説明
主な学習内容
- Learn how to produce machine components using the load requirements to establish what geometry will work
- Learn how to place clearance holes through components after calculating the fasteners required to hold the assembly together
- Learn how to choose a standard belt size and position pulleys based on power handling requirements
- Learn how to create meshing gears based on the loads without having to draw the gear features
スピーカー
- TTThom TremblayIn 1988 Thom Tremblay became convinced that a 3D model should be used as the primary way to create the 2D drawing he needed. The next several years working as a drafter and mechanical designer in shipbuilding, planning, casework, commercial electronics, and centrifugal compressors eventually led Thom using his skills to teach others. With over twenty years of experience consulting with businesses and education institutions of all types and sizes, Thom has developed an understanding of how people use and learn technologies. Thom also holds professional certifications in Autodesk AutoCAD and Autodesk Inventor, and is an Autodesk Certified Instructor. Thom has authored several books and online learning content on Autodesk Inventor and is authoring online learning content for Fusion 360.
THOM TREMBLAY: All right. OK. So this will be a hands on lab. There's extra computers so you don't have to share. So feel free to spread around. Chances are these computers up here have not been used all week. So feel free to live on the edge there.
Yeah, so we'll get started here. So how many of you have not been in a lab yet this week? OK. So on the desktop, there will be a folder. Let me see if I can navigate through this with you. See if we have a nice transition. Oh, yeah. Cool. All right. Let's see if it's this zero data sets.
So blended in a very small number of courses is this one. It will be down-- well, if I just looked up the number myself. OK. MFG 321419 hut. So in there will be a handout and the data sets that we'll use. And what I'll do, or what I recommend doing, is-- of course, you can use Alt tab to hop back and forth between Inventor and the handout. I'll also have a video, more or less, of the instruction going on.
So what we'll do is we'll cover the topic. Then I'll show you kind of what I'd like you to do. And then you'll have the handout and the video to refer to. So as I'm going through things, I'll be explaining some options and talking about some other things. So rather than trying to follow along while I'm doing that, please just kind of watch, and then we'll give you some hands on time.
There's a decent chance we won't get through everything. But let's see how far we can get and how much material we can get through. So hopefully we'll be able to get through most of it.
So my name's Thom Tremblay. How many of you have been using Inventor more than a year? More than 10 years? More than 15 years? All right. Couple, yeah. So I started using Inventor in alpha, so a little more than 20 years ago. Inventor's crazy, crazy, crazy powerful software, just incredibly rich. Serves a lot of different industries.
What we're going to be focusing on today, though, is really focusing on machine design elements of it. So bearings, belts, bolts, gears, that sort of thing. And We'll also get into a little bit of frame generator, hopefully, at the end. So managed to put together a couple of books and a lot of video lessons on Inventor and a few other things, AutoCAD Electrical Fusion.
But one of my favorite things in Inventor are the design accelerators. And I was asked a question the other morning, how are design accelerators like generative design? Everybody keeps generative design, generative designs. Big buzzword last few years. And I honestly hadn't given it any thought. But in all reality, the two are very closely related in concept.
So generative design is the ability to use simulation inputs and results to create unique geometry to solve a problem. Design accelerators, you put in your engineering requirements, and the computer can tell you what standard components, things you would purchase, or maybe with gears, you might make a unique gear. But the tooth profile is most likely going to be based on a standard that's been around for 150, 200 years.
So the two are very similar in the idea that the computer can help assist you and guide you in the process of designing. So today we'll talk about the overall concepts of why designer accelerators, take a look at shaft energy, gear generator, belt drive, bolted connection, and metal frames. And hopefully we'll get through all that if I stop talking.
But the basic thing about design accelerators, there's two primary types of tools. There's generators, which will create geometry, either bringing in a component from a library or by helping you develop teeth on a sprocket or items like that. They can use calculators to select what that geometry will be. And then there are calculators, which are just standalone tools which will tell you the sorts of objects you need, how much braking surface you need on a disk brake to stop this amount of power.
But you have to come up with that geometry because that's something that is probably going to be unique component, or it could be a specialized design based on your manufacturing processes. So do you recognize that dividing line? Something very cut and dry, something that you would probably use the machinery handbook to use. But you're still going to have to come up with the geometry to solve the physical problem.
In fact, that's one of the other features of design accelerators is there is a handbook built in that will show you what formulas and calculation processes are used to determine the results that you're given. So you can compare that to the processes that you use. Sometimes there are alternate formulas that you might be using. And you can see how it's done, see if it jibes with how you're approaching it, and how you want to address it.
