A Collection of Hot Inventor Tips
For even the most seasoned users of CAD software, tips and tricks are always in demand. It’s what piques our interest in using design software—knowing that you can always learn something new or a different approach to a common problem.
In this article we will take a look at several tips I have found over the years as well as a new one in the 2013 release that not a lot of users know about.
Are You In The Loop?
This tip brings one of those “aha” moments when you see it for the first time. It doesn’t mean what you were doing before was wrong, it just means perhaps your method wasn't as efficient as what I am about to show you.
A common modeling question is: “What is the best way to center a hole on a face of a model?” Make a constrained sketch? Link model parameters to a linear placement? Well, if it always has to stay put in the middle, then let’s use a Work Point instead.
With this method, we are going to place a Work Feature on the face that will always stay in the center of the face regardless of geometry change on the face itself or the rest of the model.
To place the Work Point using just the Work Point command and not the menu flyout, start the command as usual from the ribbon or use the period key for the shortcut. Right click and choose Loop Select to enable that type of selection.
Once you select the desired perimeter loop, the command will place a Work Point on the face that will always stay at the center even if the original parent reference geometry changes.
From there, start the Hole command and choose the On Point placement method. Select the Work Point and then chose a direction reference for the Hole. This can be an edge, or as I have used it here, one of the origin axes.
A Scaling Effect
Usually when I start sketching a new part file I take a semi-unintelligent approach and just throw together the rough shape of the geometry first before I put any dimensions on it. In recent years with the advent of the Dynamic Input and Dimensioning, I really should be doing dimensions and geometry at the same time, but old habits are hard to break. I originally learned to build a simple geometric reference and then control the sizing with dimensions placed afterwards.
When I did this in the past, if I wasn't careful about how much magnitude I gave a certain sketch object, my model would end up being blow out of proportion by my first dimensional change to the model.
But now I get to be extra lazy thanks to an enhancement in Autodesk Inventor® 2013. Now I can sketch something and even if my overall scaling is way off, when I put my first dimension in, it will automatically scale the entire sketch based on that first dimension. Notice in Figure 3 how it changes the entire geometry based on the change made from the .125 to the .5 dimension value.
One thing to remember is that you cannot have more than one dimension on the sketch for this to work. If you have two dimensions placed, simply delete one of them and then this trick will work with a change to the remaining dimension.
A Link to the Detail
There are not a lot of settings that need to be set in an Assembly template for Inventor. Let’s face it; most of the focus goes to the Drawings or Part template settings, but Assemblies? What is there to have in Assemblies for a template? Well that all depends on how you accomplish your work and how big your designs get.
If you design large equipment, AEC content, or have to supply customers with simplified models you probably have already heard of Level of Detail Representations in Inventor.
Level of Detail or LOD is commonly used to suppress components that are not needed during a particular time in modeling, hence making the opening and work inside an assembly file a little less frustrating. Think about it—is it easier to open a file with 2,000 parts or 200? If you have a 64-bit, high-RAM CAD station, you probably don't care either way, but if you are working with a five-year-old box that management refused to upgrade, you definitely have an opinion on the matter.
Inventor ships with system defined LODs called Master, All Components Suppressed, All Parts Suppressed, and All Content Center Suppressed.
Master: Everything is loaded (unsuppressed); no exceptions.
All Components Suppressed: Suppresses all children of the assembly, which results in a fast load of only the assembly file. Sub-assemblies are fully suppressed so that their browser structure is not visible. All Components Suppressed is the lowest-weight loading of an assembly.
All Parts Suppressed: Suppresses all parts at all levels of the assembly hierarchy. Sub-assemblies are loaded. You can investigate the assembly structure, constraints, and other attributes without loading part files.
All Content Center Suppressed: Suppresses all components designated as content, and does not load their occurrences in memory. For example, consider the hundreds of fasteners in a design. If the Content Center files are stored in a remote location, reduced network traffic may also result.
As soon as you try to suppress a component outside this scope and try to save, you will get a message stating that a new level of detail will need to be created to accommodate the suppression. This is because the Master cannot be saved with a component suppressed. And you inevitably start creating LevelofDetail1 for the parts that are suppressed. But what if you already had a LOD in the Assembly? How about default LODs in our Assembly templates?
Template LODs accomplish two goals for us. One, it creates a defined LOD for me to categorize the work I don't want loading, and secondly since this LOD is in all my assembly files, I can use a command to link them all together. You may not have known about the latter option before. If you have a LOD in a lower assembly—let’s use "Customer Requested" as an example—when you activate "Customer Requested" at the top level of the assembly it does not automatically link that to the "Customer Requested in the sub-assemblies (left image below). What Inventor does do though, is if it is a system defined LOD (Master, All Content Center, etc) it will link those together (see Figure 5, right image).
So how does the linking take place? Well if you don’t know the next tool I will show you, then the process has to be done manually throughout your assembly structure and that could be quite tedious and time consuming for different LODs. Instead, use a tool that was introduced in Inventor 2010 call Link Levels of Detail. This little gem is located on the Assemble Tab > Productivity Tools Panel.
