Did You Know? Hidden Command Options in Inventor.

JIM O'FLAHERTY: Welcome, everyone. This is Did You Know? Hidden Command Options in Inventor. I am Jim O'Flaherty, and I began my career in 1980 as a draftsman on the board. I've worked in numerous industries, a few of them listed here, mainly as a contractor. I started on Inventor Release 3. I was also the first commercial implementation of Autodesk Vault Workgroup. I'm an Autodesk Inventor Certified Professional, Certified Instructor on Inventor, and also an Expert Elite member. I've spoke at Autodesk University since 2015. I am also a speaker mentor, 2017 through 2019 and again this year. I'm also known on the discussion groups as The Angry Elf or The Angry Elf's Alter Ego.

My professional life-- I am currently the engineering training manager at Material Handling Systems. I was hired on about four years ago as their Autodesk licensing and support manager. I am currently now training and supporting in excess of 750 users worldwide on all our Autodesk applications, including Inventor, AutoCAD, AutoCAD Electrical, Navisworks, Revit, and Vault among many others.

MHS is the preferred supplier for conveyor systems for Amazon, FedEx, UPS, the Postal Service, Wayfair, and Walmart. Chances are, if you ordered anything online, it traveled on one of our conveyors.

And with that, I'll r off to Radu real quick.

RADU STANCESCU: Thank you. Thank you, Jim. So you see in the picture I'm the only one sitting there, actually, with the blue shirt. So that was one of my visits in Manila. Currently, I'm in Portland in Oregon, but I support training and other things related to Inventor and Vault in many other offices like in Asia, in Singapore, Vietnam, Manila, India, so kind of a very busy schedule at any time of the day and night. Like Jim, I've been teaching and training at Autodesk University for three years, I think. And that's me.

So next slide, Jim. Here is me outside whenever I have some time, whenever I find some time to do other things than work. I'm doing-- I'm running a lot, like ultramarathons. I like to hike mountains, family, and of course, food and drinks, like everyone, I guess. Next slide, Jim.

Related work-- what my company does, which is MiTek or Benson Industries, we do curtain walls, and we place them on buildings. It's a very easy process that could be complicated. These are some projects. You see the Manila Bay-- not Manila Bay, Singapore Bay in Singapore, One building in New York, and The New York Times, and a few out of hundreds over. You're next.

JIM O'FLAHERTY: And with that, I will take it back from Radu. Thank you, Radu. So most users learn the basic processes of commands and stick with them. But then they fail to realize that a lot of Inventor's commands have hidden or lesser-known options that can and will improve your efficiency in modeling and detailing. While this may seem very basic and Inventor 101 type-- this is Inventor 101-type class-- we hope you'll come away learning something new from this class as well.

So our class objectives today-- number one, what are hidden options, and where do I find them? Options for basic commands that will make them, well, not so basic. How to crop a view other than the default rectangular crop. How to put in Ordinate dimensions on a Crop view or Detail view. The User Interface/My Home options. Assembly options, and Analyze Interference options. Please note, this year, these classes are a lot shorter. They're not one hour long. They are now 30 minutes. There's a lot of information that we are not able to cover live, so please be sure to download the class handout as we go into much further detail as well as cover other items on this subject.

So objective one, what are hidden options, and where do I find them? So prior to 2021 release, those on older releases of Inventor, these hidden options are typically found on secondary and tertiary tabs within the pop-up dialog menu. For example, the Extrude command looks like this. You got the main menu, and then you got the More tab on there. You'll find some commands that have at least three tabs as well.

Now, for the 2021 release and beyond, the Extrude command now looks like this. And notice all your options are now up front and visible. There's no more tabs that you have to click, or nothing is hidden. Everything is right there and ready for you to use.

So, sure, some of you might say, "So what?" Good point, and I'm glad you think that way. Why? While these may seem rather obvious, it has been my experience, while users may know the options are there, they still don't tend to use them, either due to not being familiar with them or know what they actually do or even how to use the options, as well as what I call the comfort factor. Familiarity is comfort. People like to be comfortable, and they tend to stick with what they know. By moving these command options all into the main menu, users should start using these options when needed as opposed to doing an extra task or separate command. So the fact is a lot of users never bothered to look beyond that main tab.

So let's look at an example here. So you got the basic Extrude command. Now, let's say you needed a Draft. You could use the Taper option, and you can generate that Draft to that operation, avoiding having to add another command and feature. Now, again, you know your product better than anybody else does, so this may not apply to you in that certain instance, but then again it could. So knowing the option is there, it's up to you to use it and utilize it and use it to your advantage. So again, as you can see, you put that Taper on there, and that could act as a Draft for that particular feature.

So some quick examples-- the Loft command. So as you can see you got the Loft command, and you got the Condition tab, which is the second tab over. It will offer a wide variety of results depending on what you select. So you got the different option here. You play around with it and see what works for what you're trying to design. Again, you know your product better than anybody else. Work smarter, not harder.

