Inventor 2018 Model-Based Definition: Why and How to Apply

PETER DE STRIJKER: Everyone, welcome in this [? trek. ?] And I'm glad to see that many people are interested in model-based definition, the new feature in Inventor 2018. The purpose of this presentation is to show and learn how to use model-based definition and how not to use model-based definition.

My name is Peter De Strijker. I'm working for the EMEA team for Autodesk. I live in Belgium and I've worked now for 8 and 1/2 years as technical specialist for manufacturing products. I have a co-presenter with me, who is going to present a part of the presentation. And Stephen, please help yourself.

STEPHEN WERST: Hello everyone. My name's Stephen Werst. I'm a senior product strategist with a company called Sigmetrix. We've actually had a relationship that started with Autodesk about three years ago, where they actually leveraged some of the technology that we have in our GD and T authoring space, utilizing what Peter's going to show this morning.

More recently, though, our company is founded on tolerance analysis software. And as of last month, we introduced a new 1D tolerance analysis solution called EZtol. That leverages much of this information to make that process as easy as possible, and that'll be what I'll be showing during this morning's or this afternoon's class.

PETER DE STRIJKER: OK. So the reason why we introduced this model-based definition functionality inside the Inventor is because there is a new era and a new industrial revolution coming to us, if you have a bit more broader picture of the positioning area.

I think, in this room, everyone has heard about Industry 4.0 or something like that? Like Smart Factory or Factory of the Future. It's a buzzword that's going around. But that's in effect the basis of how you can apply this functionality inside Inventor. This is one of the main pillars to make this transition from a conventional way of working to Smart Factory. This is the main reason. OK? This is the big picture now.

Who in this class has used model-based definition BMI or GD and T 2D annotations for production? In the past or recently or now? OK. So you control the process retrieving this information and use it for production? OK.

So then, I see two or three hands. That's good, because that's the purpose of the class, is just to give you a good idea introduction for people who are not used to use this technology today. So again, these buzzwords that say Industry 4.0, there is no real standard or definition that defines this Industry 4.0.

So the Germans did a good attempt to describe it. And this is a kind of, let's say, chart what's summarized the Industry 4.0, and the main topics which support this evolution. And very interesting to see is the yellow part, the four main pillars. Sorry.

It says, in general, that Industry 4.0 is a current trend to automate and exchange data for manufacturing technologies. So you have to make products smarter to make the automated manufacturing possible. It won't work without it. Another one, very important thing, is you have to have a smart factory to monitor, to supervise the production, the ongoing production, which is also based on the smart intelligence.

And what the point we'll be coming on today in this session is, we're going to focus on smart production. Intelligent production, smart manufacturing. This is where model-based definition comes in place. Because in an ideal world, in a digital enterprise, there's the information and how and where to produce it, it's going to be taken out of the model.

The complexity, the accuracy of the model, will define on which machine this model will be machined, for example, or produced. And on top of that, the system will automatically rebatch and reshuttle the products. When the machine is down, for example, or an urgent order comes in, you have to reshuttle all these things.

Now today it's done by humans, people. So the system, if the models are intelligent enough and they contain all information to make that automated shift, the system will take over. That's called a manufacturing execution system.

So to make this work, we need four technologies built in the model or, let's say, have in place. The first one is, you need to have the capability to build your model and to add enough information to the system that the downstream consumption of the information works. OK?

So today you have a drawing and a model. It's not connected. You do have a geometry, but let's say that the accuracy of the model and the surface finishing is in the drawing. It was. Let's say before 2018 version. 2017, you have two documents. Today, we can add this information straight in to the model.

The second step is engineering based on GD and T. For that, we have our partner Sigmetrix with EZtol, that helps you to make a study how the worst case, median case scenario is if you accumulate all tolerances in the model. The tolerance on dimensions can be surface or geometric tolerances in general.

So this is a pre-study to make this work. And if all the information is in place in the model, then you can use the information in a CAM system, for example. Or CMM control, quality control system. And this is where a digital factory is built on. This workflow has to be automated with less and less human interaction in there.

So what is model-based definition? Well, it's a big buzzword for a lot of things. It effects the way how to enrich your model with production information or information that can be used downstream the design process. That is model-based definition. It can serve to document, to collaborate, or to program, let's say, the production cycle.

