It’s always great to get feedback and requests for content and following our last blog, we got a request for an example of detailing the end of a spring with some closed coils and hooks or tabs.
Here’s an example of one way that the tools in SOLIDWORKS can be used to create a more advanced spring end including some closed loops and a small tab. The tab can be made as simple or complex as you need it to be, the process would still be the same.
Firstly, I started with some circular sketch geometry centred at the origin of the part to create a Helix. But this time, in the options for the Helix instead of making it a constant pitch, I chose to make a variable pitch Helix. A table is displayed in the property manager and SOLIDWORKS will generate a Helix with a smooth transition between pitch values at the specified revolution counts. It is important to allow for this in the table by specifying a number of revolutions at the same pitch and then a smaller number of revolutions for any change in pitch.
In this example I have applied revolutions 0-3 with a 3mm pitch, then in the space of one revolution (3-4) the pitch changes to 12.5mm. The pitch stays at 12.5mm for 6 revolutions (4-10), and then it reduces to 3mm between revolutions 10 and 11. Finally, there are three more revolutions at 3mm (11-14) to keep the spring symmetrical. You may also notice that you can also control the diameter of the Helix. This allows you to create tapered Helices.
Because I centred my circular sketch at the origin, my Helix is also centred at the origin. This makes it easy to put in a centre line on one of the standard sketch planes as reference geometry.
From this centreline sketch, a reference plane can be added by selecting the line and the end point to fully define the reference plane. This reference plane is to be used for creating geometry that is flat to the end of the spring rather than angled like the Helix.
Next, a sketch can be drawn onto the newly created plane to define the tab at the end of the spring. In this example, I created a centre-point arc based at the origin with no dimensions. This is because I want to relate the arc to the Helix. You will need to rotate your view slightly to be able to select the arc and Helix end points and then add in a ‘Pierce’ relationship to connect the two pieces of geometry.
Next, I added in the detail for my tab at the end of the spring. I have created this all in the same 2D sketch, but it is possible to create a new 3D sketch to allow for any possible tab geometry.
This process can then be repeated at the opposite end of the Helix.
Once the opposite end of the Helix has been added to, the spring is nearly ready. However, at the connection between the Helix and the flat sketch for the tab, there is a change in angle which may cause a small ‘kink’ in the end of your spring.
SOLIDWORKS has a sketch tool that will automatically neaten this up for you with very little input.
Generate a new 3D sketch and go to Tools – Spline Tools – Fit Spline. This tool will generate a single spline curve that mimics the geometry that you select to a tolerance that you specify. By selecting the sketches at the top and bottom and also the Helix curve, and making the tolerance value sufficiently small, the spline that is generated will exactly match the desired spring. Increasing the value of the tolerance will ‘round off’ any sharp edges or corners such as the connection between the Helix and the 2D sketches. In the property manager, deselect the option for ‘Closed Spline’ as this will attempt to close the loop between the 2D sketches.
The resulting geometry is a single spline curve that is fully defined that we can use as a sweep path for the spring. A little tip at this point is to hide all of the unrequired sketch and reference geometry by selecting it in the Feature Manager Design Tree and selecting Hide. This not only keeps your graphics window nice and tidy, it also makes for easier selection when using the spline for feature use.
Next, a reference plane was easily created by selecting the spline and one of the end points of the spline. This generates the ideal reference for creating a sweep profile sketch as it is perpendicular to the spline that we will use for the sweep path without having to work out any angles or measurements.
For this example I sketched a circular profile of 2.5mm diameter.
Lastly, in the Command Manager, choose Swept Boss/Base. Because all of the preparation work has been carried out and only two sketches are visible in the graphics area, it is simply a case of selecting the circle as the Sweep profile and the 3D Spline as the Sweep path to create your spring.
Duncan Crofts CSWE is an Elite Applications Engineer at TMS CADCentre.