Details, Details, Details—Tips and Tricks of Detailing in Inventor

JIM OFLAHERTY: Welcome, everyone. This is Details, Details, Details-- Tips and Tricks on Detailing in Inventor. I am Jim O'Flaherty. I began my career back in 1980 as a draftsman on the board. I've worked in numerous industries, a few of them shown here, also as a Autodesk reseller for short stint.

I started on Autodesk Inventor and Release 3. I was the first commercial implementation of Autodesk Vault Workgroup. I am also a Autodesk Inventor, certified Professional Certified Instructor, and an Expert Elite member. I've spoken here at Autodesk University from 2015 through 2021. I've also been a speaker mentor for 2017 through 2019 and again this year for 2021. And you will find me out on the discussion groups, known as either the Angry Elf or the Angry Elf's alter ego.

My professional life, I was hired on by General Handling Systems four years ago as their Autodesk licensing and support manager. I am currently heading up their engineering training group. We are training and supporting in excess of 750 users worldwide. MHS is the preferred supplier of conveyor systems for Amazon, FedEx, UPS, United Postal Service, Wayfair, and Walmart. If you've ordered anything online, as I'm sure you did during the shutdown of COVID, chances are your packages traveled on one of our purveyors. And with that I give you Radu.

RADU STANCESCU: OK, so this is Radu Stancescu and, like Jim, I have over 20 years experience with Autodesk software, especially like AutoCAD Inventor and Vault. And my job I'm actually working for My Tech for Benson industries. And I'm the one sitting there, the only one actually sitting there. And over this year at my company's training and support, that's one of my visits in Manila. And we have offices all over the world.

So, like I said, at My Tech we do actually a lot of stuff starting from designing. And first of all our product is curtain walls. You can see there famous buildings. And we design. We manufacture. We put it together the curtain wall. We assemble, install, and all the way to the warranty. So we provide the whole nine yards, like people like to call.

These are a few of our buildings, our projects, Marina Bay in Singapore, pretty nice building, actually. The One World Trade Center, the below right, New York Times. And we've got hundreds of other projects.

OK, outside of work, I like to run a lot. I go through mountains. I play soccer. I eat. I drink. Family guy, you know kids, wife and be happy with that. Jim, all yours.

JIM OFLAHERTY: Thank you, sir. So tips and tricks of detailing an Inventor. Do you wish detailing your drawings took far less time? Do you wish there were quicker, more efficient ways to get your detailed drawings done? This class will go over some of the tips and tricks that you can use in creating your drawings, as well as best practices.

So our class objectives today. Number one is Inventor drawing environment, how to deal with Views, detailing drawings, some tips and tricks in Dimensioning. We'll cover standard and custom Symbols, as well as modeling for drawings using View Representation and Model States Please note due to the shortened classes this year, there's a lot of information that we are not able to cover live. So please be sure to download our class handout, as we go into much further detail, as well as cover more items on this subject.

So legally speaking, drawings are in fact legal documents. They communicate all needed information about what is to be created for the customer. If the product is produced incorrectly, liability can be assigned to the responsible party based on the drawing and whether the product was created per the drug specifications or not. If those specifications are found to be wrong, that liability falls squarely on those who signed off on the approvals for the drawing, your engineer, director of engineering, quality control, so on and so forth.

You've got to consider the drawing is part of the contract. Because when they're all bundled together with the purchase order, parts list, bill materials, other documents such as ECOs and specifications, they're all part of that same contract. They're all part of a legal document.

So objective 1, inventor Drawing Environment Section Views, probably one of the more common types of views that you're going to use when detailing your assemblies and your parts. So it's pretty straightforward. But let's look at some issues or some way of doing it. And I want to point out a better way of doing this other than just your basics.

So here we have a part or an assembly. And we just want to come in, and we want to cut a section. So you select a section cut command. And notice that you get these little glyphs if you hit the midpoint or endpoint of a line. Use those to line up and eyeball your cut line for the section. Simply place it, right click hit continue, put in any information, as far as the identifier, and then locate. Easy peasy, right?

