Thread for Screw Tutorial/it

This tutorial is a collection of techniques to model screw threads in FreeCAD. It was updated for v0.19, although the overall process has been essentially the same since v0.14, when the tutorial was originally written. The updated content focuses on the PartDesign Workbench to create the thread, but does not use the PartDesign AdditiveHelix tool as this was introduced later.

Many of the techniques presented here have been collected from different forum threads:

• Gathering thread modeling techniques
• Creating a thread: Unexpected results

See also helpful videos:

• Introducing a strategy for designing a bolt without the commonly found problems.

Remember that thread shapes take a lot of memory, and having just one thread in a document can increase the file size significantly, so the user is advised to create threads only when absolutely necessary.

Using utilities and parts that other people have created is easy and saves time. See the external workbenches page for information on external tools.

In particular, three resources are recommended that can be installed from the Addon Manager:

• Fasteners Workbench, to add/attach various fasteners to parts. The screws and nuts don't show a thread by default, but this can be controlled with an option.
• BOLTSFC Workbench, to place fasteners from the BOLTS library.
• ThreadProfile Workbench, to create common threads.

Various standard screws inserted with the Fasteners Workbench. An option controls whether an object shows the real thread or just a plain cylinder.

• In the past, the Macro BOLTS was used to insert the parts from the BOLTS library. This is now deprecated. Use the BOLTSFC Workbench instead.

• In the past the stand-alone Screw Maker macro, by ulrich1a, was used to create individual bolts, screws, and washers. This is now deprecated. The Fasteners workbench, by shaise, includes the complete screw maker macro, together with a GUI to select the right component.

In many cases we don't need real threads, we just need a visual indication that the threads will be there.

Left: simple bolt with a fake, non-helical thread. Right: simple bolt with a real helical thread. When 3D printing is not needed, a simulated thread is often sufficient for visualization.

Revolving sawtooth profile

1. Click on PartDesign Body.
2. Click on PartDesign New sketch. Select XZ_Plane.
3. Draw a closed sketch with the required inner diameter 10 mm, outer diameter around 12.6 mm, pitch 3 mm, number of teeth 8, and total height 30 mm.
4. Select the sketch, then click on PartDesign Revolution. Select Vertical sketch axis, and press OK.

Profile used to create the revolution that will simulate a thread.

Sectional view of the resulting non-helical thread produced by revolving the sawtooth profile around the vertical axis.

Stacking discs

1. Repeat the first two steps from the previous section.
2. Draw a closed sketch with the required inner diameter 10 mm, outer diameter around 12.6 mm, and pitch 3 mm, but draw only a single tooth of the sawtooth.
3. Select the sketch, then click on PartDesign Revolution. Select Vertical sketch axis, and press OK.
4. Select the Revolution, then click on PartDesign Linear pattern. Select Vertical sketch axis. For a fake thread with a pitch of 3 mm, set the Length to 3, and Occurrences to 2, then press OK. This will create two discs, one on top of the other.
5. You can add more discs by increasing the value of Occurrences in the linear pattern, and by raising the Length, which is the total length of the fake thread.

The Length and Occurrences are related. If the length is too large, but the number of occurrences is not high enough, you will have disconnected discs, and the Body computation will fail, as the resulting object must always be a single contiguous solid. For example, to get a total height of 30 mm, set Length to 27 mm and Occurrences to 10.

If you wish, you may add a PartDesign Additive cylinder with a diameter equal to the inner diameter of the discs, and as high as the total thread height. This will join all discs into a single solid, thus guaranteeing that there will not be disconnected discs.

Profile used to create a revolved disc that will be used to simulate a thread.

Left: single disc created by revolution. Right: multiple discs placed in a linear pattern in the Z direction simulating a helical thread.

PartDesign Workbench

A true thread consists of a closed profile sweeping a solid along a helical path.

1. In the Part Workbench, click on Part Primitives to create a Part Helix. Give it the appropriate values for Pitch 3 mm, Height 23 mm, and Radius 10 mm.
2. Move to the PartDesign Workbench, and click on PartDesign Body.
3. Click on PartDesign New sketch. Select XZ_Plane.
4. Draw a closed sketch with the required profile for the thread teeth, normally a triangular shape. In this case we will use a height of 2.9 mm, which is slightly smaller than the 3.0 mm pitch used for the helix path. The profile must not create any self intersections when moved along the helix, neither between the turns nor in the middle, thus the sketch as shown for stacking disks cannot be used.
5. Select the sketch, then click on PartDesign Additive pipe. In Path to sweep along, click on Object, and choose the helix object previously created. Then change Orientation mode to Frenet so that the profile sweeps the path without twisting; then press OK.
6. When the dialog asks for a reference, choose Create cross-reference.
7. The helical coil is created, but there is no central body or shaft.
8. Click on PartDesign Additive cylinder with the appropriate Radius 10 mm and Height 29.9 mm to touch the rest of the helical thread and automatically fuse to it.
9. Additional boolean operations are needed to shape up the abrupt ends of the coil. For example, you can use additive features to provide a head to the screw, and a tip.

Left: profile for a helical thread. Right: helical path that will be used to create a sweep.

Left: helical coil resulting from the sweep operation of the closed profile along the helical path. Right: sectional view of the coil produced from the sweep.

Left: helical coil fused to a central cylinder to form the body of the screw. Right: more features, a head and a tip, added to improve the shape of the screw.

Part Workbench

This process can also be done with the tools of the Part Workbench.