Without knowing it, we are using a part of model-based definition for a long time. All the Inventor iProperties is a kind of model-based definition. Volume, the weight, all these kind of things, material that you assign to a model. This is a kind of intelligent piece in the model which you need to have for production. You know, stainless steel has other production methods than cast iron, for example.

So based on that material, we can define production cycles or [? such ?] [? as ?] [? these ?] that are different. Bill of material, tolerance dimensions, surface finish, geometry tolerances, GD and T, holes and threads, and general notes, production notes, [? that's ?] [? my ?] [? drawing, ?] is model-based information.

So what introducing the model-based definition standards? Let's say about 10 years ago or a little bit longer. All the regulations, standard regulations, introduced a new standard like ISO and ASME. They had to set in place a regulation that controls how GD and T or BMI or general model-based definition has to be treated.

And there's different than-- today we are doing on three drawings. It looks like the same, but you have some new rules and some new techniques to learn to make 3D model definition or 3D GD and T to work.

For example, it's allowed to have a combination of drawing, model, or both as a deliverable. So the drawing is not the only piece anymore that has value. You have to define it in the model. That's it. But there is a regulation that says, you can deliver both products or both deliverables same time. Just refer to each other. Make that end user see there is some documents. [INAUDIBLE], for example.

And there are standards called Dataset Classification Codes, which gives the level of, let's say, information level of the model and the drawing. So each of these steps is officially standardized, is allowed to use, as they said. And it's nothing wrong with having a level three or four. Because in some cases you need it.

If you're automated-- if your production system is automated until the machining part, but inspection is still minimally, we need to have a full model level four, where we have a complete model documented but also drawing. Because the guy needs a drawing to have to reference the dimensions to measure and to control the parts.

So none of them is wrong. It depends on what you want to do with this information. OK? An example of a Class Three. This is a 3D model which has 3D model annotations on it. It's not a drawing view, it's a model. There you have a drawing. But? You have to add a note on the drawing that's, for the complete set of information, you need to model as well.

And in your model you can note, you have a note space to put notes, you have to refer to the drawing. That the drawing goes with a model to have the complete information. So Inventor supports all these steps. Another way to annotate fillets. In a 2D drawing, normally fillets and chamfers are never annotated or mostly not [INAUDIBLE] is dimension, with four multiplied by 45 degrees.

In this case, you can use a note. Again, Inventor supports this way of annotating because you can add a parametric texturing in your notes that has the dimension inside. So there's no problem. Another example is, if you put some GD and T information on a model.

In a 2D drawing, you say the flatness of this surface is [? 0 to 2 ?] millimeters. In 3D model, the direction is important because you can have a straightness in the direction of x and the other way can be y. So these are a few examples that in most cases we don't use in 2D this way. So some little things, little behaviors that are a little bit different to you. So be aware that that is there, and Inventor supports these capabilities.

Best practice. Don't try to emulate 2D drawing views in the model, or you get this. It's useless. It doesn't make any sense. Because why should you-- why should you put a dimension of 50 nominal on a model if you want a millet? The CAM software can't read it. Check geometry. It's 50, he said.

So if a model of the tolerance of a dimension is not falling in the normal tolerances, that makes sense. So this is a model or a tolerance scheme that's useful. Because the diameter of, I don't know how much it is, circle, the software sees it so you can read it.

So just put the information that's needed for the purpose you want to use it for. Machining, controlling, inspection, you name it. But this is the way how you should do it. And I can make a different model for the foundry to make this part, as a rough model. It's a different sort of drawing. This is a production drawing. This is a finishing drawing or manufacturing drawing.

These are little different tricks just to be aware that applying 3D tolerances is a little bit different than the 2D world. OK? So, diving deeper in this Inventor technology or the effective functionality.

Model-based definition is supported in, as well, parts, sheet metal, and assembly environments. OK? And it supports standards like ASME, DIN, and ISO. That's a dick. It's about 200 pages, so don't try to go through it. Just-- it's supported.