Well, there are other ways of doing this. So again, the key thing here is you want to eyeball your section cut line first. OK? So you can use those glyphs to line up. As you could see, you'll get the little dotted line that will line you up and keep you in line of that. And you can still just eyeball.

Once you're done, what this does is it creates a sketch. So after you place your view, you can double click on that section cut, or right click on it, and select Edit, as well. That'll through you into sketch mode. OK? Now this is very key to this. So you come in here and you can constrain that line, that cut, wherever you want that to be.

So we're going to put-- come in here. We're going to put out a 1/4 inch away from this edge. And say, OK, right click, say finish. That's going to constrain that cut line. Double click that line, automatically throws you right back into sketch mode. Again, you can edit that dimension at any time. OK, so here we'll do it again, select the Edit, here's your parameter. Once here, we'll select it. We're going to change it to 1/8 of an inch. And you can see it updates, finish sketch. And that'll update you, as well.

Something I want to point out here before we move on is do not go through the practice of drawing a view-based sketch to create your section cut-line. OK? We have found in a couple of years of process that by doing such, it can, in essence corrupt the file. So I believe, and this is just me. I believe part of what it is that, with section of view, it creates its own sketch in the process. So if you create a sketch, and then use that sketch to create another sketch, you basically create in a sketch within a sketch. And I think that that could possibly be why those corrupt.

We found this on a lot of our files, out of our [INAUDIBLE]. And this is what we boil down to. As soon as we stopped doing that process for the past two plus years now, we have not had a single drawing go corrupt in this case. So I would highly recommend eyeballing your cut in there first. Let the section view create the sketch. And then go back and edit the sketch constraint the way you need it. It's a better way to do it. I'll get off my soapbox now.

Breakout Views, so these are used to display components or areas of our components that are hidden by other components within an assembly model. And this kind of throws people off, because you have to have a closed loop sketch already drawn within the view. So let me demonstrate this.

So here we have an assembly. And again, if I go right up to the breakout command and select the view, I'm going to get an error. It's going to tell me there's no sketch loop in there, closed-loop sketch I should say, to use to make that cutout. So selective a view. Hit the S key. That'll throw you into a sketch mode for that view. And then go in and draw your cutout area that you want to use. So I'm just going to throw a [INAUDIBLE] here randomly, and close it off.

Again, it's got to be a closed loop. Again, have one sketch within the view. And Inventor will automatically select that once you hit the command. So identify the view you want. You can see it highlights in green or whatever color scheme you're using. And from here you can select the depth of that section-- or that [INAUDIBLE]

You can specify whether it goes all the way through the part. You then select the parts, at least in the assembly you can do this. You can select the individual parts. Hit OK. It'll cut right through that part and only that part, because that's what you selected to cut through.

So we're going to go through a few different examples here. From here, you hit the depth. And we could also do through again and like other parts. Again noted, the key point is here in assembly you can select individual parts to cut through. Or you can select the entire assembly.

And then we're going to do a depth, here. So section-- hit the breakout. I keep saying section. I'm sorry about that. We're going to do from to a point. So here go come in and put your depth, select an edge where you want that. And then it'll cut the break-out view to that depth from that point. So this is actually cutting in 1/2 an inch from that corner.

Objective 2, better drawing environment dimensions, tips and tricks, intersection dimensions. These require a few extra steps and a specific in order to function correctly, or to give you the dimension you desire. It takes a little finesse on your part. And you're good to go at it. So let's demonstrate this, as well.

So here come up. You got the part we're going to do some dimensions. Just select a dimension command. Select the first line. And then before you select the next one, right click and select the intersection option from the pop up, and then select the line. And you keep doing this in order. And then you get your intersection points there for that dimension.

So we're going to go through a couple quick little lessons here, little examples. Again, click the line first or your first point. And then select a line. Here, you want to right click and say I want the intersection of that line and the bottom line. That'll give you that dimension.