So more quick examples on the new menus-- the Hole command. You got Preset options, and you got the Advanced Menu options. The Advanced Menu option icon is numerous commands. These options change per command and allow you-- how you interact with that command. So definitely check into them, see what the options are, and use them or apply them as needed.

The Fillet command-- although it's located on the main menu of the Fillet command, one of the items that users seem to miss the most is the Click to Add option, as you see circled here. This allows you to literally insert all required fillets in one command for that entire part. The second tab on your Fillet is for Variable Fillets. So it allows you to do just that. One fillet has variable radiuses. You can put them all into one command. And then the third, you're allowed to adjust the setbacks for each fillet at their intersection.

Objective number two-- Advanced View Cropping. So if there is one command that users seem to stick with the default setting or simply do not know that it can be done more efficiently, it has to be the View Cropping command. Now, the question is, that's fine and dandy unless you have an Iso view. As you can see here, I got an Iso view. And in this first picture, here is your Crop window. What if I don't want all this extra info included in here? Unfortunately, using the default, that's all you got to play with. Well, there's a better way of doing it.

So step one, select the Iso or the desired view, make it active, and then press the S key. That will put you into Sketch mode for that view, generating a view-based sketch. Step two, sketch the desired boundary of the crop that needs to be-- and it needs to be a closed loop, and constrain to prevent it from shifting during any kind of edits. Step three, select the Crop View command, and then select the Sketch. As you see, it's highlighted here. And then step four, finish the Crop command. Adjust the line appearance per your company standards. Much better, much cleaner for an Iso view. The key thing is any shaped sketch will work as long as it's a closed loop.

Objective three, Ordinate Dimensioning of a Crop or Detail view. So creating an Ordinate dimension or a set of, in a Detail view, has always been a bit of a head scratcher. And this has always-- this little trick has been a hit in a lot of my classes. So I want to demonstrate this and show you exactly how to-- this will be shown step by step in the handout. So this video may go through quick, but we'll definitely have it step by step within the handout, so check that out.

So here, we have a view that-- a Detail view we have sectioned off, and we've got the dimensions. So what you want to do is you want to open up the browser until you get to that part, and then right-click and select the Include Work Features and make visible whatever you're using as your origin. So here's your origin point. Granted, it's off the drawing in this case. Select a view, and locate the origin for the Ordinate dimension. And then go in and select your lines as you normally do.

Continue the command. Place your dimensions. Finish the command. And now, you could come in here, and you can adjust your Ordinate dimensions so that they're legible if they're close to each other. And if that origin is on the drawing and you don't want to see it, right-click it, and de-select the visibility for the point and for the indicator. Pretty nifty. Like I said, this little trick definitely helps. I've seen a lot of people that scratch their head on this.

RADU STANCESCU: And the first slide is about My Home. And I lie here when I say the most visible is an option. I mean, is it visible, or is it hidden, right? So, My Home, it's on the main screen, and I will share my screen right now in Inventor. And this is the Home button, OK? You may see it, or you may not. And actually, I am demonstrating right now. It's live. And under the general tab here in the tools application options, you can actually have My home displayed or not. And it's going to show like 50 documents, the most recent. They're going to be listed here. Maximum 50, you can change that. So if you want to see it all the time, just click on it, and I am doing it. So if you ask me if I like it, yes I like that.

Something else about here, you're going to see the New, where you can start any type of Inventor file and some other information here on the left. About depending what you have selected, projects, or shortcuts, or file details. And if Projects is on here, like blueish, then you can see previous projects that you played with or the current one. And then, on the right side, you have information details. And for the file details, just to show, if you select a file down here, it's going to provide more information, like location and other things that you have set up.

Next one. That was My Home, and I display the project and the file details. Next slide would be about the down panel here, what you see here. OK, so, down here, you're going to see the recent files. And what I like about that, maybe you know, maybe you don't, you can pin a file. If you pin, it's going to be always there. If you unpin, it's going to be displayed, or if you have other files, it's going to go to the end. But if it's really important, like for me, this assembly is very important. I like to pin it, so I will always see it there. So that's very important right here. And also, you can drag this down. And you can see more options depending what you would like to see.

Next, very important here on the left, I don't know if you knew about, but you can actually sort files. You can sort by recently opened. That's the default. Or you can sort by the name, or by the location. I like the default one. And also, when was it modified. Like last day, I want to see the files I worked last month. Inside the files, by default, again, is all days, the most recent ones. And what type of file you would like to see again? Assemblies, drawings, if you have a vault project, you might get more options here. So this is actually very important. Pinned, you can pin it so you can see it all the time. And what do you want to see? You want to see active projects or even all recent documents? If you switch projects like I am doing, you can see here I have several projects that I work on almost daily. Maybe I want to do the all recent.

