Creating the Basic Shape
Now that the model is centered, it’s time to start converting it to a CAD model. And we’re going to start by sketching the basic shape of the bottom section.
Go to the Construct menu → Plane through 3 points → Select 3 points across your model → Ok.
Next, create a sketch: Go to the Solid Tab → Click Sketch → Select the created plain.
Now we’ll sketch around the model’s shape from a bird’s eye view. As you can see, it’s a somewhat complex shape, so we will use a few drawing tools to get an accurate sketch. But we’ll start first with the line tool.
Select the Line Tool → Draw lines along all the straight edges and ensure they intersect the line closest to them. You may have to stretch them quite a long way to do this. → Once this is done, right-click on the lines and select Fix/Unfix to keep them in place.
Don’t worry about the curves yet; we’ll get to them soon.
Select the trimming tool and cut off the excess ends of the lines so that they all end at a point.
Now it’s time to change those points into curves with the Fillet Tool. → Select the points and then drag them in to get the curved parts of the model sketched. Pay particular attention to the smaller curves that can be easy to miss.
With all the curves done, we’re ready to finish the sketch and do our first extrusion.
Go to the Solid Tab → Select Extrusion.
To get the right thickness for your model, you will need to use the measurement tool beforehand on your model. The exact settings for the extrusion depend on your object, but you can play around with them and look at your model from all angles to see which options work for you.
Creating Vertical Surfaces
Ok, you might have noticed that the part has a lot of vertical surfaces, don’t worry. We will deal with those next. So, we’re going to sketch the model we’ve just created.
Go to the Solid Tab → Select Create a Sketch → Click the New Model.
This time it’s more straightforward as all our lines and curves are much smoother. As you can see, we’ve not done any intersecting lines this time because we will use another tool to sketch the curves. So like before, draw all the straight lines first.
To deal with the curves, we’re going to use the Arc Tool.
Go to Create → Arc → Tangent/3-Point Arc
Select the line points on either side of the curve, and a line should snap around the bend. You may need to use the 3-point Arc for some of the curves to get an accurate curve.
Once you’ve finished sketching, we will need to offset this line to create the thickness of the vertical parts. So first, we measure the width and height of the highest verticle part.
Inspect → Select Measure, then zoom and carefully select the points on either side of the face you want to measure to make it as accurate as possible.
Now that we know the size, it’s time to offset. Click the Offset button → Select the sketch’s outline and enter the measurement → Click Ok, and finish the sketch.
Ok, now it’s time to extrude the model’s vertical surfaces.
Go to the Solid Tab → Select Extrude → Click on the Offset Outline → Change Operation to Join → Adjust the Size → Click Ok.
When you do this, ensure that “Join” is selected in the operation settings, as we want this to connect to the base plate to form one complete model. As you can see below, we’ve extruded to the highest point on our model because it’s easy to cut it down to the correct size later.