1. In the Part Workbench, click on Part Primitives to create a Part Helix. Give it the appropriate values for Pitch 3 mm, Height 23 mm, and Radius 10 mm.
2. In this case, you don't need a PartDesign Body. Switch to the Sketcher Workbench, then click Sketcher New sketch, and choose the global XZ plane.
3. Then return to the Part Workbench, and use Part sweep.
4. Select the appropriate sketch from Available profile and click the arrow to pass it to Selected profiles.
5. Click Sweep path, and choose all edges of the existing helix in the 3D view. Click Done.
6. Make sure to tick Create solid and Frenet. Obtaining a solid is the key to be able to perform Part Boolean operations with the resulting coil, otherwise only a surface will be produced.
7. Click OK to exit the dialog and create the coil.

• Rule 1. When the profile sweeps the helix, the resulting solid coil must not touch or self-intersect as it will be an invalid solid. This holds for the profile moving along the helix, as well as intersections in the center of the helix. Attempts to do boolean operations with it (fuse or cut) are very likely to fail. Check the quality of the coil with Part CheckGeometry; if self-intersections are reported, you must increase the pitch of the helix.

• Rule 2. When a cylinder is added to a coil to form the main shaft of a screw, the cylinder must not be tangent to the coil profile. That is, the cylinder must not have the same radius as the inner radius of the thread, as this is very likely to fail a fuse operation. In general, avoid geometry coincident to elements of the sweep, such as tangent faces, or edges tangent to faces they are not connected to. In order to produce a good boolean union, the swept coil and the cylinder must intersect. Check the quality of the fusion with Part CheckGeometry; if coplanar faces are reported increase the cylinder's radius by a small amount.
• If the coil and the cylinder are tangent, even if the first fusion succeeds, it may fail in subsequent boolean operations with a third solid.
• This is a limitation of the OpenCASCADE Technology (OCCT) kernel; in general, it doesn't handle well operations between coplanar surfaces.

• Rule 3. The inner cylinder has a seamline. You should avoid placing the start of the helix along that seam. Either turn the helix or the cylinder by some degrees.

• Tip 3. For 3D visualization and 3D printing it may be okay to leave the cylinder and the thread unfused, that is, with intersections between the two solids. Reducing the amount the boolean operations results in less memory consumption and smaller files.

General

Figuring out the horizontal profile to obtain a certain vertical profile is not easy. For simple cases like triangular or trapezoidal it can be constructed manually. Alternatively, it can be constructed by creating a short thread with method 4, and getting a slice of it by doing a Part Common between a horizontal plane face and the thread.

1. First create an Archimedian spiral in the XY plane.
   1. Set the number of turns to 0.5.
   2. Set the radius to the inner radius of the thread, the outer radius will be this plus the depth of the cut.
   3. Set the growth to double the depth of cut of the thread.
2. Part Mirror the spiral against the XY plane
3. Part Fuse the spiral and the mirror to obtain a closed wire, shaped like a heart.

• a ready-to-use thread-on-a-rod solid shape is created by the sweep directly.
• fewer or even no boolean operations are required, so generation speed is very high compared to Method 4.
• thread ends are nicely cut straight away
• long threads are not a problem, unless a boolean operation is needed. Otherwise, it is not going to be much better than Method 4.
• threads without a gap are not a problem.

Le Spline elicoidali estrudono delle facce coassiali che possono essere usate per un loft, mentre l'elica parametrica di FreeCAD no. Per definire una filettatura servono due spline elicoidali. Esse possono essere prelevate da una libreria di spline, poi posizionate ed estruse in modo appropriato per ottenere la giusta forma.

Le eliche parametriche di FreeCAD non sono veramente elicoidali, ma non è difficile tracciare delle b-spline elicoidali. Un metodo manuale consiste nel creare delle matrici dodecagonali (poligono di 12 lati) con 5mm di raggio, o 10mm di diametro, a intervalli z di 1/12mm (0.08333.mm) e tracciare una spline da vertice a vertice in ordine ascendente e rotazionale. Considerare di costruirle, ad esempio, per 10 giri, e poi archiviarle come file di una libreria in modo da poterle importare e riutilizzare. Per comodità di ridimensionamento, conviene usare un diametro di 10mm e un passo di 1mm. Fatto manualmente, è più facile disegnare una Dwire e poi convertirla in un b-spline che disegnare direttamente una spline. Nelle linee Dwire non viene calcolata la curvatura mentre vengono disegnate, quindi seguono meglio il cursore e obbediscono di più all'aggancio.

Once the splines are scaled to the right size and located so that the loft will have the right included angle between the thread flanks, they're extruded along their axis, a pitch length's worth for the inner spline, the outer pitch/8.

ISO e altri thread hanno alleviato, cioè bordi piatti, interni ed esterni piuttosto che affilati, il che si adatta agli utenti di FreeCAD con questo metodo, perché possiamo loft alla faccia elicoidale alla dimensione nominale del fissaggio, mentre una faccia interna non può essere loftata una spline del bordo esterno perché una faccia è un profilo chiuso, una spline è aperta. Lo standard ISO afferma che le dimensioni nominali dei filetti esterni hanno un passo della larghezza della faccia/8. L'immagine mostra come è organizzata la geometria e le facce elicoidali che ne risultano. Quindi, ai fili viene aggiunto un loft tra le facce e quindi un cilindro che dà la faccia elicoidale interna, che ISO mette a passo/4 di larghezza.

Questo metodo produce solidi affidabili che booleano correttamente. Sebbene non produca filettature "parametriche" in dimensioni standard nel senso di avere un accesso semplice alla forma in base alle dimensioni del dispositivo di fissaggio, è un modo semplice di produrre una libreria accurata per il riutilizzo e modelli di forme specializzate come ACME o viti Archimedian , sono anche semplici come one-offs.