All right. One last note. As we start creating things, if you decide that you want to get rid of something that was created using a design accelerator, or as we go to modify it, don't try to use the standard delete tools in Inventor or any double-click to try and edit it. We want to use the special Edit Design Accelerator component or Delete Design Accelerator component because that will take into consideration in the other things.
Something as simple as a bolted connection, you might think, oh, it's just like using Content Center. I'll just drop a bolt in. But with the bolted connection, it will place the bolt in, possibly punch holes in two or three components that are sized based on that fastener. And if you just delete the bolt, you leave all that other stuff behind. So follow the recommended process on that.
All right. So first thing we want to take a look at is we'll take a look at the shaft generator. Really, it's called the shaft generator, but anything that you're probably going to turn or spins, hubs, things like that, can all be created with the shaft generator. It will create external profiles and internal profiles. Instead of focusing on drawing, maybe, a half section of something and revolving it, this will use a wizard, which you can see in the upper left of the images, to create a stack of features-- some cylindrical features, you can use conical features, you can use wrench profiles. So for example, at the end of the shaft, you want to put a set of hex faces on there so it could be positioned with a wrench.
All that can be very easily built on, as well as other some specialty features such as what's the best process in Inventor to put a whole axial through a shaft? Oh, I like to use a tangent plane and put a sketch on. I like to use a sketch and then put a perpendicular plane. This had it just built into the wizard, and it works pretty nicely. So a lot of capability.
You also have the option of applying the calculators. And we'll apply the calculators, though the values that I'll put up for you aren't really the ones that would be used in this machine, but just to give you a good idea of how the process works.
So if you will, please just bear with me and I'll just walk through this fairly quickly because, as I said, you'll have the written step by step. You'll also have a video playing. And, of course, we'll have our wonderful lab assistants in the back of the room, who are all phenomenally gifted and, frankly, should probably each be up here instead. So they'll be able to help you out with any questions you have. And I'll, of course, be coming to help as well. So you'll have four lab assistants.
So let me just pop over to Inventor here. One of the things you'll want to do is make sure you activate the project file for the lab. And again, please just watch now. You'll have a chance to go on. And first thing I want to do is get my mouse to show up. All right. Welcome back. It's nice. All right. I'm going to open up the belt-driven gear reducer shaft assembly.
So just taking a look around the design, we already have one shaft component. In fact, if you look at the browser-- I don't think I have any zooming tools installed. Nope. Pardon me a second. Too much time on a Mac. I forget that Control Z is undo.
If I look at the browser, there's even a special shaft icon for this rather than, say, an assembly or part. Many of the design accelerators, while they might appear as a single component on the screen, are structured in Inventor as an assembly. But it's no big deal. So to access the design accelerators, I'm going to click on the Design tab. And again, if you'll just watch, you'll have plenty of time to do this hands on.
The design accelerators have five primary tabs. Fasten, which will have bolted connections and pins, frame for your metal frames, power transmission, which we'll be spending most of our time in. And there's also a spring panel, which we don't have any exercises on, but if you were to-- and I'd be happy to send you the data set if you like-- and you should be able to download it from AU online pretty much as soon as you get home.
The completed version of this assembly has a spring in it that you can right-click and edit with design accelerator and see how the working load was established and the range of spring motion was established. So I'm going to just click on the shaft tool. In your hand on exercises, it recommends that you hold the Control key when you do this. That's really if you want to just start from the template.
If you've been creating shafts, one, you can create a template. And two, if you want to create something similar to the last one you created, you can just shortcut the process by just clicking on it. But just to show you what the walk-through is, I'll hit Control and hit this, and it will bring up the default shaft. Let me just rough this on the screen. I'm just going to click to place it.
There are tools for sizing and locating initially. But for right now, let's just focus on this. In the hands on step-by-step instructions, the step-by-step instructions allow you to take this standard shaft and just edit it into what we need. But just for the sake of time, I'm just going to select the sections and use the small x to simply just delete a few sections and just get it down to one. I'll show you some of the editing capabilities using this one.
So I now have one shaft segment. It's a cylinder that's two inches in diameter by four inches long. It has a chamfer to start it. It's a cylindrical section. And it has a fillet at the end. Now if the next shaft segment is larger, that fillet will be a fillet. If the next segment is smaller, it will be a round, so it will be an external fillet. It automatically changes. You don't need to adjust that. And there are no special segments.
