension anywhere on our work-space. After we click again to place it, Solidworks will open a small window that asks us for a dimension. We’ll type in 15 mm for now, and then hit the Enter key, or click the OK button on the small window.
Drawing the Circle
Next, we will draw the first hole, or should I say half of hole, for the coat hanger. To do this, we’ll select the circle tool (next to the line tool on the sketch toolbar). You can also select it by holding the right click on the work-space and navigating right.
To start the circle, click somewhere on the line. Don't start at the middle of the line, since then we would have to drop a sketch constraint. Move the mouse away from the initial point and click again to place the circle.
Define the Circle Relative Position and its Diameter
Next, we will place the circle at 8 mm from the origin, while adjusting its dimension to a diameter of 3.5 mm. To do this, first select the Smart Dimension tool. Then click on the point at the center of the circle, then on the point of origin (the red one with the arrows).
Drag the dimension out and click to place it. When the small window appears, input 8 mm then hit Enter or click the green check mark. You’ll notice the circle will move its position to the specified distance.
Now we will proceed to dimension the circle diameter if you haven’t already done so. If the dimension tool is still active, click anywhere on the circle perimeter. Drag out a dimension.
Click to place the new dimension and input 3.5 mm in the dimension box that appears, then hit Enter. You will notice the circle will either get smaller or larger, depending on its initial size.
Trimming Away Unwanted Sketch Entities
Since this part will get mirrored twice, we can go ahead and remove the "excess" circle. What I mean by this is that we can remove the top side of the circle and the line that intersects the circle at this point.
To do this, we’ll be using the Trim Entities tool, in the sketch toolbar. Click on it, and make sure you select the Power trim option in the left toolbar. The power trim works by dragging a freehand line on the work-space. It will remove any sketch entity encountered along it’s path up to the nearest point or intersection.
So, with the Power trim tool selected, start dragging with the left mouse click. Move from the top of the circle, down through the top perimeter section of the circle. And through the line that intersects the circle.
While dragging, you should notice a faint line of the path you’re describing with your mouse. Only the bottom part of the circle will remain, along with the two parts of the initial line we drew.
Our First Vertical Line
Next, we’ll start a 5 mm vertical line down from the right end of the initial line. If you followed along, you should already have a good idea about how we can do this.
Select the Line tool, place the starting point of the new line at the right end of the initial line. Drag down (notice the yellow square that indicates verticality) and click to place.
Select the Smart Dimension tool, click on the new line, input 5 mm and hit Enter.
Our First Custom Defined Point in Space
We’ll now place a point which will help us with some of the next steps.
In your sketch toolbar, you should notice the Point tool in the last place of the third row. It's in the same section where the line and circle tools are. Click on it and place it anywhere below your sketch. Your next move is to position the point exactly 10 mm below the origin (the red dot with arrows).
To do this, make sure you deactivate the Point tool. You do this by either clicking on the Point tool again in the sketch toolbar or by hitting Escape on your keyboard. Next, with the mouse pointer select the dot you placed.
While holding down Shift and select the origin by clicking on it, so in the end, both points are in the same selection. You will notice a new section in the left toolbar that reads Add Relations.
Click on the Vertical relation button (the one with the vertical line symbol). You’ll notice the point moving straight below the origin point. Also, a new Vertical relation appears in the Existing Relations on the left toolbar.
With both points still selected, activate the Smart Dimension tool. Drag out a new dimension and input 10 mm. What you’ve done is place a new point, at exactly 10 mm below the origin. Let’s move on.
Finishing Up the Initial Sketch
Starting from the point we placed, draw a 5 mm horizontal line to the right.
Finally, connect the far right end of this line with the bottom of the vertical line we drew earlier.
On the left side, use a vertical line to connect the origin point with the bottom part of the sketch.
I know it doesn’t look like it yet, but now we almost have a quarter of the base of the mounted coat hanger.
Exiting Sketch Mode
Now you can click on Exit Sketch since we’ll move on to Features.
The Extruded Boss/Base Feature
Click on the Features tab, below the Sketch toolbar. We will now use a simple extrusion operation on the sketch we drew.
So from the component tree, select the Sketch (it should be "Sketch1"). Your dimensions should reappear now if they disappeared when you exited the sketch.
Next click on the Extruded Boss/Base in the Features toolbox. You’ll notice the camera shift to an isometric view and a preview of the part taking shape. This is the preview of the extrude operation.
Modifying the Defaults and Applying The Feature
On the left tool panel, notice the 10 mm dimension that the tool defaulted to. We will change this to 5 mm and then click on the green check-mark to apply the extrusion. If all went well, you should have a 5 mm extrusion of your initial sketch.
You should notice in the component tree on the left side that a new Boss-Extrude operation exists. If you click on the small chevron on its left, the feature will expand its contents. You will notice that it contains your initial sketch.
Reorient the Camera and Place a Sketch on a Surface at the Bottom of the Part
Next, we will start a sketch on the bottom side of the extrusion. To do this, you can hold down the middle mouse button to rotate the part. Or, for a more precise look, hit the Spacebar and the orientation window should appear. Select the bottom orientation.
Now click on the small square surface at the bottom of our part. Switch to the Sketch tab and click on Sketch to start a new sketch on this surface. This will be an easy sketch since we’ll be outlining the profile at the bottom. Select the Corner Rectangle tool from the Sketch toolbar.
Draw a rectangle beginning at the top left part, down to the bottom of the surface you’re sketching on. After the rectangle (square in our case) is in place, exit the sketch.