The class for today is not to learn which every symbol means. That's not the purpose. It's how to apply it. That's just in case. So the first time you run-- if you open a model in an older version of Inventor, the software will pop up this dialogue box, asking you which standard do you want to use for the model-based definition.

The moment you take the annotated environment, this will pop up. Because in the old templates, there was no such thing available. So you need to know what to apply. Automatically. Done. You don't do anything for it. It just pops up.

For your new templates, if you start 2018 and you use the templates, you can define a standard in the drawings in the document template, which you can then save as your standard templates. OK? That's good to know. Because the standard defines how GD and T information will be displayed and appear in the model.

Second thing, a little bit strange at first sight but it makes sense if you think a little bit deeper. To change the standards styles, you need to go in to drawing styles. Nevertheless, it's a 3D model. And the annotations are visible in 3D. Every setting has to be done in 2D stats. OK?

You recognize them with an extension 3DA at the end. That's standard. That's from 2018 version. You will see the 3DA extension as an extra style. You can edit them or you can make your own copy from normal standards. Do what you want, but these are the predefined standard definitions in there.

If you watch the ribbon, or the UI in the software, this is what it looks like. So you have annotate tab in your menus. And there are three big, let's say, chapters in there. The first one is the geometric annotations app, which allows you to add geometric tolerances and do some diagnostics, which is powered by Sigmetrix technology.

So it's not just like this. The title says, annotate is not just an annotation you put on your model. It's a kind of database driven system that keeps track on what's possible, what's not possible, what's consumed, what's not consumed. So it's not just putting a text label on your model.

Be aware of that. So if sometime you try it out and things don't work, there is a reason for that. The software will prevent you to do stupid things. That's a good thing, isn't it?

The next thing is, to apply general annotations like text notes dimensions to a model. And then the last chapter is collaboration. How to communicate information externally. So for Inventor use case. These are the three main blocks in this menu.

In the middle, it's just to manage your, how you say it, visibility of your annotations. Scale, for example. If you have a small mobile, the annotations are automatically scaled or you can have a fixed scale in there. That's what it says. No, back, yes.

In the feature tree, they also added two chapters. Two new tabs in there. The annotation tab and the tolerant feature tab. So you can use them both for editing. And this stuff, you can click on the annotation itself or you can go in there and annotate in this area, as well.

So it's to say, it's not just information. It's a working area where you can not add, but edit and sometimes delete annotations if you want. Hide, show, you can do it here. If you have a set of notations to hide in one block, it's easier there than going in the model. Say, one by one, [? high, ?] [? high, ?] height. So that's the interface, the UI.

And then some shortcuts. You know, I told you that the direction of the annotation can be important to know. So you can toggle between candidate planes by tapping the spacebar. So if you, before placing the annotation, it's [INAUDIBLE] the display.

If you tap spacebar, it will turn like this, like this, in the same face. And then the tab key will tilt, let's say, the annotation, like this or this depending on what you want, if it's vertical, [? horizontal. ?] So you need to play with these things to get it right.

And you can also define an annotation plane as a reference for direction of your annotation. That means, if you want to have it for 45 degrees for a certain reason, with the shift key you can set the 45 degrees plane. And then the annotation will change direction as well.

I told you not to do this. In most cases, no. If you really want to do it, you can use design views to make this work. Design view is a very powerful method to manage, let's say, the bunch of information in this model. Because for each design view, you can help show and hide some stuff that you don't want to see in there.

We have a company using this technology, design views, to show and hide information for the CAM programmer or for the quality control guy. Different views, same views, front view for the CAM programmer, front view for the inspection guy, different information. So you can build as much as you want off that information.

The good news is that all design views you make here are exported to 3D PDF and DWF as well. OK? So if you manage this well, that can work. So there's only way [INAUDIBLE] would say, OK, put the benches on there. But it's not replacing the 2D drawing. Not at all.

Some best practices. Lucky of you. If you make a view, lucky of you. That means the new annotations you add will not show up in that view. Otherwise, if you add one annotation, you have to go through all the dead [? hand ?] views to hide it, which I don't like. OK?

And the camera view. Say the current camera, because that's the position you want to have to have to view. That's one important thing. There is a publish option there, which means this option publisher views also to the PDF, 3D PDFs and the DWF files. If that is not selected, it won't go through. Be aware of that.

