Learn how to create the Neck component in a detailed project using the Solid menu. This process involves creating a new component, establishing a construction plane, and executing a series of steps to create and define the Neck component.
Key Insights
- The Neck component is created between the fork and the folding bracket using a New Component option in the Create menu from the Solid line in the project browser.
- The creation process involves constructing an offset plane, defining dimensions, and establishing various construction lines to set the angle and foundation for the Neck component.
- Finalizing the Neck component involves sketching, creating geometry, and defining the tube path using the Pipe option in the Create menu, setting parameters to make it hollow, and saving the created components.
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Now let's create the Neck component. The Neck component sits between the fork and the folding bracket. In our project, let's go ahead and go back to the Solid menu and let's make sure that our top line is currently active in the project browser.
With those two steps, we can go to Create and select New Component. That New Component will give it a name and we'll call it Neck. The parent should be our top line of the project browser and we will click OK.
So here we are in the Neck component and we want to start by creating a construction plane. We'll go to the Construct menu, select Offset Plane. We'll click the center plane with zero offset and click OK.
So there is the center of our Neck. Now we want to create a sketch. We'll go to the Create Sketch button and open up our Neck component.
Look for our construction and click that New Construction Plane. We can select the Line tool and zoom into the center of our wheel hub. We'll click one time right in the center of our wheel hub and we'll pull our cursor straight up.
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Now we can type in some dimensions. We'll do 110 millimeters and click Tab on our keyboard to lock that distance in. And then our angle will be 106.
And we'll notice that places the line directly at the top of our fork. That's what we're trying to aim for. We'll go ahead and click Enter and we have this line.
Now we're not going to use this line to create geometry. We will select it, right click on it, and turn it to Normal Construction. So that essentially gives us two construction lines.
A line going out from the wheel hub and a line going up. That lets us set our dimension for our angle. It's 106 degrees, which sets us up for the 16 degree offset from vertical.
Everything will be created for our stem, handlebars, everything going up. Alright, with this let's create a couple more construction lines. We'll go back to the Line command, click right here at the top, go to the right, and just move our cursor out.
We'll type in 15 for 15 millimeters. We can hit TAB to lock it in and then type in 16 degrees and hit ENTER. There we go.
We've got that line and we'll select it, right click, and make it a construction line. What we're creating so far is a base and everything needs to be 16 degrees on an angle and so this helps us have a solid foundation. Now we can start to create some of that neck.
We'll go up to this Line command yet again, click right here where we left off in this tall line, and this time we're going to go up. Instead of hitting Tab this time for the degrees, we can notice that we have a perpendicular constraint. It looks like a small blue square, lets us know that we're moving perpendicular straight up.
We'll type in a dimension 5 for 5 millimeters and Enter. That takes us 5 millimeters off the top of our fork and again we'll turn that into a construction line. Now from here we're finally getting into a line that we're going to use.
It's just a lot of setup to get us here. We'll click the Line command again, we will click one time where we left off, go straight up, and we'll notice that parallel constraint. It looks like double blue lines.
We are going in a parallel direction and we can type in our dimension. It'll be 105 millimeters and if everything looks good, we're sticking straight along our path, we can click Enter. Okay, so there is a line for our neck.
Let's go ahead and click Finish Sketch and now we can create our geometry. Under the Create menu, we're going to go down and look for Pipe. The first thing that we do in the Pipe window is select our path.
We'll click on that blue line that we created and we'll notice some defaults start to show up like 50 millimeters and our distance. So let's go through these. Distance of 1 means going from end of line to end of line.
If we were to type in like 0.5, it would only go halfway. We'll keep that at 1. Section Circular, we'll leave that alone. Section Size will be 30 and we want to make this hollow.
I'm going to orbit up so you can see what it is right now. It's a solid tube. I want to select the hollow and that gives us a few more options here.
Right now we have the section thickness of 3 and that looks good and the operations new body. If everything looks okay, we'll click OK and there we go. We've got the first little portion of our neck.
Now let's do some housekeeping here. First in the Neck component, we have our Construction Plane. We'll call this Neck Center and we have our Sketches.
In Sketch 1, we'll call it Tube Path. It's a Tube Path and then in Bodies, we have Body 1 and we'll call this Neck Tube. And with that, it's a great time to hit the Save button.