Reorient Camera Again And Sketch On Another Plane
Now, hit the spacebar to open the Orientation window again and select the Right orientation. From the element tree on the left, select the Right plane and start a new sketch on it.
Place a point on the left side of the part. Deactivate the point tool by hitting Escape. Now select both the created point and the lowest point on the left side of the part. Apply a horizontal relation (left panel). With both points still selected, hold the right click on the work-space.
Navigate up to the Smart Dimension tool in the contextual menu. Place the new dimension and input 5 mm.
The Centerpoint Arc Tool
Next, we’ll play with the Centerpoint Arc tool. This tool works by first selecting the center of the arc. Then you place the radius. Finally, you go along the length of the arc you want. It's a total of three clicks. Don’t worry about the shape of the arc, we’ll fix it with a relation.
To start, with the Centerpoint Arc tool selected, first click on the point you created earlier. This will place the center of the arc. Then for the second point, click on the left lowest point in the part (the same point we used earlier). You should have now a set radius of 5 mm.
The third part is to describe the length of the arc. So click somewhere at the left side of the arc's center-point. Deactivate the Centerpoint Arc tool (Escape key) and deselect the arc if it’s still selected.
Hold the shift key down and select both the endpoint of the arc and its center-point. Add a horizontal relationship between these two. You should now have a semicircle. We’ll use this semicircle as a path for the next Feature operation. Exit this sketch.
The Second Feature: Swept Boss/Base
Switch to the Features tab now. Select the Swept Boss/Base feature. This feature will ask you for two inputs. The profile and the path along which the sweep will occur.
For the profile select the small square sketch at the bottom of our part. For the path, click on the semicircle we sketched. You should see a preview of the sweep you’re about to apply. Click the green check-mark on the Sweep (left panel) to apply the sweep.
Aesthetic Features: The Fillet
We’re getting closer to a quarter of a finished part. Looking at the part it seems a bit rough around the edges. Let’s fix that before the mirror it.
We’ll select a few edges that we should round off a bit for the final design. Look at the picture below for a good reference point. Your selection should have 11 edges in total. Next click on the Fillet tool in the Features toolbox. By default, the Fillet tool is set at a radius of 10 mm and No preview. So set the fillet at 2 mm and Full preview.
Use the images below as a reference. If you selected too many edges, or too few, click on the Items to Fillet. Then either Delete the ones you don’t want or add more by clicking on the model’s edges.
When you’re happy with your selection, click the green check-mark in the Fillet panel to apply the fillet.
Aesthetic and Functional: The Chamfer
One final detail we should consider is the chamfer. This will make sure our mounting screws are nice and flush.
To do this, we’ll use the Chamfer feature, that’s in the same location as the Fillet feature we used. So click on the small arrow at the bottom of the Fillet feature and select the Chamfer.
In the left panel make sure you input 2.5 mm for the distance and 45 degrees for the angle. Then click on the Chamfer Parameters box and select the top edge of the open screw hole. A preview of the feature will show up.
Click the green check-mark in the left panel to apply the chamfer.
Mirroring The Part Twice
We are finally at the point where we only have to mirror the part twice. To do this, expand the menu next to the Fillet feature, where it reads Linear Pattern. Then select Mirror from the list.
We’ll need the right plane as the mirror for the Mirror Face/Plane section on the left panel. So on the right of the left panel, expand the component tree and select the Right Plane as the Mirror Face/Plane.
Now we need the body we wish to mirror. Click on the box in the Bodies to Mirror section, then click anywhere on the part. Make sure you also enable the full preview, so you know what’s going to happen.
You should see a preview of your mirrored part. In the Options part of the left panel, make sure you check all three check-boxes. These are: Merge solids, Knit surfaces and Propagate visual properties.
If you’re happy with the current preview, click the green check-mark of the left panel to apply the mirror.
Only one more mirror to go. So again, from the same drop-down list in the top Features toolbox, select the Mirror feature.
This time you’ll need the Top Plane as the Mirror Face/Plane.
Then the whole body constructed selected for the Bodies to Mirror section. If you’re happy with the preview, click on the green check-mark to apply the Mirror.
Saving and Multiple Exports
Congratulations! The part is complete. Now let’s save it, so we don’t lose our work. Click on File and select Save As... from the menu.
Then pick a location on your hard drive, name the file and click on Save. To 3d print, the part, go to the File / Save As… part again and select the STL file type from the drop-down menu. Click on Yes if a new window appears. If the Export window appears after that, check the All bodies radio button and click OK. You should now have two files: the SLDPRT extension file and the STL file.
You can use the SLDPRT to change your part in Solidworks. And you will use the STL file for any slicing software so you can 3D print the part.
Next, we’ll move onto slicing and print the part so we can bring it to the real world and use it. I’ll be using Cura version 3.0.3 for this part. You open the STL file you created and place it on the build plate. In my case, I actually need three of these, so I’ll multiply the part.
I’m quite happy with my other slicer settings, so I’ll export it in GCODE for the 3d printer. I then load the GCODE file onto my printer and hit print.
3D Printing our Designed Part
Beyond this point you'll need access to a 3d printer. If you don't already have one, I recommend the models below.
Tevo Tarantula 3D Printer
This article is accurate and true to the best of the author’s knowledge. Content is for informational or entertainment purposes only and does not substitute for personal counsel or professional advice in business, financial, legal, or technical matters.
Leave a note
Emanuel Bucsa (author) from Baia Mare, Romania on November 07, 2017:
Well, I tried to be as explicit as possible :)
Eugene Brennan from Ireland on November 07, 2017:
This is great! Lots of detailed easy to follow info and and graphics!