And next one, next slide, now you see my PowerPoint. I'm going to talk about this too. You can resize. So maybe you notice, maybe you don't. Depending on what you would like to see, you can grab that. Of course, you can grab this one too. Interesting about what this open does, if I go to my project, that's my project, and I go to the File Details It's whatever file you have selected. If we hit open, see, things appear and disappear. So it's very important when you drag this that you cannot discover other things. So if this is selected here, the open shortcuts is selected when you click on a shortcut, on your active project, it's actually opening Windows Explorer. See, this is Windows Explorer.

If you don't select that. What's going to happen? What's happening now? If I click on the same file, it's going to open within the software. You see its Inventor open. So if you want to open from the shortcut, just go there. You don't need to go open and then find the shortcut. You can see them right here. That, I think, is very important. OK, next one. Now you see my PowerPoint, and we're ready for objective number 5. On the 5, let's see. So we did drawings now, let's do some Assembly.

In the Tools options, let's go to the Assembly. So I'm going to share my Inventor. And in the Tools options, in the Assembly here, I really like a couple settings. Maybe you guys like it, maybe you don't. But I do like them and the audio notification, I do not like it. This here display component names after relations and place and ground force component. This is actually pretty good. Because when you start a new, let's say, start the new Assembly and place a part, it will always match the origin of the part.

And I only want 1. It will match the origin of the part with the origin of the Assembly, which is very, very nice. You don't need to add any constraints or anything. So you can see here in the browser the YZ on the left, the YZ there, x-axis, and of course the origin is on the bottom left and bottom right. And it's not moving. I mean, it's pinned in origin. So that's very important. I suggest you do that.

And the other setting would be, let me go back to the assembly. It's place on ground, we saw that, display component names after relations. So if I add another one and how to add something else, Control+C, we all do it everywhere in emails and documents, right? Control+V, and just paste another one. And I want to add a constraint, and again, just instead of going there. You can see it's C. We can always C and get the command.

And I want to add a constraint between this and that. It's very easy, very basic constraint. As you see here, in the browser what files actually open, and also not these two, sorry. And then under the made, they're both listed. That's because the setting. And if I go back there, let's just see what's happening if you don't have it. If you don't have it, click apply, it disappears. So you see Made 1 but you don't have a clue what Made 1. It's between what components. So I really like that. If you select it here and it's going to display in the Inventor browser.

So that was a good thing. I like that it's very easy, but you have to know about that, like many other things in life. So let's move to the next one that's my PowerPoint. We talk about object number 5. Let's go to number 6. So number 6 is about Analyze Interference. Maybe you guys use it. Maybe you don't. But you know we're talking about Inventor it's 3D, so interference is very important. That's why you move from 2D, right? So in any Assembly, you can see if there are components sharing the same volume. I am sharing my Inventor, and I can close that file, I don't need it anymore. And I have a message here. To help you see if I have interference between parts here. And that's actually really a model from my work. I didn't create this just for this session.

It's under Inspect and Analyze Interference, Define Set #1. You can actually select all together, is the easiest way, and click OK. And that's very interesting. I have 12 interferences. You see all 12 if you want to know and you can see them highlighted on the screen. I can Zoom in with my mouse, you can double click on any interference and it's going to Zoom in and it selects in the Inventor browser here, see I'm selected. And double click here, it's going to Zoom in here. But what I like to do is, you can actually go to it instead of double clicking, go to. That's from Inventor, you know, the basic icon. An it's going to do that. Reset, I don't know or not, sometimes I've seen people just close it and start it again. Reset, bring it back to the Home. So reset is very good.

What else I've got here. You can ignore some of them. If some of them just don't make sense to you, you can do the right-click and ignore. And you see, I had 12, now I have 11. Let's say I don't want that guy, I can ignore that. So now I have only 10. Why would I do that? Because right now, I can copy the ones that I'm interested in. How do I get them back? Of course, what people do they just close the dialog box, but we're going to right-click and Un-ignore all, and we're all clear. Say I want to copy them, you can just copy them, and they're placed in the memory. And then you can just go anywhere and place them. Or just-- I mean, I have my Outlook closed, but it's going to go really well. It's going to place them anywhere.

Or just print them. And, of course, I'm not going to print them on paper. You can go by PDF, so you can save all that information in a PDF. So that's actually pretty nice. And that's about the sixth objective. And please ask questions, ask like right after the session. Don't hesitate to ask about anything you learn. And I hope you learned something in the session. Even though both of us use both and we never cover, but if you have a question or something and we know, we will gladly help you. And again, this was objective number 6 about Interference, and that's a good characteristic. It's something very good for the 3D. And this is my last objective. And here we go. This is the end of the session, so again, go ahead ask questions and we will help you with anything we know. Thank you, guys.