This video looks at extruded features based off of a sketch.
- [Instructor] In this lecture I wanna talk about the extrude as well as several various options with the selection intent. So I'm gonna click on the extrude. Now once again, when you go into a function, you're gonna have your selection intent morph the toolbar. So you have to go and make sure that you're picking the correct thing. So if I come over here, just leave everything at Feature Curves. You'll notice I have one sketch. If I pick the sketch, it's going to pick all of the curves of the sketch and you may end up with some peculiar behavior.
I'm just gonna simply select OK and see what I ended up with. I have one extrude. Now you'll note, I'm just gonna hide this main body. So I'll take you and hide everything except for that little surface. Now that little surface is the result from that sketch. Why? Let me show that sketch. You'll notice that I have a curve that's kind of floating out in the middle of that sketch. When I extruded the entire feature, well it's part of the feature, it has to extrude that.
So it just made a surface a sheet body. All right, how do I not get that? So I'm gonna undo, undo, undo, go back to this point. When I do my extrude, instead of Featured Curves I can use what's called Connected Curves. So when I come in here, if I pick this you'll notice it just picks the connected curves. It ignores that hole in the middle. It ignores that fillet. So in this case I'll just end up with a final solid volume. All right, I'm just gonna cancel, restart the menu.
I'm gonna go back into extrude. This time I'm gonna go into Connected Curves and I'm gonna use what's called Follow Fillet and there's another tool here called Stop at Intersection. I wanna turn these two on. And the reason why I wanna do that is, is when I pick my sketch now, you'll notice I get a different behavior. The stop at intersection is telling it stop where the two lines come together. That's technically an intersection point. And the Follow Fillet is saying, hey if it's tangent, continue along that tangency.
So now I can basically pick one curve that tells the extrusion, again, remember these selection intents are built into the feature, to follow that fillet, stop at that intersection, follow that fillet, and work it's way around. If I pick another curve, like this circle in the center, you'll notice that there's no intersections, there's no nothing, it just goes ahead and does what it's supposed to do. I'm going to select okay and create that extrusion. Now I'm gonna go back in and make a modification to that sketch. I'm gonna move this out to here.
I'm gonna finish and I end up with something completely different. Now you'll notice I have two bodies. Those two bodies are because I have basically two different profiles now. All right, when I picked this, I picked two different profiles. I did outer and the inner. Well when that sketch was wholly inside, that circle was wholly inside the initial outer profile, it recognized it as a hole. Now that it's outside of that profile, it doesn't recognize it as a hole any longer, it recognizes it as a separate profile to make an extrusion out of.
So this is what I mean by selection intent. You wanna make sure that you build that intelligence into your feature correctly. Just be cautious when you're sketching and when you're extruding revolving anything that has heavily to do with the selection intent. To make sure that you use the correct intent for your selection, because you can end up with different results like this. I'm just gonna undo that, undo that. Now here, I'm just gonna go back into extrude. I wanna use again Connected Curves.
I'm gonna use the Follow Fillet along with my Stop at Intersection. Gonna pick that curve. I get exactly what I want. Once again, I can adjust the height, positive and negative directions. You'll notice if I go in the opposite direction it's a negative value, if I go in the same direction it's a positive value. I also have the ability to use a symmetric value. So if one side grows, the other side grows as well, symmetrically across the plane. You have different options that you can select surfaces or other faces to trim up to as well.
We'll come down. Boolean, once again this is what can potentially happen to solids that share a similar space. We'll be talking about this. Come down, below that, you also have the ability to apply a draft. So if I click on draft I can say from, in this case, start section. So the section curve is driving the draft. You'll see I have now angled walls on that and I can go ahead and change this any way that I need. You have other options in here. From Start Limit. In this case the Start Limit is this top up here or I apologize, this bottom down here.
This is starting here and it's drafting in from there. So if increase this, it maintains the start limit. It's no longer looking at the section as the start for the draft. You have asymmetric angles as well. So you may be able to draft top and bottom differently, castings, forgings, that type of thing. Switch that back to none. You also have the ability to do offsets, single-sided, two-sided, symmetric. So if you're building a wall, like in this case, I'm just gonna do symmetric. This is just gonna measure off of that initial sketch as its neutral element.
So it's coming off the center point. And I can again do a symmetric by doing a single-sided or two-sided, whatever it is I need. And let's change this back to none. Come back down to the settings at the very bottom and once again if I need a sheet, I can switch that to Sheet to get a surface. Select OK and there's my solid body. So once again, whenever you're doing extrude, any of these features that require you to pick a section, you wanna make sure you have your selection intent set correctly and from that, once you have that set correctly, then worry about what's going on inside the menu, because what you pick will definitely affect everything downstream, how you pick it, what features you have set for selection intent as well.
- Navigating the user interface
- Creating and editing a sketch
- Creating and modifying curves
- Using tools to measure objects
- Building an assembly
- Making contextual edits
- Inserting parts into an assembly