So first thing I want to do is I'm actually just going to get rid of the fillet and the chamfer by saying no feature. And I can edit the size of the shaft in two different ways. I can use grips on the screen to drag the diameter down to 3/4, and I can drag the length by editing the grip. Or I can just simply double-click in the dialogue and update the values from here.
So I'll place that first segment. Next to the sections pull-down, where I can choose if I want to bore in from the left or bore in from the right, that's your internal geometry. Or I'll just leave it sections for external. I have the ability to insert cylinder, split a selected section, add a conical section or a polygon. I'm just going to insert a cylinder quick, and I'll go fairly quickly here.
Like I said, I'm just going to start accelerating through some of this, making a one by 3.41. And again, don't worry about trying to memorize these sizes. They'll be on the documents. I'm going to add another cylindrical section that will be three inches in diameter, not 32. That's going to be tough to turn, at least with my equipment, which is essentially just a drill. Add that segment. Add one more step back down to the original size.
You'll notice that as you add each segment, it wants to add one that's the same size as the last. So again, it's just trying to help you out, remember what sizes you are working with. And then the last segment, I'll add-- again, you'll have all these sizes-- we'll be back down to 3/4 of an inch by 0.55. All right.
So now I have the geometry of my shaft. Now I can add some additional features. The first one-- I'm going to select on this first segment, and on the left side where the chamfer was, I'm going to change that to be a thread, and it automatically picks up the diameter that I'm working with. I can change the thread designation to a fine thread, but I'll just go ahead and leave it 3/4 by 10.
I can change the class, the thread direction. And down here, you'll see a little dialogue showing the z value for the chamfer. So it will put a chamfer back on it for me, but it's part of the thread, so therefore there's no reason to have the chamfer there. You can always set that value to zero if you want a sharp edge. And then set the thread length. I'll set that to one.
All right. Now what I'll do is I'll click OK, and I'll create my shaft. It will offer me the opportunity to change the name of the shaft, change its location, anything like that. Then I'll just use a rough preview, click it in place again, and I have the shaft with the threads.
Now I didn't add everything that I want on the shaft. And in the step-by-step instructions, I think it goes ahead and has you put an axial through hole in the process. But I want to show you that I'm just going to hover over it, right-click, and from the marking menu, I can select Edit Using Design Accelerator. You'll also notice in the Context menu below that is Delete Design Accelerator Component. Those are the proper tools for editing and deleting this component.
So I'll select Edit Using Design accelerator. I'm going to select on this shaft segment either in the dialogue or in the window. It'll highlight it. And I'll come to the end of these pull-downs and say that I want to add a through hole. I'll double-click on it. Sorry let me just change my view properties. Should have done this before. Sorry. Let me turn off ambient occlusion. There we are. Little easier to see?
So you can see the preview of the hole. I'll double-click on it to bring up its details. Take the hole diameter. I'll make it a clearance hole for 1/4 inch, so 0.26. And then we have a choice to measure off the first distance or the second distance. We can also, of course, have our mouse misbehave. I'll fix that in a second. We can change what the distance will be from our point on the x value. And it's 2.15. And that is based on the first edge of this section, which is on the right side.
You can always base it on the second edge as well. So you can choose which datum to refer to, click OK. And like I said, you can modify it from here as well. I'll just leave it. Mine screwed up. You can also rotate it about the shaft by clicking and dragging here. And you could set the diameter there as well instead of using the dialogue. But go ahead and use the dialogue. I'll click OK.
Now I'll just quick pop back to Assemble, use the joint real quick, and just pop that in place on the bearing. Make sure that's good to go. And I'm all set with that particular shaft. I also have another shaft on here. And again, I can hover over it, right-click, and say Edit Using Design Accelerator, and modify it if I want to.
However, for what I want to do, I want to use a different design accelerator. So back on the Design Accelerator tab, in the Power Transmission panel, there is a Parallel Splines. Under Parallel Splines I can select Involute Splines. An Involute Spline requires some input.
So just like much of the rest of Inventor, look for red arrows. When you have a dialogue box and there's a red arrow, what does Inventor want? It wants you to pick something, right? Or dark gray if you're colorblind to red. Sorry. It's amazing how much stuff in these CAD tools are red and green. Like, thanks.