And the annotation scale. My best experience, automatic. That's worked for most of the cases very well. Again, if you're using old drawings, which don't have these right top front isometric views built, in because in 2018 templates you get it automatically, because of the model-based definition functionality every template has this now.

For older ones, I made a script and I posted it on the class links. You can download this. The scripts-- you can run a bunch of scripts. You just click it on, if you can use it as an external script, and this view will be created automatically.

Just easy to use. You can do it manually, if you want, if it's not too much work. But if you have more than a hundred parts to do, it's better to do it automatically or even in batch, something. That works. OK? So I published it on the class page. You can download it for free.

Another one. In the object visibility, there is a new option that says you can hide/show 3D annotation in one go. You don't have to go through all the [? dimensions ?] to hide them or show them at once. You can just do it quickly. That's about the interface. Any surprises, questions here? No? OK.

So then we go to the workflow. And the workflow, you can take three main blocks in there. You apply the annotations. You retrieve some information. For example, promote dimension, the model dimensions. You can promote these dimensions as a 3D annotation, as well, which gives you some more benefits. I will talk to you later about this.

And then organize the views and export them all. These are the three steps, normally, companies take to make use of this information for production. First of all, apply geometric annotations.

This can be a geometric annotation on a plane, on an-- how do I say it? An etch, what I'm looking for. Circular, flat, and etched is possible. And also on dimensions. So if you have, for example, two faces, you can select slap. You can put a dimension on these two faces, and automatically a tolerance on this dimension. OK?

The datum reference plane is automatically created by the Sigmetrix engine behind it, OK? So don't go looking for a datum plane icon somewhere in the ribbon, or in the menus. Again, it is not adding an annotation to something. It's the system that works for you.

So if you click the first time a face, that's for the first-- reference eight, for example. You start from there. If you take the next one, you can refer to that A, to consume as A as a reference second time. Again, per face you only have one annotation possibility.

No reference mode-- no annotation possibility, sorry. If you want to have more, you can add more stacks to this annotation. So the [? better ?] will be grayed out for that face, that time. So if I see that button don't work, it means there is annotation. You can edit annotation and add more information about it. Again, the Sigmetrix engine behind it prevent [INAUDIBLE]. Right?

Now, our experience. Not everywhere in the world, we are using a tolerance in combination with datum reference in the same symbol. Where I come from, in Europe, in the DIN or ISO, we can say a face has a reference A without saying anything about the conditions with this.

There is a workflow to get it done in Inventor, but it's not so obvious. I'm going to show you how to do it. I show it immediately. [INAUDIBLE] [? reference? ?] There we are. So for example, if we have the assembly here and we take this model. Open, yes.

If you go to the [? Annotates ?] app and we put in tolerance, let's say. You see, the question pops up? What you want? It's not saved here. That's OK. That's a good one. I take this face as a reference.

I can confirm, position it, and then I can go here in this symbol and say, remove tolerance frame. And then he will put this A on this face. That's the only way to get it done, OK?

Our people use this way of annotation, like this, without any conditions on it. Yeah. So that's the way to get there. If you're looking for just a symbol, it's not in there. You need to delete the condition first time, OK?

The datum reference frame allows you to create combinations that are not exposed immediately. So if you have reference A and reference B somewhere, and you consume A or B in other tolerances, you might be-- it can be useful to have a combination AB reference. Or BA, depending on if you have a condition that has to work for both.

So you can put together your own targets here for reference planes that are not consumed yet, or the combinations not consumed just. So I can make here an AB, for example, with minimum material conditions. Or maximum material conditions on there. So I can use this as a reference to build a new tolerance scheme in there.

And then the big one. Tolerance Advisor. In the interface you will see a tab. It's called Tolerance Advisor, also powered by Sigmetrix, which will give you some indications of what is missing to have a fully defined model. So one golden rule. Don't try to solve everything in there.

Because you always-- it takes the optimal situation to make things fully defined. Sometimes we don't want to have it fully defined. It's on purpose. So go to these options. Sometimes I say, it is important or not?

