Sketch and revolve

Tutorial series: Introducing Shapr3D basics


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What you'll learn

Get familiar with sketching, dimensioning, revolved features, and general workflow designing the wheel of a motorcycle. You learn how to set relationships between lines, angles, and shapes to quickly sketch and use the Revolve tool to create a 3D model.



We've been working through the parts in this motorcycle, so we're going to continue by recreating the rear wheel. Now the rear wheel, as you can see, will be a revolved part and it's symmetrical left to right. So we'll be able to get away with sketching just a quarter of it. So let's get started. I'm going to sketch on the front plane.


and I've turned on some settings here that I want to use. I'm snapping to the grid, take advantage of all of that. I'm also using inch units and I have some constraint settings turned on such as auto constraining. There are some limitations to this, which I'll demonstrate right here. I've got the line turned on and you can see that it's identifying the X axis and


as I sketch it identifies the origin and the z-axis and it also gets the vertical and horizontal relationships automatically. There are a couple of relationships it didn't get that that you might hope that it would get and let's let's take a look at those right now. If I grab the endpoint and drag it off the origin it moves okay it didn't pick up an automatic relationship to


and it didn't pick up relationships to either of the axes. So if I want it to stick to the origin, after I sketch it there, I've got to use the lock symbol to lock it in place. Now, if I try to move it, it says lock point can't be moved. That's your sign that it's where it needs to be. It's a good idea when you have an involved sketch, especially sketches that have angles and


arcs in them. It's a good idea to dimension them as you go. So that's what we're going to do here. We're going to use the grid snap to some extent. I'll start at the one inch height level and go to four inches the way I know this should go and draw in an angled line. Now I'm going to stop with escape twice, zoom in,


little bit and apply some dimensions. The first dimension I'm going to apply will be between the center line and the inside diameter of the hub. This is just going to be a radial dimension in the end because this will be revolved and it's a it's half of the actual diameter. And next, we'll apply a four inch dimension. Even if this is what you need it to be, you need to go through the steps of


going through the dialog or just press the lock icon. For example, if I wanted this to be one inch, I could just click on the lock and leave it there. However, I need to change that to 0.5 and put a dimension here between that line and this point. Make that two, we'll just click the lock. Now the next thing I need is, and this arc has to have the center point


on the center line. I want this to be a spherical surface, so I'll just press A on the keyboard to start the arc, and I'll click on a couple of points. I don't know any dimensions right now, so I'll just sketch it in and then start to move things. Now if you, if I didn't have these other dimensions and relationships on, moving this would be kind of dangerous. You can see that that angle isn't behaving very well, so let's...


Let's lock down that angle before we go any further. I'll click on this line, shift click the angled line, get the angle dimension, then we'll call this 30 degrees. Now I can put a relationship between the arc center point, just click on that, and shift click on this line to give those a coincident relationship. Now this allows me to do a lot of different things in a constrained manner.


and this will always remain a spherical surface when it revolves. Let's pull it up here and then give this a dimension.


call this nine inches and we'll give it a dimension off of the center line or center plane as well. So back out a little ways and put this dimension on. This is 4.5 inches. Now everything's locked down. Continue sketching lines. L on the keyboard. Click angled line and I'm just going to leave this as a straight line right now. We'll come back later.


and change it to an arc. But for now, we're just going to roughly sketch in some of these items. We'll get in some more dimensions. Click between these two, make this 120.


and between.


These two.


and make that 20 degrees.


Now I'll convert this end line to construction and add an arc.


I'm going to zoom in a little for this. Hit A on the keyboard to get an arc and place the two endpoints. And then drag this out. This doesn't get the relationships I need. So I'll click on the line, shift click on the arc, get the tangent.


click, shift click, tangent. Now I can add a dimension and this should be quarter inch radius and there's another dimension I need to apply here. That's between the center point and this mid plane. This should be a six inch dimension. Now from here I can change a couple of these other dimensions because


We haven't got a dimension for this line, so I'm just going to move it up and we'll control this dimension from this other line on the rim. I'm not modeling this after an actual motorcycle wheel model that I've measured, but that's not really the point here. The point is to understand a little bit about sketching, dimensioning, revolved features, and general workflow. We'll make this 0.75.


everything the way we want it. We'll just look over this one last time. I'll change this to a three inch dimension. Make it a little narrower in the middle. Two and a half will probably do. And now I want to revolve the part. So the first thing I'll do is hit control one. Control one changes to an isometric view and it pops you out of the sketch and you can see that you have an enclosed area.


with the sketch. You can also see that this time I didn't trim up this vertical line and I left the center line as a regular line, not a construction line. The only construction line here was where I drew this little arc. I'm just doing it this way to show you that there are multiple ways of doing things. So let's use the tools to get the Revolve feature which is the V key on the keyboard.


Select inside the enclosed area, select the center line, and it automatically goes to 360. We can say done. From here, the next video will show you how to add more features to this part.


Try it yourself

Motorcycle cover
Piston rod
Rod clamp
4 motorcycle wheel
Block casting


About the instructor


Matt Lombard is an independent product development professional, working in the field for 30 years. He has done a variety of work from plastics design and surfacing work to writing instructional and reference materials and writing about the engineering technology industry. Matt has also served as CAD Admin, PDM implementor, and engineering process consultant.

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