All right. So the first thing it wants is a reference. That means a cylinder, so I'll pick the shaft. Now it's ready for a secondary reference, which is where do you want this spline to start from? I can choose different spline classes, but I do want an ANSI B92.1 37 and 1/2 degree fillet root. I do, however, want 12 splines. So I'll just change the spline designation, and then I can set the length of the spline if my mouse would just behave. All right. I think we're going to make this two and 1/2 inches, something around there.
All right. Now one last thing about many of these design accelerators is you have to be aware-- and it can cause errors. And a lot of times, when you get an error, when you click OK, it's because one of these options down at the bottom isn't needed.
So right now what it's expecting to do is cut geometry into a shaft and cut geometry into a hub. Well, I don't have the hub here, so I need to deselect the one on the right. Otherwise it can be argumentative and demand that I select the geometry for a hub groove. So I'll click OK, again, giving it the naming convention to update things. And now I've got my involute splines. All
Oh, one thing I didn't do-- and let me show you this quick-- I'm going to come back to my shaft, my first one. This is what I get for getting in a hurry. And one thing I didn't refer to, to a couple of things I didn't refer to, are first, the calculation tab. So it will show me where right now it's putting in a radial force, I can change that using the pull-down to a torque, and 100 pound feet. We'll just leave it whatever it is.
Now if I try to run this calculation, it will fail because there's no counter to that torque. So I need to add another torque. And roughly, where I put that hole through is where there's going to be a pin that's going to be driven by a clutch. So that's what I want to put my counter torque. So I'll slide one or the other to roughly where that pin will be.
And then there's going to be a bearing on either side of this larger profile. So I'll take my bearings and move their support location to between the torque loads and on the smaller shaft section. I'll click Calculate. It'll give me my results in the panel on the right.
And if I select Graphs, I can look at the shear force, bending moment, deflection angle, deflection, all that. I can even look at the ideal diameter. So with these loads, I probably need a slightly larger shaft than what I have. So handy? Seem cool? Do this every day, right? No?
All right, your turn. So let's have you go ahead and bring up your handout, bring up Fusion, make sure you activate that project file. And we'll be around to help, and then have at it. And Brian, Caleb, and Kevin will be as well.
All right. Let's get ready to take a look at the next section. One of the things that isn't necessarily recognized a lot of the times, as someone who does a lot of training, is the hardest thing to teach someone in Inventor, or Fusion-- for that matter, probably just about everything else-- is sketching because there's so many ways to do it. You need to know, all right, that's easy. Well, do you start with a line and then start doing offsetting and trimming? Or do you just draw the perimeter, or you create two rectangles? Which one's the smaller one?
And they're all right. It's just totally up to you. When it comes to things like design accelerators and the very, very industry specific tools, they're usually really quick because you can only do so many things. You're not really allowed to do that so we won't give you that option. So these things should go fairly quickly.
All right. So let's take a look at Gear Generator. So there's three different gear generators. There's spur gear, worm gear, and bevel gear. All will work on standard tooth profiles. All of them will have different ways of calculating how you set the gears up. You can calculate a center distance between shaft based on the module and the number and the ratio. Or you can calculate the ratio knowing the center distance but wanting a certain module. It's crazy. It's just super powerful.
It will guide you through that process. So as you pick the different design guides, you'll see certain areas. See how some are grayed out and some are left white for entry? That's how you'll start working. You can also create the gears in different ways. You can create components, so it will generate a gear with the teeth. You can create features.
So for example, the large diameter you put on that shaft will cut teeth into that so you can add the gear teeth as a feature to that shaft. And you can also do virtual. So let's say you're going to do a planetary setup, or you've already got a gear that's modeled with the teeth, and what you need is something to mate to it. Well, you can put in the information for that virtual gear, and it will guide the design of the second one.
So let me just jump into that real quick. Pop back over to Inventor and there we are. Oh, my mouse disappeared again. There we are. Hi. Let me go back to Open this time. I'll grab the belt-driven reducer gears file. Pardon me a moment while I remember what I'm supposed to be doing.
All right. I'm going to just start the gear generator on the Design tab again. This time I'll select a spur gear generator. And what I want to do is use a design guide of total unit correction. I know the distance between the gears. I have a diametric pitch in mind that I want to set, which I'll set to nine.
Then what I want to do is start specifying what the gears are going to be. The first gear is going to be the one that I want to cut into this shaft. So I'm going to change it from component to feature. I'm going to say I want 24 teeth, and I want the face width, knowing what I made that shaft segment to be of 0.8. So I'll set that to 0.8. You can also use a measure tool, which is just attached to the little arrow on the end, as it often is in Inventor.