Do I need to solve this or not? It's just an advisor. It's not a mandatory list to solve. It's advice. That's why the name says advisor. OK? But it keeps track on things that can be improved or information that can be added.

For the assembly, it's a smaller ribbon because it doesn't make any sense to put GD and T information on an assembly. You can add overall dimensions for inspection, that's OK. Annotations. But you never machine, let's say, the entire assembly in a certain tolerance for flatness or [INAUDIBLE].

It's on part level we do this. So there is no such thing like tolerances in assembly.

AUDIENCE: [INAUDIBLE] tolerance [INAUDIBLE]?

PETER DE STRIJKER: Pardon me?

AUDIENCE: [INAUDIBLE]

PETER DE STRIJKER: Yeah, it's not. It's treated as assembly. [INAUDIBLE] assembly says it's not in there.

AUDIENCE: [INAUDIBLE]. But I mean--

PETER DE STRIJKER: Yeah, you're right.

AUDIENCE: Do you notice that something is there maybe [INAUDIBLE] on?

PETER DE STRIJKER: I'm not sure about that, no. Not sure about it. But it makes sense, you're right. If you have an [INAUDIBLE] assembly, you can machine it. You [? half ?] machine it. Reference rates after assembly [? for ?] [? welding. ?]

AUDIENCE: [INAUDIBLE] But that's-- I'm trying to get away from deriving--

PETER DE STRIJKER: That's a good one, yeah. Yeah, you can derive it. You can have a [? welding ?] drawing model but then a derive drawing. OK, I understand your question. It's a good point.

AUDIENCE: [INAUDIBLE] instance where you can do assembly [INAUDIBLE].

PETER DE STRIJKER: Yeah. Can be posted on ID station as an extra addition. Because it's not in there today. OK? So promote model dimensions. We can promote dimensions that are created originally in the model as a sketch parameter or a function feature parameter.

Why should we do that? Well, there is a big advantage of having these dimensions promoted. Because it takes over tolerances and the dimensions, and you will see later on in Stephen's presentation that Stephen can drive the information back to the model parameters, then.

So we can modify some things in the scheme and he will send it back to the model. So the model will change. The tolerance in the model will change based on the calculation we make, OK?

So that's the big advantage of having the model promoted instead of doing it manually. Because if you do it manually, if you put in a dimension on geometry, it's just geometry. He sees not the driver of the geometry, OK?

How to promote dimensions. Pretty straightforward. Not this one, but here, for example. So you go in to the sketch. Where are you? Not here. Here for example. You can say here, show dimensions.

If you click on dimension, you click on it, right click on the dimension. Then there is an option, promote. OK? Now this dimension has turned in to a 2D annotation instead of a dimension. OK? So I can hide this.

Say you take this over. You take this tolerance over, and if something changes here, it's updated. It's linked together with this. All right? Which was it? This? So that's how you can retrieve dimensions.

See, you can preferably add your own dimension manually. It's possible. It's like dimensioning to a drawing. But this is not driven to geometry afterwards. Big difference. That's what I was telling.

Say just, by default, it's enabled to have this link. You can disable it. You can promote a dimension and then disable this link. It's possible. But I wouldn't do that.

Holes and threads, there's something that you need to know there. If you do a hole, retrieve hole information, the quantity doesn't show up. If you have a pattern, let's say of repetition of holes, it doesn't say the number of holes that are there. You have to use a tolerance feature to show the quantity.

Something that is driven by Sigmetrix engine as well, I guess, this tolerance feature. So they pick it up. But if you just do the information in a drawing, you can see the number of holes. It's not in here. You won't see the number of holes. So that's different between three and two.

Then surface texture. There's nothing different with what we can do in 2D. Same weight to put it on. So that's what you have here. There's now a new feature that's, there is an all around symbol. But it's just standards.

In text, you can have parameters coming from your model. So you can type texts like, for example, sets the radius of chamfer there. You can say, this chamfer, and use a parameter coming from your model to, let's say, populate this texture, which is then automatically updated and changed.

General notes. We have four quadrants in your screen to put a note. Saying, for example, in my model of a valve, that all the non machine surfaces have to be paint in a certain color, for example. Or that this model goes with drawing xyz. That's general notes we can add in there.