And then you can also do this from an intersection to a tangent. So select the first line, right click, say intersection with the bottom line. That gives me intersection. And then I find the tangency of that curve. And then place a dimension. And you got a tangency to an intersection. So again it takes a few extra steps, right click, select the option, and then.

Ordinate dimensions within detail views, creating an alternate dimension, or set thereof, in a detail tends to be a bit of a head scratcher for a lot of people. Once you learn a trick, you'll be able to impress your friends. So let's demonstrate that. So here we got a detailed view already cut. OK? And this is a shaft, and we wanted to dimension those edges on the shaft.

So, what we got to do is, in your browser, open it up until you get to that part, right click on it. And then select Include Work Features. And make sure that whatever works features you use as your origin is visible. In this case here, it's going to be the 0 point or origin point of the part, Select a view and then put the origin location there for the ordinate dimensions. Select your lines that you wanted to mention. Hit continue, as you typically would. Finish that. And you have your dimensions in there. Go in rearrange them as needed.

And if you have the indicator that's visible now and it happens to be on the drawing sheet, you don't want it, right click on it and de-select the visibility. And then for the origin indicator same thing, right click and say hide the indicator. And now that point and the origin location is not there anymore. So go in, there's your view. You're all set. Dimensions are all good to go. And with that, I will hand off to Radu.

RADU STANCESCU: So I'm back here for you guys. It's objective number 3. So number 3 and 4 coming up. This is about symbols, standard symbols and custom symbols, everything about the drawing. The standard symbols are predefined annotations. We all know where to find them in the Annotate tab, where a bunch of symbols that we can just use it. They come straight with the software.

So this is about the standard symbols. And I'm going to demonstrate here something, like that's the location where they are. So you can see Inventor. It's the latest version of all the symbols under the Annotate. And I'm going to just go away for surface. Because it's the first one. Click on the location and then you have to annote the detail.

So if I want to go like, let's say, some numbers here-- I'm not staying here to teach you how to do that. When you're done, you can actually save as a preset. That's the key of my demonstration. OK? I can go there and say, hey you, 2021 Vegas, right? We save it and I don't want another one. And you can go here and actually pick any other symbols you want. We actually at my company we use sometimes the welding symbol. It looks like this. And I'm not going to go through it. We can preset that to.

What's good about this preset is you saved it here. And if you go and create another drawing, like another new drawing using your template, when you go to the symbols, It goes to the surface. When you place it, you can actually have it. You can reuse it. So it doesn't need to be saved in a template. You just created one. It's in the memory. And you can just use it. You can actually alter a little bit. But it's all there. So this is a good start for preset. I think that was new like a couple years ago.

Let me go to the next one. So what do we have next here. We talk about standard symbols. Next one is custom symbols. Custom symbol is like what we create and we place them in templates. OK? So local sketch symbols, like we all know, they're going to be stored under the drawing resources. All the templates have drawing resources. That's where we have our bag of stuff, and we just use it.

And talk about all these custom symbols You can actually save all. We talked about that. That's the location. Actually, there is one drawing that saves everything. And let me show you a couple of things here. So about the custom symbol, actually I don't need this here. I am going to actually open another template. Because they are part of the template.

So I don't need this. It's been a little bit here. And then open from my template location. OK? That's what I have all my stuff. And it's called iFABORD. I for Inventor, because they have all the templates, too. So that's one of our template you see. That's my company. And all the symbols are stored here. OK? Under the sketch symbols, you can see them. We have [INAUDIBLE] We have glass information about stuff. So they are all coming with the template. They are custom.

I wondered if there is another symbol here. But that's a little bit more complicated than a sketch symbol. It's part of a sketch and added more intelligence, so I'm not going to go into it. Actually, I covered that last year. So we can find a lot of information about that. If you don't like it, that's not how we do. If you don't like it, if you don't use it in your template, it easy to get rid of it.

So how to create one symbol? What's the catch here? So you got the right click of the sketch symbol and say define. It's not new. It's not create. It's defined. And now you are in the sketch, right? You are in the sketch here. And first of all, I would like to add the picture. I want to add a few different things like a picture, [INAUDIBLE] association with a [? I ?] property, and then some geometry, right?