The second component, I'll leave a component. I want the number of teeth to be 48, and I'll set the face width to 0.8. So now I've kind of prepared what I want. Now I need to tell it where I want it. So the cylindrical reference for the first gear, the feature, I'll select the outer cylinder of my smaller gear.
The second reference will be the start plane. I'll make sure that's selected in the dialogue, and I can pick the face. And I get a preview of what that gear will look like. For the second gear, the component, I'll choose the cylindrical face of the shaft that it will be mounted to. And for start plane, I'll just reference that same front face on the shaft.
However, if I look, it's putting the gear in the opposite direction. So I'll just simply flip the start plane and put it back in line. Again, you have a calculation tab where you could go in and put your load, you could put it in your life expectancy. You can put in all sorts of information and validate whether or not these gears would do the job. For today, though, we're just going to just say OK, give the naming information, and it drops my gears in.
I do want to do one other thing while we're here. I want to go ahead and put a bearing in as well. So I'll come up to the bearing generator, also in Power Transmission, select it. And I'll tell it what sort of bearing I want. So I'll open the overall menu. And in here, I can choose just from a small set of options on what type of bearing I'd like.
So I'd like tapered roller bearings. Now it will give me the options that I have. One thing you can do with bearings is you can pre-select geometry for the interior and exterior, and it will filter out what bearing options are available to you. So if I were to come back and select a cylindrical face and pick this shaft, switch the start plane over, or set the start plane at the end of the shaft. If I come back in and ask for tapered roller bearings now, in this case, I get pretty much the same number of options. Had I picked a different shaft size, I might not. I might not get any options. So I might not be able to buy one of those.
And that's the key because it's not just whether or not it's strong enough, as can you get it. This is where we're getting into the standards. So I'm just going to grab the ANSI 19.2 TS tapered. And it will give me my various sizes based on the width and the outside diameter. Just for expedience, rather than getting into all the detail, We'll? Just select the one that starts out 05075. Actually, I'll click OK.
Now when it comes in, I think it comes in backward, but if I want to change that, I can just say Edit. It brings me back to the exact same dialog box, which is another great consistency, and I can say flip it. Actually, it was right the first time. But you get it, right? That's why my most commonly used tool is Undo.
All right. Just that quick exercise. Let's have you go ahead and do the same thing. And again, bit.ly/AUDA2019 if you want to hand out if you don't have it already.
So you might have noticed in the instructions, it says if you want to reset the gears, again, on these machines, you don't really need to use these because no one's created these shafts. But at work, if you don't want the last thing you made, in this case you hold Alt. Some of the tools that are on a pulldown, Control doesn't reset the dialogue.
Now there's another one-- I can't remember which one it is-- that Control does work on a pulldown to reset the dialogue. So just experiment. It's either Alt or Control. Or you can just rebuild it.
All right. Let's go ahead and move on to the next one. I'd really like to try and get at least you some exposure to each of these. Of course, there are going to be others that we just won't even go near, including most of the calculators. But the belt and chain generator's a fun one.
As you probably know from your real world experience, there are a couple different types of belts and a few different types of chains. So with each one of these, you start to get more and more options and more variables. There's V belts, synchronous belts, and roller chains. And what's special about these, of course, is you can't buy chain in any length that you want, at least not for the engineering purposes. The same goes with belts. I'm sure Gates would make you a belt to whatever specific length you want, but that's a great career-limiting error if you just get a $50 belt instead of a $2.00 belt. So just remember that. Not saying I'm speaking from experience.
So these use standardized belts and standardized chain lengths to set up sprockets and pulleys and help position them based on the ratios you need. The loading calculations are there as well, so you can go validate whether or not the belt or the chain will work. And you can also start using that as a tool to maybe optimize some things. Perhaps you really don't need that big, heavy chain that you've been using all these years. Maybe you can go with something less expensive and lighter. It's just that no one really messed around with it or tried it.
So let me just hop through this real quick, and then we'll have you do it. I'm going to open up the gear reducer belt drive assembly. Now this one is going to be the most kind of pick-intensive as far as getting things roughed in. Another thing that you do need to be aware of, much of Inventor is noun verb. So if you pick a piece of geometry and then start a command, it doesn't care. Or if you start the command, then pick the piece of geometry, it's fine, too.
With design accelerators, it's good to set up some of those properties. Like on the shaft generator, make sure you don't have a face selected before you start it because then you're kind of committing to a first reference, things like that. Or if you select all your references, then start putting in the information, you might have to fight through some errors before you can get it straightened out.