This command will look at the top level of the assembly and then automatically link the LODs that have the exact same name. That is why it was important for me to add them to assembly templates. Simply select the LOD to link, hit OK, and the software does the work for you. This can help you take your design to a more manageable size a lot faster and more efficiently.
Blank Slate Templates
Another tip that not a lot of users know about is the creation of a blank slate template. This will basically start up a new drawing with no Drawing Resources or Styles loaded into the document. This is the perfect way to start a new Company Standard for any and all styles as well as new Drawing Resources such as Title Blocks and Sheet Formats. It keeps the Inventor default styles manageable by not loading them all and gives you the power to start renaming them correctly from the beginning.
To start a clean slate template, hold down CTRL+SHIFT and at the same time select a new drawing from the pull-down in your Quick Access Toolbar.
The Styles and Drawing Resources will be blank, allowing you to start from scratch on your new Standard or Title Block.
Check Model Complexity
I received an odd request from a user about how to check the number of faces and edges a model contained. I was actually taken back by this request and had to ask, “Why do you care? What is that going to tell you?”
His response was something I should have seen coming. He was trying to import a file into Autodesk 3ds Max® and wanted to know how much of a load the faces are going to put on the machine. The answer is a versatile tool called Check Design. While it was used heavily to maintain sanity before passing off models to AEC consumers, it now has an added purpose with the Autodesk Suite bundling.
We can access this command on the BIM Exchange Environment. Start the tool and examine your results.
Figures 9, 10, and 11
Holy faceted faces, Batman! There are a lot of faces and occurrences in that design (Figure 11). Now let's imagine we used LODs properly and prepared for this eventuality during the development of this design.
Consider LOD or Substitute model in the place of this example; a reduction to a single component and a reduction from 74k faces to 13.5k faces. My AEC and Visualization consumers are going to love this version compared to the larger one. Oh, and I almost forgot, for my AEC folks I can add Omni class table information, connectors, and metadata to the file so our lives are a little more accurate than before. Remember this trick next time you are asked for an export for a 3ds Max user or AEC consumer.
I'm sure this has happened to you at one point or another when documenting with Autodesk Inventor. You start placing Base and Projected views and then maybe a Section, the occasional Auxiliary View, and then your Detail views. Design changes happen, documents update, somewhere its 5:00 PM and someone is enjoying a nice refreshing after work beverage, but not you. You have to fix those detail views that didn't move with your geometry when the design updated and changed. So how do we get out of work sooner and with fewer headaches next time? By attaching our detail views.
When you place a detail view in the drawing manager, after the initial placement you can move it around in case you didn't like its initial placement on your view.
This flexibility is also the reason why, when a design updates, the detail may or may not move with the update. This can cause incorrect dimensions (shown in Figure 12) as well as those pink orphaned dimensions we hate to see.
So next time you place your detail view, take an extra step and attach it to some geometry. This will essentially anchor it to a point so when it updates in the model the corresponding detail attached to it will also move in conjunction with it. Simply right-click on the center green dot of your detail boundary on your view and select Attach.
A View from the Top
The Inventor view cube holds many secrets. In fact, I could probably do an entire article on just that little guy. However, we’ll focus here on just the ability to change the top and front orientations of the cube and what that does for your models and drawings.
By right-clicking on any flat face of the cube you have the ability to change it to be the new orientation for top or front view.
Doing this will change a couple things. First it will change how your model shows reflections when you turn them on in the modeling environment. The selection of the top view is most important for this change.
Second, a change to the front grants the ability to have a predefined “From Model” understanding of what you want your front view to be when placing views into the drawing environment. Just make sure the settings in your Style Library accept the view from the model instead of using the XY plane. The latter would be common if you have reused your styles over the last five years instead of starting new ones.
This tip is one that I didn't really know was “a thing” until I was asked for it. In my past experiences I have never had a need for this type of documentation object, but who am I to judge?
We all know that most companies use ANSI as a guideline and have their own way of documenting and annotating their designs so when I was asked about this I immediately went to the “out-of-the-box” tool that should perform this type of annotating. I went to Sketched Symbol, but I ran into problems since the geometry created in the symbol would always require a similar quantity of text and never quite worked out to my satisfaction.
The solution is balloon overrides. You are able to attach it to geometry the same way you would a sketched symbol, but the software defines the bubble size for you instead of predefining it with a sketched symbol. Simply right-click on the balloon after placement and select Edit Balloon.
Next, choose a shape override if need be, and then start typing in the override area the information you need to put in the bubble. This will be single-line, no-carriage-return text—anything else you should probably put in a notes section on the drawing anyway.
What about an individual part? Surely this wouldn't work on a single part without a BOM or Parts List to speak of? Young grasshopper, pull up a CAD mouse and pay attention. You can absolutely do this. Simply start the balloon command and select your part. It will prompt you to create a simple BOM for just this part.
There you have it, a geometry enclosed leader with a perfect fit for you text.
I hope you have enjoyed a few of these quick hot tips and tricks. Now share some of your own with your co-workers and on the AUGI forums!