SolidWorks is one of the most popular CAD software when it comes to 3D modeling and here is a quick tutorial that will help you have a glimpse of what modeling is like while working with Solidworks
As the many CAD exercises we worked on here, we will start with having the target image information to lessen the burden while modeling. Here are the info.
In Solidworks, we have three environments which are part, assembly, and drawing. In this tutorial, we are going to use Part section.
Right click on the Front Plane from the Feature Manager design tree and select a Sketch.
Click on the Circle command and click on the center of the Coordinate system. In Solidworks, you do not need to give dimensions when you draw. So, first, finish sketching, then select the Smart Dimension and give it 77 mm.
Now, draw the centerline and normal line as shown in the image below. Select the Smart Dimension and select two lines and put 15 degrees.
Let’s use the mirror command.
Mirror Entities Command >> Entities to mirror = Select line 1 >> Mirror about = select centerline
Now, draw another circle with 65 mm as a diameter and click on Circular Pattern
Click on Circular sketch pattern >> First select center point >> Second Select two lines
Extra lines should be removed from the Sketch
Trim Entities>> trim to closest >> click on extra lines
We need new center points. First, draw three centerlines to give dimensions. Use the Smart Dimension and click on the two lines. Then draw a circle of diameter 65 mm but we need this circle for construction. So, activate for construction (Number 2).
Draw two circles with a diameter of 5mm in center points that we found from previous steps and then use the Circular Pattern to copy it on your sketch.
Go to features tab and select Extrude then give 10 mm of Thickness. Instead of Blind, you can use the middle plan, then Solidworks will give the same amount of thickness to both sides.
The purpose of this section is to make another sketch. To do that, first Select the highlighted surface and click on Sketch.
Change the view.
Draw a circle with a diameter of 25mm and centerline the same as the following picture. To copy centerline use Offset entities and give 2 mm offset from each side.
Draw a straight line and then remove extra lines by using the trim entities command.
After removing extra lines, use circular pattern and select three line and copy it 6 times.
You cannot have more than one sketch when you want to extrude a sketch. It means that your sketch should start from one point and come back to the same point. So, before extruding the second sketch, you need to remove the extra line to have one sketch. And then extrude the sketch (Thickness=15 mm)
Make another sketch on the highlighted surface and draw a circle with a diameter of 15 mm.
We want to subtract a new sketch from the model. For this first click on extrude-cut and then select the sketch. You can give the dimensions with the Blind method or you can select through all.
Through All: Extrude a feature through all the other bodies in the model.
We can now make a drawing for this model. First, you need to save your model, then click on New >> Select Make Drawing From Part and then select the desired sheet. To see drawing: View Layout >> Standard 3 views >> select part