It won't fail or anything. But you're going to have to put up with dialogues. Oh, I can't make that. Well, I haven't finished telling you what I want to make yet. But it's trying to generate those previews . And just like anything else in Inventor, if it can generate a preview, it's pretty much done the work. It's just a matter of whether or not you want to keep it.
But with the belt drive, when I go to design accelerators, as I said, V belts, synchronous belts, and roller chains will be using a synchronous belt. And as we're going through this, you'll see that we not only need to select geometry to position, but sometimes, as we will hear, even though there's a model of an idler, we really won't be able to use the physical model to do what we need initially.
There are times where you just kind of need to use things like virtual components help you sort out what you need from your physical components, and then use that standard purchased part to guide the rest of the design, even when it comes to sizing an idler or positioning it, as in this case.
So the first thing I'm going to do is make sure I'm using a Type H synchronous belt. I'm going to set up my midplane offset. So it's the midplane of the belt. And I'm going to select that front face. I'm sorry. Let me turn off this goofy ambient inclusion.
And so you can see right now there is a green belt, there's a green preview showing. That means that I can buy a belt of that length. If I click and drag on the diameter of a pulley, you'll notice that it repositions the other pulley. Why? Because a larger or smaller diameter affects the position of the other pulley. Belts are only so long. If I click and drag a pulley itself, you'll see it snaps, and it's snapping between the size of belt available. It would do the same thing four chains, but it would be a finer snap.
So I want to offset this so that the midplane of the belt is lined up with the existing pulley in the assembly. So I'll say I want that minus 0.49 back. Then I need to start positioning things. So the first pulley, setup is a synchronous pulley. For the position, right now it's just based on a set of coordinates. But I'm going to change the position to a fixed position by selected geometry because I want to choose the shaft of the motor as the center of that pulley.
The second pulley I really don't need, at least as far as physical pulleys go. So I'll select this in the dialogue and say I have an existing pulley. And then I'll come over to the geometry. There we go. Come on. It'll be picky on me now. I like to select the whole thing. There we go. Pick the root of the spline or the tooth. And you'll see now that preview is red, so I don't have a belt length that will go directly through here. So I'll need to use an idler. So I'm going to say add a pulley, and I'll just pick whatever because we're going to actually replace that with a virtual pulley.
And you'll see it's roughly placed this in. I'm going to drag this out a little bit. You'll see it puts it way out to the next size. I'm going to flip it around using the arrow and drag it over to this side and flip it again, try to get it to behave itself. But it's not going to. Oh, sorry. You have to be smarter than the dialogue.
So what it's doing is it's demanding that that is the last pulley. I actually want to click and drag this pulley up to be the second pulley. Now I have more control. Now I can snap positions more easily. I want to make the diameter of this second pulley two inches. I'll drag this in, and I'll flip it to be outside of the belt and drag it in again. It's snapping in a way I wasn't expecting because there's people here.
Oh, I haven't corrected this one yet. Let me drag the number of teeth down on this, either using the guide here, to 24, and pull this back out. And now I'm getting roughly what I was expecting. So by flipping the direction of the belt across that idler, you'll flip which side it's on. By making sure you have the sizes roughed in, you'll get a better prediction. This is, again, one of those instances where you might fight through it till you give it the proper information. So it's not the computer's fault. It was my fault.
One last thing I want to do is, for the position, I want to set it to be rotation-driven sliding position. So what I'm going to be saying here is that based on the center of where this idler is using an arm that I'll double-click on here and make that arm two inches, I want to know where that idler would be.
All right. Now if I go over to Calculate, this is kind of an interesting thing. If I calculate now, I'll get an error. And if I expand the dialogue, it's about the diameter of the pulley. So this pulley, even though this is what I asked you to use in the step-by-step, is too small. It creates too sharp of a transition.
So if I modify that pulley to be two and 1/2 inches and calculate, it's fine with that. It can deal with that radius. That's pretty slick, huh? I think that's pretty amazing that it understands what needs to be done.
One last thing, though. Down at the bottom, you might have to expand your dialogue using the double arrows. I want you to tell it to create the build as a detailed belt. When you've made all those changes, click OK, accept the files. You'll notice that the virtual pulley goes away. I need to update the design of my idler, but until then, I can just sneak that over or create a tangent constraint once I have it to be two and 1/2 inches, and I have a nice accurate model of the belt drive.