And you can also have a general profile note, which is a general, let's say, tolerance note for faces that are not, let's say, have no specific GD and T information. You could say, OK, take care of all these faces with a flatness or, let's say, straightness a certain way.

The organized drawing views. You can retrieve information from the 3D model on a drawing view. So it's not really made-- the first intention is not using 2D annotations to prepare a drawing, because it's to just avoid [INAUDIBLE] drawings [INAUDIBLE] big information.

But you can retrieve this information. So if, when you populate a drawing with, let's say, overall dimensions you create, that can be a good one. Inspection dimension.

So if the engineer was thinking about this important dimension, the draftsman can then retrieve the information to populate his drawing views without rethinking or guessing what can be important. So that's a good use of this 3D drawing, the dimensions.

AUDIENCE: [INAUDIBLE] drawing [INAUDIBLE] changing those in a 3D environment won't [INAUDIBLE] 3D environment.

PETER DE STRIJKER: If you have the promoted one, yes. It it's promoted, yes. If you had it manually, no. It doesn't drive geometry.

AUDIENCE: [INAUDIBLE] updating the 3D environment? [? Do you ?] [? use ?] 2D?

PETER DE STRIJKER: Oh yeah, delete. You mean delete?

AUDIENCE: Yeah.

PETER DE STRIJKER: No no no no. It's just a visual copy. No, you don't delete it. I'm sorry. I thought change. No, it's just a local representation of that annotation on a drawing. Yep. OK. And then the export.

The export, there is a list of CAD exports. And I think the only one meaningful in that list is the Step file. Because Step AP242 supports GD and T information in the model. So if you open that, there is an option here, 242. If you have, on the other side of the chain, someone who can read and capture the information, this information is built in here automatically.

If you export a 3D PDF, automatically Step 242 will be added to the PDF file, which gives you a good capability to communicate how a product has to be modeled.

He has the model in 3D, and he has the physical model, let's say, the CAD file, that he can use for his production. [INAUDIBLE] production. Yep. OK? So it automatically normally, yeah, you can unselect it. But standard, it's enabled.

AUDIENCE: So that's key one, right? That's addition one. [INAUDIBLE]. That's addition one, right? 242 is going to--

PETER DE STRIJKER: Yes.

AUDIENCE: [INAUDIBLE]. Is that-- are you guys going through a third party device [INAUDIBLE]?

PETER DE STRIJKER: It's a third party application. It's a third party vendor who makes these 3D annotations.

AUDIENCE: [INAUDIBLE]

PETER DE STRIJKER: Or this 2D PDF, sorry.

AUDIENCE: How soon you guys [INAUDIBLE]?

PETER DE STRIJKER: You know the step, the step? All will be using the Autodesk trans-- the ATF technology. It's the standard that all Autodesk applications use. So if Autodesk, let's say, implements the new version in this ATF, then it will be in Inventor as well. OK?

And recently in the last version of Inventor, we also support DWF or the, let's say, model annotations in DWF files also, which does not contain the 3D-- the Step file. [? Step ?] file. But you have this annotation visible.

And you also see the design view is in this list. So you can pre-define some 2D views if you want. It depends on what your production site can read. If he only is allowed to read 3D PDF files, you can send a PDF. If it's internally, this works perfect as well.

The model-based definition is also supported by API. So you can use the API code to organize these things inside the drawing. Or for example, to build a link to CAM and CMM software. So this API available of this information, which is very important to automate your processes. [INAUDIBLE].

So that's, in short, an overview of what we have in Inventor today for these model-based definitions. The real meaning of this information is to use it further downstream in this production. You have to-- you can put information in your model, but if you can do anything with it further, it doesn't make any sense.

So where can we use information besides only make a drawing of it? Well, the first thing is the stackup tolerance calculation. And I think Stephen can tell you more about that, because that's his part of the show. I have a clicker, as well.

STEPHEN WERST: This scroll? OK, I got it. Thanks, Peter. So I will be very brief. I'm just going to do a quick overview of the EZtol product. Again, this is a product that was launched last month for Inventor, our first product that we're selling as in Inventor add-in.

