2010 October

Archive for October, 2010

Creating twisted wire in Solidworks Tips and Tricks.

October 29th, 2010 |

When creating assemblies we sometimes need to incorporate wires or wire harness to have a complete perspective of the design. We need to create a model representing these wires to find out

the proper way to route them. We sometimes encountered twisted wires that are difficult to represent. So here are some tips and tricks in creating twisted wires. Step 1. The first requirement is that you have to have a path to which the wire will follow. We usually do this by a spline curve between two points. See fig.1

Fig. 1

Step 2. Create a plane normal to the curve. And create a sketch and then draw a line depending on the diameter of the wire to be use so they will not hit each other. See fig.2

Fig. 2

Step 3. After creating the sketch use surface sweep to create a surface following your path and under Option “Orientation/Twist type:” choose Twist along Path and in the “Define by: “choose turns, then choose the number of turn depending on your requirement. See fig. 3 and then click OK. See fig.3a

Fig. 3

Fig. 3a

Step 4. After creating the surface that is already twisted create a plane normal to the curve using the edge of the surface as the curve. Do this in both sides. See Fig. 4

Fig. 4

Step 5. Create a sketch and draw a circle that the center will pierce the curve. Do this in both sides of the surface. See Fig.5

Fig. 5

Step 6. After creating the sketches use sweep command and the sketch as the profile and the edge of the surface as the path. Do this one both sides of the surface. See Fig. 6

Fig. 6

Fig. 6a

Step 7. After you are finish on both sides we can now hide the surface that we used as reference and add some details in our wire; like the color, the copper wire at the end of each wire or add connector or crimp at the end of each wire. See Fig. 7

Fig. 7

Note: That you can also do this in a regular solid sweep command by creating two circles in a plane normal to the curve and configuring it to twist, but you will have an unbalance diameter of the wire as the wire twist.

Posted in 3D Modeling, Solidworks |

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How to Create a Screw Thread Flute in Solidwrks

October 15th, 2010 |

Author: Jon Cano

Solidworks usually give us the standard sizes of thread through toolbox. And from smart fastener command we can easily create screws, nuts and washers we need. Screws from toolbox are configured in different standard sizes defends of what we choose during creation.

But do solidworks will give us the screw with correct flute? Or a well detailed screw? Of course not! Because the program need to save memory, simply means creating additional feature means additional memory to be consumed. And this really affects the speed of the program.

It is a fact that in cad designing we do not need a well detailed screw to have a good design. But as wealways say – there is always an exemption. Sometimes we need to show thread flute for presentation or maybe there is a need for us to show it due to some reasons. This article is just a little tutorial on how to
create a thread flute on a screw we got from solidworks toolbox.

Figure 1 shows a standard socket head cup screw (M5x0.8mm) from toolbox.

Figure: 1

Before proceeding, here are the things we need to know before we can create an exact screw threadflute: (1) Type of thread (2) Major diameter (3) Pitch (4) Root depth

Below is the procedure in creating a thread flute:

1. Create a reference plane. Plane distance should be the equal to thread pitch.