All right. Want to give it a shot? All right.
15? Oh, boy. I think I'll just demonstrate bolted connection and let you guys try frame generator. So like a lot of things when you're learning these tools, especially when it comes to this stuff, it's easier when you're making your own stuff because you already have an idea of what it is you normally do, and you can just go right to it, where here it's like, well, I don't really use those belts, so I don't recognize if I do have any sort of problem, how am I supposed to work through it?
All right. Bolted connection generator, I'm just going to show it to you because it's pretty simple. It's also one of the most common things you'll use. Did anyone get through, or was the key way included in the handout? Yeah? Anybody get through to that? So you calculated the hub and the shaft groove. Pretty cool? OK, good.
So for those of you didn't get that far, if you put a keyway in, selecting the shaft, if you use all three options, it will cut a groove in the shaft, cut a hole through the gear, cut a groove in the gear, and place the key in the keyway, in which is pretty nice.
All right. Bolted Connection, really powerful tool, right down to the fact it can tell you what diameter bolt you need based on the number of bolts you have and the loads you have. You can also reverse that and ask it, well, we got a whole bin full of 1/4-20s. How many of those would I need to hold this together under these loads? So you can be a hero of purchasing and get rid of a lot of 1/4-20 bolts. Manufacturing might not like you because you just asked them to put 400 1/2-20 bolts in. But that's OK.
So a lot of different options. A lot of the placement options are very similar to just using a whole feature. What's great about bolted connection generator-- although I think I remember now there's still an error in this data set-- is you can go through multiple parts, placing clearance holes in parts right up to the one you want threaded. Or, if you plan to put a washer and a nut on the other side, put a clearance hole through any number of parts all at once.
So none of the old how much time have you spent in Inventor making sure that all the holes and all the parts line up before you even put them in the assembly? And then you drag a bolt into them, and whoa, magic. Here, just think about parts fitting together and fasteners keep them that way. That's really the approach that design accelerators take.
So I want to just pop over to Inventor quick. And again, I'm just going to run through this quick, and then I want to show you-- we'll use the last few minutes here to take a look at frame generator.
One quick piece of housekeeping, though. I want to try and go in here. Let me see. Sure enough, there they are in this plate. There we are. I want to get rid of these holes. Let me come back up to the top level. No, I really do. All right.
So I'm going to go to the Design tab, as always. The very first one is the bolted connection. You can choose if you want through holes or a blind hole. The primary difference is if you say through, you'll pick the starting plane or starting face of the bolted connection and the ending face of the bolted connection. And any number of components that are between start and finish get punched.
With a blind, which is what I'll use, I pick where the last hole will start. Does that make sense? So for example, I want to start on the face of this flange. And I'm going to change this to on point. And then I'll pick my point. Then I'll start where the blind start plane will be. Now there's a gasket between that housing and this plate, but I want to start the blind hole on the face of the plate.
Shows me a little preview, all nine locations. Or eight locations, excuse me. I can set a diameter or I can go into Calculation, say I want a bolt diameter design, tell it that I want 200 pounds of axial force, and I'm afraid of someone dropping this thing on its side, so I want to calculate for 400 pounds of tangent force.
And watch the preview of the holes. I'll calculate. No, that should be good. Oh, I forgot to specify the number of balls. I'm sorry. Eight. So one bolt of that diameter could hold it, and it's not behaving itself. Let me make sure if I have my calculator on. No, that's just fatigue. Calculator should be on. Come on. I don't want that. So it should calculate. Yours will because, you know, why not? I probably should have reset the dialogue. But it's basically going to end up at a number 12 on yours if you do this at home.
Then what you can do then is say that you want a fastener. And like it would for all the other ones, it won't give you fasteners that won't fit. So if you can't get a bolt of a certain diameter short enough, it won't offer you that type of bolt. So it starts making life easier. You can also filter, saying you want, maybe, not round head bolts, but socket heads, hex bolts. Grab the one you want.
You'll notice Click to Add Fastener reappears underneath that. You can click again, and it will offer you washers. So you can grab a helical spring washer, drop it in. If you come up to this top one, you'll see it click and drag for the length of the fastener. Notice that it is not infinite. It only goes in standard lengths. So again, helping to eliminate career-limiting errors. And I can pull back that hole as well. When you're done, click OK. You see already it has the holes in place. If you edit apart, you'll see there's a clearance hole in this part, and there's a clearance hole in the gasket and a threaded hole in the plate.
