Learn how to make threads in your 3D models using a helical sweep.
A helical sweep is a very powerful tool most often used for creating cosmetic threads in a CAD model. Whilst Fusion 360 has an inbuilt function specifically for making threads, it’s still a very important function to learn. Take, for example, the giant scale LED project from Issue 27. We needed to design a centre post for the LED to mount an LED strip to. For this, we used a helical sweep using the coil function in Fusion 360.
There is no possible way to make this geometry without the use of a helical sweep. As such, we decided that the coil function should be the next function explored in our Fusion 360 series. A helical sweep or coil in Fusion 360 is a simply a sweep that follows a path around the centre of an object, and can be used to join or cut material. For this tutorial, we will show you how you can use this tool to create your own thumb screw and nut with a custom thread pattern. This will be a good introduction into the uses of the tool and a solid starting point for designing helical sweeps in your own designs.
To get started, we need to build the basic outline of the nut and bolt we wish to create. Select the top view from the orientation display cube in the top right corner. This will allow you to view the part from the top down and should result in the part being created so that it sits flat on the build surface when imported into your slicer program.
Press the ‘C’ button on your keyboard to enter the centre diameter circle tool. Create a circle with a 30mm diameter, with its centre at the centre origin point. After you have created the circle, extrude it 20mm as a new body.
This is the head of our bolt. Of course, if you were so inclined, you could make this a hex head bolt that can be used with spanners or sockets, by using the polygon tool in the sketch. However, since we are designing parts to be 3D printed, thumb screws seem like a much better option due to the lower mechanical strength of the manufacturing process.
With the head created, create the shaft of the bolt. This can be done by pressing ‘C’ again on your keyboard to enter the centre diameter circle drawing tool. Create another 15mm diameter circle on top of the previous extrusion with the centre point at the centre origin, and extrude this by 40mm as a join.
With the general shape of the bolt created, we now need to create the nut. Press ‘C’ on your keyboard to once again, and create a 30mm diameter circle to the right of the bolt. Press ‘D’ on your keyboard to use the dimension tool, in order to make the origin of that circle 35mm from the centre of the bolt along the X axis. Once done, create a second circle with the same centre origin but only 15mm in diameter. Do this by pressing ‘C’ on your keyboard to use the centre diameter drawing tool again.
We then simply extrude the outer circle by 30mm, giving us the shape for the nut.
It’s now time for us to start creating the threads for the bolt. Select the create drop-down arrow in the menu and select the coil tool. Select the top of the bolt end point at the centre origin, and create a circle to match the 15mm diameter of the bolt shank.
Set the type to “height and pitch” and the diameter to 15mm (if it isn’t already).
The height needs to be -40mm to cover the complete shank of the bolt. Let’s set the pitch to -2.2mm, which is essentially the distance between each of the thread peaks or valleys and is the most important defining feature of the thread. Next, set the section to Triangular (external), which sets the shape we are extruding to a triangle that faces away from the centre.
Finally, set the operation to join. This will create a fully custom thread which we will need to repeat on the nut side.
To repeat this process for the nut, select the coil tool from the create drop-down arrow.
Select the centre origin point of the nut’s body and create a 15mm diameter coil.
This time, we need to set the height to -20mm and the pitch to -2.2mm to match the bolt thread. The section needs to be a triangular external, and the operation needs to be set to Cut, to cut the thread into the nut.
You should now have a nut and bolt design that can screw together firmly.
Note: There is no allowance made here for your printer’s tolerances, and in some cases, 3D printing these could result in insufficient clearance to work properly. Usually, the thread will loosen up quite a bit during normal use though.
The current design so far isn’t very useful, as there is no way to use this bolt with a tool due to its round shape.
Therefore, we need to add some grip to the edges and do some general tidying of the design.
We first need to fix the excess thread on the bolt created when we joined the thread to the shank.
To fix this, we need to add a chamfer and extrude a cut on the end of the bolt. Press ‘C’ on your keyboard to create a centre diameter circle from the centre of the bolt. Make this circle big enough to extend past the thread.
Next, press ‘E’ to use the extrude tool, as we want to extrude this as a cut to remove the excess thread.
You will still notice the abrupt end of the thread, which we need to remove so that the bolt can move smoothly through the nut. Click on the expand arrow of the modify menu in the main menu and select Chamfer. Add a 1mm chamfer to the end of the bolt and the leading edge of the thread.
Alternatively, this abrupt thread end can be removed by making the thread complete another 1/4 turn or more past the desired endpoint. To do this, select the bolt head as the origin point and set the distance to be slightly longer than the desired thread. You can then extrude a cut from the end of the bolt to remove the excess thread.
Next, add a 2mm Chamfer to both sides of the bolt head and nut bodies.
Upon inspecting the threads in the nut, we can see that there is also an abrupt end to the thread cut into it. To rectify this, we should chamfer the end. However, this should have been done before cutting the thread.
To rectify this, we can travel back along the timeline to before we placed the thread.
This can be done by clicking and dragging the end position indicator back until before the threads were made. Note that this will temporarily remove all of the progress past the point you move the slider to, however, it will be restored once the slider is moved back.
Once you have gone back to before the threads were made, you can add a 2mm chamfer to the inner edges of the nut.
When you’re done, you can simply slide the timeline back to the right which will re-apply every action to the now modified model.
The very last step is to create the knurling on the bolt head and nut. This will allow you to grip both when tightening or loosening them. The knurling pattern is created using the same coil tool. (This will show us how this tool can be used for other applications instead of just making threads).
To get started, select the coil tool by clicking the create drop-down arrow in the main menu. Looking up from the bottom, select the bottom of the bolt head in the centre/origin point, then left-click and drag out the tool so that it has a diameter of 30mm.
Create a 1mm deep triangular cut into the head of the bolt that only revolves 1/4 or 0.25 revolutions around the axis, as shown here.
We now need to have the same cut made in the opposite direction so that when we create the pattern the two lines cross each other. To do this, we can use the mirror tool. Click the drop-down arrow for the create menu in the main menu and select mirror.
For the object, click the icon in the timeline for the coil we just made. For the Mirror plane, select the Z axis so the new cut will follow the same centre origin, as shown here.
With that done, we just need to create a pattern that will repeat that shape, until it covers the entire surface of the bolt head. To use the pattern tool, you need to select the drop-down arrow for the create menu in the main menu and select pattern, then circular pattern.
For this object, select the coil and the mirror that we just made in the timeline. The axis is the Z axis and the quantity is your decision. We went for 40 to give a fine knurling, but feel free to adjust according to your own preference.
Note: We are creating the physical geometry for a knurl pattern here. This can result in system slowdown due to the complexity, especially after adding a surface appearance. This is only needed when you intend to create a 3D printable model. If you’re just wanting a CAD model and don’t intend to print the object, you can simply give the item the knurled appearance by using the appearance options. This will use significantly less computing power.
You should now have a knurled pattern that is revolved 360° around the bolt head as shown here.
It’s now just a matter of repeating the same process to get knurling on the nut.
If you plan to print, simply export the result as a .stl file and slice and print in your favourite program.
WHERE TO FROM HERE?
Hopefully, this has shown you how useful and powerful the coil tool is. We hope you have a few ideas of how you can use it in your models in the future.
If you’re looking for something a bit more complex, have a go at replicating the varying diameter coil we used in the Giant LED project last month, as shown here.
PART 1 - BEGINNERS GUIDE TO FUSION 360
PART 2 - CREATING CIRCULAR TEXTURED OBJECTS
PART 3 - BLENDING & SWEEPING
PART 4 - RENDERING TECHNIQUES