Before I start though, just a quick show of hands. How many people have either, you know, done tolerance analysis before in their own designs, or worked with people who do or understand what they are? OK, tolerance stackup analysis is typically what it's called, what is referred to.

So up until this point of the presentation, what has been described is how to define correct tolerance information. A lot of it focused on GD and T. And from that perspective, the tools that have been discussed help you understand which symbol is the correct symbol to use, or combination of symbols. What doesn't make sense?

And that's where the Tolerance Advisor provides that feedback in terms of the accuracy of the GD and T definition per the standards. What it doesn't tell you, though, is whether the number you have in that field is correct. That's the realm of tolerance analysis. And it doesn't have to be GD and T.

What I'll actually be talking about and showing is a stackup involving parts that have both GD and T annotations applied and standard either promoted dimensions and tolerances, or annotations that were added. It does need to be part of the PMI collection for the tool to automatically utilize it.

However, you don't have to have that information for this tool. What I'm going to show you is utilization, because that's the subject. And so what we're talking about here is to make sure that those tolerances that have been applied are correct, and your design is good, before the transfer to manufacturing.

So in terms of the downstream reuse of this information, we're that first step. We're just trying to make the final analysis function, if you will, of design a little bit easier, utilizing the work that you've done this far.

So what is EZtol? We've actually started with the ground up with this tool. And it was-- I won't go into all the history. We have a lot of objectives, and I've highlighted the ones here in the main bullet points. And these are the ones we're going to show very quickly in the demo. And it is going to be very quick.

First of all, we want a tool that lets you do those stackup analyzes on your models very quickly, with as minimal clicks as possible. That means, if you have tolerance information in the model files, we're going to use it. If not, that's OK.

You can still apply the tool. There's more information you have to type in manually if you just have it on your drawings. But again, we've tried to optimize that workflow, as well. Also, as you define your stackups, you know that you go from part to part to part to part.

Well, if you have functional assembly constraints or joint definitions within Inventor, we'll utilize that to create that stackup loop automatically. Again, you'll see that in a minute. Typically when you're working with your designs, there's not just one thing that you want to understand.

You want to understand multiple things. And if you're using spreadsheets, that's our number one competitor, to manage that, that can be problematic. If you have a dimension that influences more than one stackup, now you have to maintain those relationships in the spreadsheet.

It can be done. It's subject to error and kind of challenging to do. It's not technically challenging. It's just a lot of work to make sure those links are valid. We take care of that automatically for you. We show the results in a dashboard.

And whether you're using [? mix ?] worst case, RSS, or generalized statistical analyses, you can actually define that at sheet stackup level. And then of course, doing the analysis, modifying the results, modifying the tolerances, getting the design good, that's certainly an objective.

But inevitably, we're got to tell somebody else what we did. And so we include a very easy to use comprehensive report to show others the results of all your hard work. Right? And that's what I'm going to demonstrate very quickly and then turn back over to Peter.

All right. So the demonstration, thank you, is going to be on this caster wheel. It is one of the models open. And I'm driving somebody else's computer, so bear with me here.

Specifically, what I'm going to study on this is, you see there's a slight gap that's designed in between the wheel and that bushing. Pretty important for that wheel to roll, right? We don't want that going to zero.

And so one thing I'll also show you very quickly on this wheel is that this and all the other parts have tolerances that have been applied to the model. In this case, I'm going to point out this.

The wheel width, which is going to be part of this gap calculation, is controlled with this limit tolerances of 38 and 1/2 to 39 and 1/2 millimeters. OK? Just want to highlight that, because you'll see this again in a minute.

So coming back to our model, I'm going to start the environment. It's an EZtol. It gets added in. And when I start the application, you'll see that the tools, they're in the ribbon to define your stackup. I'm going to start by defining [? me a ?] stack up, and it's going to prompt me with a mini toolbar prompt to select things.

First, the two things that I want to measure between. And in fact, if I move my cursor off the selection, it's going to tell me on the cursor to select a face, an edge, or a vertex. It's kind of guiding me through the process. Again, we're trying to make this as easy as possible from a process perspective.

So I'm going to select the first face on the left side of the wheel. I'm going to select the right face on the bushing. It's asking me for an analysis plane. This is really an annotation plane.