So that's just kind of how that works. Try it out another time.
I do want to talk a little bit about Frame Generator. Yeah, we really don't probably have time for that either. Frame generator. Any of you do metal frames? OK, a couple. All right. Any of you using Frame Generator? You are? OK. There have been some enhancements in the last year or so for reuse. So this example, I think it reuses one component. But if you know that a piece of geometry is going to be the same, two members are going to be the same, you can just reuse them rather than recreating them, rotating them.
But the concept of Frame Generator, for those who don't typically work with it-- I'll just show it to you quick-- is that you start out with a skeleton. It can be sketches, surfaces, as it is in this case, or even solid models. You can pick where you want a frame to start, where you want it to end, or pick an edge to drop a frame on it. It's all based on standards, as you would expect.
So you select a family standard, then the family. And then you're able to place the components on that skeleton. Another thing that you can get into is frame analysis. So this is beam element analysis versus finite element analysis. So based on the section that you place on your model, it will know what that should be able to support. So I'll just choose an ANSI. Remind myself. I think I just grabbed a-- where's a square?
Oh, sorry. Where on earth did that go? Grabbed the wrong one. Let's just grab a square tube. And you can see it comes in one or two size options. I wouldn't want to haul around 16 by 16. You have your selection options here, and you have orientation. So you can select how you want to orient the frame members.
So I'll pick the edges of the base of the frame. Now I want these to be above that and within the footprint. So I can pick the orientation in the dialogue, or I can use the quick icons on the screen. And of course, I've got one because there's people standing here, that goes the wrong way. Let me try that again. There, it wants to behave now. So there is some pick sensitivity there.
You can also rotate the members out of just a normal plane. And when you apply them, you'll set up the name for your skeleton, the location for it, and set up where your files are. Then it will drop in those frame members. Let me just drop in a few more, relocate those. And let's drop these in as well.
That one just doesn't want to cooperate. So I'll leave that one. Apply. Put that to the outside. And let's grab these angled ones. So essentially all you're doing is roughing in where these will go.
Then the fun begins. Once you have these in place, you're able to turn off your skeleton and go in and do some cleanup. And I won't trim all these up, but just to show you each one of the tools, I'll say Trim to Frame. And I'll grab these two members, but not trim the frame. Good grief. Trim and extend. Grab these two members, and then say trim them or extend them till they meet that face. Apply that. Let me grab the angled ones here. I can right-click and use Continue to select the angle face, and you'll see it cuts the angle.
I'm not going to do all of these. There's some other tools as well. So I can, for example, grab and lengthen or shorten based on a distance and based on a direction. I'll say midpoint. I want to lengthen this or shorten it. Or I'll lengthen it four inches, grab that front section, and just extend it. I can do the same thing to the back.
Up top here, I can say trim to frame, saying I want to take this as the blue frame and but the yellow frame up to it. With each of these, you can set in offsets. So you can create weld gaps, everything else, while you're on the fly. If I get done with that and I decide I really don't want that, we even have tools, if you expand the frame to say Remove End Treatments, select that frame section, and clear out that member.
Then I can always come back and say I want to miter not just the two, but all three up top. Any of those, you can reuse if they're the same geometry so you don't duplicate effort on the parts list. You can also modify the frame members after the fact, changing out the standard or the size, and keep everything up to date. You might have to reset some trimming options. But by and large, compared to trying to use content center components, things like that, it's really powerful.
Over the years, there have been some implications around parts lists and that. But with Reuse and other enhancements over the last few years, it's getting much easier to work with in a team environment and group environment.
All right. We're pretty much out of time. But just wanted to show you real quick-- by the way, all the videos and the content and everything else are going to be made available from the Autodesk marketing team, actually, extended versions of these. So if you have people at work who might want to see this sort of thing, of course, they'll be able to get on AU online. But there's also another version of these with extended handouts that they'll be able to go through as well.
But these are all of the tools, some of just a handful of which we went through today. So there's a lot to explore. If you work with pins, if you work with cams, if you work with springs, applying O rings, any of that stuff, design accelerators, anything around machine design, you can just do tremendous work with them.
I'll stick around for a few minutes unless they run us out. Then I'll stand in the hallway if you have questions. But thank you so much for your time. Have a great AU and a safe trip home. And thanks a lot.
Oh, by the way, I don't have enough for everybody. But if someone wants some Inventor hats, I do have some Inventor hats up here, too. If you'd like one, just come on up.