Joel Dalida

Author Archive

Repairing Surface in Solidworks:

February 18th, 2011 |

Have you ever encountered a surface in solidworks that is deformed or not smooth enough? This usually happen when converting it into a different file format. Well I have a sample that needed some work because some faces are not the way they should be.

(See fig .1)

1. First we should identify what causes the surface to deform, like the tangency of the curves.

Fig. 1

2. After knowing the problem which is the tangency of the curve use before, we should now create a new curve.

As you can see in (fig. 2.1) the difference between the new curves form the old. You could use any of the “curves command” like composite curve or curve through points. After creating the curve you can now delete the surface to be replaced by using the command “Delete Face”.

3. Now that the curves are all done we can now create a new face. We can now do the other faces

4. You could do it in the half part so we could just mirror it and knit it.

• All done!

Posted in 3D Modeling, Detailing, Dimensioning, Drafting / Technical Drawing, Solidworks |

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Creating twisted wire in Solidworks Tips and Tricks.

October 29th, 2010 |

Author: Joel Dalida

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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