Now the annotations that you're about to see are a little bit different than the ones that Peter was talking about. Those are part level annotations that get transferred to somebody else. These are only specifically for this analysis, which you're about to see.

So I'm going to select this space as my plane. I'm going to place my dimension just above it. Let's say, right here. That looks good. And now the next step is going to say-- and this one millimeter, that's indicating my nominal gap. OK?

That's the design gap that I have in there for the wheel between the wheel and the bushing. And I want to make sure that, with all the tolerances of all the parts that go into this, that gap is not going to go to zero, OK? The next step then is to define the loop, if you will.

Now, if you don't have functional assembly constraints in your model, we can certainly utilize that. But the tool is actually telling me that it found four different paths. And if I highlight these individually, it's basically going through my balls in different combinations.

OK, so I can quickly see, I'll use these front bolts very fast. I'll select OK. And almost like magic, that loop definition is defined. Ah, that's not what I wanted.

If I look over here, here's a list of all the parts, all the dimensions, all the tolerances that go into that stackup. At the bottom is my results. I'm going to give this a name. I'll say, axial clearance. I'll just call [? it wow. ?] Right?

And I see that, by default, the tool assumes you want to have something greater than zero, a distance greater than zero. Because 80% of the [? more ?] that is stackup analyzes that most people do is to guarantee clearance, make sure that the parts are not going to interfere. So we start with that assumption.

Does that mean that's the only thing we can assume? Absolutely not. We could have completely symmetric upper limits, whatever requirements you have for this distance, we can set. But at worst case, this is not working.

My requirement is zero. It's telling me, with the tolerances I have assigned, there's up to a 0.99 potential for interference at worst case. Well, there's a lot of things that are contributing to this. I can see the list of contributions in the contributions graph. And I can scroll down and see there's a lot of stuff has to be at its limit to ever get to that 0.99.

Maybe this is a good one to treat statistically. So I'll go down and say, instead of worst case, I want to do this as an RSS. And as soon as I select that, the results change. You have a kind of a normal curve, but you're still in a rectangle. And now the lower result is 0.264.

So now it's saying, yeah, 0.99 is the theoretical worst case. But in terms of probabilities, there is still a pretty good probability you're going to have interference. So let's use our contribution information to see what's driving that.

We'll see it's the width of the wheel. And all of these things can be renamed to be more meaningful. I'm not going to do that right now. I'm just going to change this to a symmetric tolerance and change it from 0.5 to 0.1. My results update in real time.

And if I go back to the wheel, notice that now my tolerance is at plus or minus 0.1. So now we're not only utilizing the information from your CAD models, but we're linked to it. We're not going to change the nominal. We don't want to break your geometry. You know how best to move surfaces. We can update the tolerances, though.

And that's what this link icon on the right hand side of each of these rows indicates. The tolerances are linked. As I make a change to my tolerance in my analysis software, it's pushing that data back upstream. If I want to do a what if and not make the change, I can break it here. Not a big deal.

All right, so that's one stack up. I'm going to do a very click next one and then I'll turn it back over. So for this one, what I'm going to do is look at, OK, let's say this wheel has to fit into a cavity. I have a restriction on the overall width, so I just want to understand what is the overall width going to be.

I'll just do a quick analysis between those two surfaces. Use the same path that I did the first time. There's the next analysis. I forgot to do something a minute ago. Because I said I want to report on this, let's take a snapshot of this.

And there's a nice little shutter sound for those who enjoy photography. I'll say, this case, I want to have an upper limit of 131.5, let's say. And just to show you that-- that's not what I-- and just to show you that we can do other types of tolerances, I can go and just show that we can change geometric tolerances on the fly.

You'll see that the position of those holes is held within 0.2. Well, if I go back to my analysis and change the position of the holes from 0.2 to 0.1, notice it changes both here and here. Because on that callout, it's a 4x.

So any instance of that hole is going to automatically change. And it changes it to 0.1. Right? So last thing. I think I got a snapshot of this one. Let me take-- it's my settings.

There is a snapshot I want to use for that, let's say at the top level of the assembly. There's our dashboard that we're starting to create. So I want to use that-- getting a little crazy with the mouse. Oh, I don't have a snapshot yet.