So let's go find an image. And I want the image to be like that size. And I need a picture. And because I love climbing mountains, this is Mount Hood. I'm in Portland. So I can see this every day when it's a clear sky. So you add the picture, which could be your logo right here in the template. Next, I would like to add a note. And the notes are-- [INAUDIBLE] have to be in the sketch. I put in the sketch here and I [INAUDIBLE]

I'm going to show the place here. And so my other screen, I'm bringing here. But I want to say, let's say Designer. Designer, and then I want the property here to be Designer and place it into my note, right?

I place it here, and I want to make it big. I just go with whatever is the highest number. And it's good. Maybe I want to size it and then move it a little bit. Oh, Designer, and it says Designer because I don't have any view here.

And the geometry, I'm going to just add the rectangle. You can add anything you want. It's the geometry, right? It's your symbol, your custom symbol. So this is just like a presentation how to do it.

And then save it. I would like to save it as-- I don't know-- Test. I like the word Test, it's easy. Oh, it's there. It saved.

And now, if you really like it, you save it in your template. So how to add it, you double click. You bring it here. It says designer.

And designer with nothing because we don't have anything. So I can bring a base. And I would like to bring, I don't know, a part. Let me go to my folder. We have a folder called Parts, just get the first one.

I want to make it here, it's a mullion. So that's fine. And as soon as you get a part in here growing, it automatically fills in the property. So that's the beauty of the Custom involved. OK?

You save it in your template. Because it's yours, you want to use at any time if you need it. And you can link a lot of-- after it.

So that was the customs involved. And we go back to the PowerPoint and let's see what we learn more about that. A bonus here, Revision Cloud-- this is actually very important.

Unfortunately, this is not coming with Inventor, OK? You have to install it from the SDK folder. I would suggest you go on internet, Google it, like ideas, inventor ideas, and then vote for it.

Because if you don't gather enough votes, the Revision Cloud will never be in Inventor. So right now, you have to install it, So you have to manually install it.

It's very easy. I'm doing it for 200-300 users every year. It's very easy, again, but you have to do it. And it looks like this. The Revision Cloud, right click, Close and Finish. You can edit.

It looks good, but again, you need to do it. So if you want to help, just go and vote. So we're going to get it implemented. Next one here, the Revision Cloud is not a default. Like I said, manually add it. It's right there.

And Symbol Mask, I'm not going to present anything because we are actually-- we don't have much time available. I cover that in my previous classes. You can go in 2020 and download and look at it.

It's just a custom symbol. But if you want your custom symbol to cover some of your geometries or dimensions or stuff, like a mask, you can do it. Just to be aware that you can do it.

Next one, let's see, objective number 4, and this is the last one. It's about modeling for drawing. We still stay in drawings. That's the class, Details, Details, and Details.

View Representations-- about View Representations, what can we do? We can set up visibility, transparency, a lot of things. I have to demonstrate something here-- very interesting. Maybe you guys know about that, maybe you don't. But it's very interesting.

So I don't need this. I can close this. No, I don't want to save it.

And I have an assembly here. In the master, that's the default. And let's leaning a little bit here.

So that's what we do, right? It's a curtain wall with horizontal, verticals, and a glass. So under the View Representations here, you can see the master and default. Always use the default. Don't go to the master. It's locked. You don't need to default-- use default.

OK, so what we talk about here are View Representations. You can create a new View Representations. Right click on New, and I'm going to call it a Frame. Let's call it Frame.

And I want to turn off Visibility because this is about visibility. View Representation is about visibility. Right click on a part. I go with [INAUDIBLE] So it's actually turning off.

I turn off that. I can turn off that, right click on [INAUDIBLE] And maybe this green part, right click [INAUDIBLE] So you just turn off visibility of some parts. I have some steps here.

And save it. If you don't save it, it's not going to be there for later. You save it. And this is the default. Default always has everything framed as what you have visible in your sketch.

