Why is parametric modeling so hard? One minute you have a perfectly good model, looking fine, the next minute, EXPLOSION! I know that this has happened to you—it’s happened to me too.
How to Use Inventor Properly?
When I’m teaching Inventor I'm often asked, "How do I use Inventor properly?" Of course, there is no "right" way to use Autodesk Inventor. It’s a tool just like any other. We can use it for lots of different tasks, and in lots of different ways—all of them correct. So, how can we quantify a "well-modeled" part? I’ve given this a lot of thought—and I can only come up with two criteria:
1. The geometry must be correct (that’s a given).
2. The part must be easy to update (this is the tricky part).
The Benefit of Parametric Modeling
Autodesk Inventor allows us to build parametric models. Models that can easily change by adjusting the value of a parameter. This is awesome for building models that need to be adjusted in a predictable fashion (configurable designs). Or building families of components that are very similar (copy and paste, adjust a parameter, job done).
The Problem with Parametric Modeling
The problem with parametric modeling is that we must model in four dimensions. We model in the usual three dimensions, and we must also consider time, or the way our model might change over time. This change over time is often referred to as design intent. Building a model that can change in a predictable fashion takes a little thought and some planning.
The problem with parametric modeling:
It’s easy to unintentionally create relationships
Editing a feature causes all subsequent features to regenerate
Part updates become unpredictable
Design intent is lost
Time is lost ‘fixing’ parts, or remodeling from scratch
We would rather build our own parts, than reuse someone else's
Reliable Modeling Technique
Reliable modeling technique takes effort up front. Back in the day, working productively in AutoCAD meant mashing the keyboard faster. Working productively in Inventor is more like playing chess. It pays to sit back and think about what we’re going to do before we start. Reliable modeling requires a plan. Reliable modeling gives us:
Editable models—Design intent is captured
Obvious models—Design intent is documented
Reusable models—We would rather reuse than rebuild
What Makes a Model Complex?
If your model has only one solid body, and a handful of features, you don’t have to worry about your colleagues figuring out how to change your model.
If you're creating a model of a part that isn’t subject to change (for example a supplier’s component), you don’t need to worry about design intent.
Building reliable models will take you longer in the short term. Building reliable models will save you time, only if you will be changing a part numerous times in its lifetime, or you can reuse a part in multiple designs.
Reliable modeling is a prerequisite when using a top-down modeling technique, or building configurable content such as iParts, iAssemblies or iLogic driven designs.
Encouraging Good Modeling Behavior
When I was a CAD manager, I found diagnosing unexpected behavior in models to be a time-consuming challenge. One tool that I found helped me a great deal is the Inventor Design Checker. Autodesk Inventor Design Checker is a tool that can be downloaded from the Autodesk App store (it’s free for subscription customers).
Design Checker can be used to check for best practice in other’s models, but it can also be used by novice modelers to give them dynamic feedback on the progress of their model. Learn more.
Relationships in Inventor
The key to creating complex models in Autodesk Inventor is maintaining control of relationships. If you don’t understand the relationships you’ve built between parameters, sketches, features, bodies, parts constraints, and assemblies, your model will not update in a predictable fashion. The bad news is that Inventor won’t manage this for you (it can’t read your mind!). The good news is that you have full control over this process.
No unintended relationships
Relationships are kept to a minimum
All relationships are planned and purposeful
All relationships are obvious and easily understood
The Model Browser and Feature History
The model browser in Inventor is also known as the Feature Tree. Each item in the tree represents a feature in our model, for example, a hole or a fillet.
Features can be broken down into two groups: sketch-based features (Extrude, Revolve, Sweep Loft, etc.) and in-place features, or features that don’t need a sketch but do need existing geometry to be based on (Fillet, Chamfer, Shell, etc.).
The model browser is also known as the History browser, because it shows the order that the features where created in. Each feature in the tree can reference features further 'up' the tree (in the past). Features cannot reference other features ‘down’ the tree from them (in the future).
