Explore how to use patterns to prevent complex assemblies from slowing your computer.
4-5 sample file here which is that simple table we created in the previous video. Double click on the sketch at the bottom to go into the profile for the table and for the legs. If you notice here, each one of these legs has a five millimeter offset from the edge at a tangent offset. If we click on sketch dimension So click on each one of the circles and delete them. Now we have our table right here. We're going to be using in this video a combination of the mirror command and the pattern command. And I'll show you when you would use each. In this case we'll be creating some mirrors. So create a center diameter circle. So click on center diameter circle up here and go to one of the corners, I'm choosing the top left. Now also notice that if I want to create the circle right around here, the mouse is snapping to this line which is automatically created with the center square command or center rectangle. If you don't want your mouse to just jump to that, you can hold down the control key, or command key on a Mac. The control key will make no snapping happen, so no matter where you move your mouse it will not snap to anything. So I'm going to click right around here and now I can let go of the control button. And say, 10 millimeters. Kind of a small leg. But we will change that later. And now I can drag this to exactly where I would want that to be. All right that looks pretty good. Now what I want you to do is go up to the line tool up here, and create two lines. Click on the center, and go up, and then click the little check box to end the line. And then the center and go to the right. Any distance. And then press escape to exit that tool. Now you have these two little floating like right here. And we're going to be using these as mirror lines. So go to create, down to mirror. And again we're still in the sketch environment, so we have a create mirror command for this sketch. And what that does is it wants what object, we're going to select object right here and select our circle. And the mirror line is going to be this horizontal line right here. And click ok. Now we can see that we have a circle down here. And do the same thing. Say create mirror again. And this time we're going to select as our starting objects both of these, so the original and the mirror, and the mirror line is going to be this vertical line and you click ok. Now have these. Now a change to one is a change to all others. Because they're being mirrored up and down and left and right. And these mirror lines are going to be important for another operation that we're going to be doing later. So make these are you want. And again, these are completely mirrored. If you double click and change this to 15, note that all of them change to 15. So do that now, please change that to 15 so that we have a little bit more room for what we'll be doing later, and then click finish sketch. You notice we have a yellow marker on our extrude operation. Because we deleted the previous legs and added in new ones. So for right now you can right click on this operation and just go to delete. It kind of overflowed my screen on the bottom. But right click and delete so that you just have the sketch But there may be times when you have 10 faces or a hundred faces that you would want to make a pattern of and it would be too onerous to click each one. In that case you would go down to features, and what features allows you to do is instead of up here in the modeling window, you would go down and say, I want to make a pattern of this extrusion. So you click on the extrusion down here. If you can use this features command then it's better to do that because it's computationally less intensive to create a pattern of this rather than having Fusion try to make two, four, six, eight, 10 different faces. This is easier for Fusion to do. Anyway, so we have selected the object. Now the axis, all cylinders have a default axis in the center of them. So if you just click on this, Fusion knows you want to create it around the axis of the cylinder. And change quantity to five. Now you can't really see it, you see something's kind of going on up there but once you click ok, you will get a full cutout. Isn't that an awesome looking table leg? Now how do we get this table leg to the other sides? Well you guessed it, we can use the mirror command. If you go to create, down to mirror, you can create a mirror of things inside the solid modeling environment. Notice, we're not in a sketch, this is in solid modeling. You go to create and mirror. Now I said if you can use features, you should. But in this case it's not going to work, I'll show you why. You don't have to follow along, you can just kind of look. If we have pattern features and we say; okay, let's mirror this pattern across a plane. And we say, okay, we get most of it but not the original extrusion. We get one, two, three, four, but not the fifth. So if we go back here we have a different option for identical, if we click on that, still the same. We have our last option right here, is optimized. Also does not work. That is because we are not creating a mirror of the initial extrusion. So you may think that we can go back in and say; ah, let's click on the initial extrusion. If we've got that as a feature. And now let's click on the pattern. Well we can't mirror the pattern, sadly, I wish Fusion could. But, I believe it's because this is based off of something that's here and you can't mirror down the timeline. Because this is based off of this, you can't run a single mirror command. So what we'll need to do is switch this to faces. And we can kind of orient our view here and drag select here. And that will select all of the objects. Now, notice, that when we drag select from right to left we select everything, which is not what we want. And I explain this in other videos in this series. There is a difference between right left dragging and left right dragging. In this case dragging from the left and going to the right will select only the things that are completely inside of this box. In which case are just the faces that we created. And now we would want the mirror plane. If it doesn't pop up you can turn back the origin, the mirror plane to be this plane right here and say ok. Now, let's look at the bottom, perfect. We have a perfect cutout, perfect cutout. Now we can do the same thing, create another mirror. So go down to create mirror, and we can say faces again, drag on these and mirror them over. Like that. Now this is a way of doing all of the legs like that in a technical sense you would only need to model half of this table. And have a mirror command right at the end to make the other half. You don't really need to model the other half of a symmetric shape. But in this case we did so, but there's a lot more timeline commands here rather than just modeling one of these shapes or one side and then mirroring over. But the pattern command and the mirror command exists both in the sketch work space as well as in the solid modeling. You could create a rectangular pattern of more legs if you wanted. If you wanted to add in more legs here and you didn't want to create sketch objects. You could do all sorts of things with patterns, as well as mirrors inside of both environments.
Note: This course was created and produced by HoneyPoint3D. We are honored to host this training in our library.
- Creating basic shapes
- Using Fusion 360 environments
- Extruding profiles to create objects
- Surface modeling
- Editing via the timeline
- Editing and combining shapes
- Analyzing your work
- Exporting models