Let's create a drawing. So let's go-- actually, I can use this drawing, maybe. In the drawing, I want to get a view of my unit. So let's use the-- but let's make it bigger and make it associative.

And you see Design View, I have Default. And I have Frame, right? So the Default looks like this. All good, right?

If I want a build of material for it, like a parts list, I go there in the Parts List, click on it, select the view, and place it. All very good, everything is in the place, right?

If I switch this to the Frame, the one that I just did it, less parts. The problem is, you see all the materials. So you see all the parts. That's not good, right? I don't like it. I like the build of materials automatically to update with what I see.

So how to fix that, you just have to edit the parts list. And under the Filter, you can actually add a View Representation filter. And I want a filter for Frame. You just do agreeing, check, and automatically updates. You can see I only have nine parts. So that's how you do it with the View Representation. You have to use the filters.

OK, so going back to the unit, and one more thing to show you. If I'm back in the Default, and let's say that you want to add more parts. I'm going to copy a glass and paste a few other glasses, like other parts, right?

When you go to Frame, they're there. So I don't want them to be. I don't want to go after I add them in the Default and then turn off this. The problem is, they come in-- they show up in the drawing too.

So you don't like that. I don't want that. So what can you do to avoid this? Well, let me delete this.

So if you want to keep it like that, because that's what I want, you can lock it-- right click and Lock. Now it's locked. I go to the Default, do the same thing, all good. If I go to the Frame, it's locked. It's exactly what I want.

Drawing is the same. And just to make sure, if it's a shear for the default, they all show up, frame-- very clear. So don't forget, lock your houses. I'm sorry, lock your View Representations. If you want to keep them safe, just lock them. So that was about View Representations.

Back to the PowerPoint and the next one. You see, I talked about Frame, the parts list, and lock your stuff. Next one, and the last one-- a couple more minutes-- it's going to be about modeling. That's the new kid on the block, Model States, in the latest version of Inventor.

And I'm going to do the same demonstration, where can you use Model States, I'm not going to read all of that. There is a lot in Help. Let's do it.

Go back to my model, I want to go to the Default and delete all the other glasses. So that's my Default and by the representations. Now I go to the Model State. Model state is right there, and I'm doing the same thing. Go New, and Model State, do whatever, I don't care, for a name now.

Simplified, actually, let's be professional-- Simplified, fast, Simplified. Now, the Model State works for suppressions. So you suppress parts. You go and suppress. Right click, Suppress.

That will save your memory. It's going to allow you to have more resources on your computer. I want to suppress that, right click and Suppress. Sure, I don't want that maybe to do more parts. Suppress, let's say I'm just suppressing some parts, OK? It's nothing, like super professional, but just some parts. You save.

So again, that's my Model State, my own one. I created that. By default, you have Master. Master has everything. That's the Simplified.

If I go back to the drawing and delete all these things, let's create another view. And that's the last thing I'm going to show here. I want my unit. And I want the Model State of the Master. And I want to look nice, make it bigger, rather, and that's it-- all good.

And again, we do the parts list, the parts list out of this. We place it here, all 11 parts, all parts list. What happens if we switch to the Model State. Again, the new thing in Inventor, you go here in the Model State. Don't go Design View. Model State, that's what we're talking about.

I go Simplified, it does this. And it's asking you a few things. Right now, it automatically updates the parts list. You see 0, 0, 0, 0, 0. You may be surprised, like why does it show all the 0's? But it's accurate, right? It's 0.

So Model State automatically updates your parts list, your build of material. You see 0, 0, 0. Any time you switch it back to any other model state, it's going to actually show the accuracy. You're going to see the accuracy here in the build of material.

So that's new. It's working very nice. I'm happy that we're actually using it.

What's next? So that was the quantity updated here in the PowerPoint. And that was my last slide, guys. So please ask questions, anything that Jim and I can help, go ahead and ask. We also cover Vault if you have a question related to the class about Vault or anything, just let us know.

But in the end, stay safe, healthy, be well. And maybe we'll see you next year live. OK, thank you.