Skip to main content

How to Design and 3D Print a Mounted Coat Hanger (Solidworks Tutorial)

I like learning about technology and IOT. I also dabble in 3D design and 3D printing.

A render of the final result.

A render of the final result.

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.

First Steps

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.

how-to-design-and-3d-print-a-mounted-coat-hanger-solidworks-tutorial

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 endpoint 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.

Notice the horizontal yellow marker when drawing the line

Notice the horizontal yellow marker when drawing the line

Scroll to Continue

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.

Placing the circle on the line

Placing the circle on the line

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 checkmark. 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 its 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.

Notice the thin path you describe while dragging the Power Trim tool

Notice the thin path you describe while dragging the Power Trim tool

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.

Vertical line placed and dimensioned

Vertical line placed and dimensioned

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.

Our finished sketch

Our finished sketch

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.

The Extruded Boss/Base feature preview

The Extruded Boss/Base feature preview

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.

The part successfully extruded

The part successfully extruded

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.