Features can be dragged into a different order within the feature tree, but they can’t be dragged ‘up’ past a feature that they are referencing, or ‘down’ past a feature that is referencing them.
These relationships are also known as Dependencies. Feature-based modeling is a powerful tool, because we can use these dependent relationships to add intelligence to our model.
At the end of the model browser is the End of Part (EOP) marker. You can drag this up or down the tree to temporarily suppress features.
If I gave you a model of a 50 mm x 50 mm x 6 mm steel plate, with an M10 clearance hole through the middle of the face, and asked you to change the width of that plate, what should happen to the hole?
Using feature-based modeling we can decide how our model will change. This is known as design intent.
Tip: Use the Feature Section Filter tool (in the Quick access tool part, green symbol) to switch between selecting faces and edges, features, and sketches. Hold down the SHIFT key and right click to bring the filter up at your cursor.
In the Feature selection mode you will be able to double click on a feature in the graphics window to edit it, rather than having to find it in the browser.
When you need to diagnose a model that you didn’t build, try using the relationships manager to help. Right click on any feature in the browser and choose Relationships. The selected relationship is seen in the middle of the Relationships dialog. The feature will be highlighted in the browser and in the graphics window.
Features that are required by the selected feature are seen in the box above. Features that depend on the selected feature are seen in the Box below.
Traverse the related features by picking on the 'Make selected’ (white arrow) button next to the feature you are interested in.
Edit the feature you're interested in by selecting on the ‘Edit feature’ button next to it.
Fixing Faults in Part Models
When (not if) you're editing a design and you get a failure, you’ll need to know how to cope. Understanding the modeling best practices in this article will help you to understand where the faults in the model lie. I also hope that this article will not only help you fix the fault, but also make the model more robust in the long run.
Here are some tips for fixing failures:
Drill Down for Help
Inventor will warn you of impending doom with a pop-up warning. Click on the plus symbol to expand the nodes until you see red text. Click on this red text to highlight the problem in the graphics window.
Roll up the End of Part Marker
Faults often cascade. This can look devastating, but often, fixing the first fault will automatically repair faults in dependent features.
The trick is to suppress all features below the first affected feature, by moving the EOP up. You can drag and drop the EOP, or right click on the affected feature and chose Move EOP Marker.
Fixing the Fault
If you know what the fault is, fix it! If you don’t know what the fault is, right click on the broken feature and choose ‘recover’ to start the design doctor, which will help you through the process.
Once you’ve fixed the fault, roll the EOP back down by a couple of features to check that they rebuild as expected. Keep rolling the EOP down a few features at a time, fixing problems as you go until the whole feature tree will rebuild.
Now. How would you have built this part differently?
Tip: You may not always be able to go back and rebuild every part in a robust manner, but there is always something to learn from inspecting other people’s models.
Sketched Versus Placed Features
You will notice that many tools are available in the sketch environment that are also available in the feature environment. Examples are Fillet, Chamfer, Mirror, and pattern. The advice here is to keep your sketches simple, use features whenever you can.
If in doubt—if the same tool is available in both the sketch environment and the feature environment—use the feature.
Diagnose failures—If anything goes wrong, it is likely to be in a sketch. Keeping sketches simple makes faults much easier to diagnose. Sketch-based Mirroring and Patterning in particular often cause problems and can be easily replaced with features.
Maintain flexibility—Features can be suppressed while you try alternatives.
Preserve design intent—It is much easier for downstream consumers of your model to understand your design intent when you use (for example) a hole feature, rather than a sketched circle.
Downstream functionality—Should your model be used downstream (for example, for CNC programming, FEA, or BIM) it’s much easier to simplify the model by suppressing features than it is to remove sketched features.
Relationships: Order of Preference
Some relationships are more complicated for Inventor to work out than others. When you're planning your design, keep this in mind. Create simple parametric relationships where you can, create complex feature-to-feature relationships only when you have to.
1. Parametric Relationships
Inventor is a computer program. Computers are really, really good at math. It may come as no surprise that the simplest relationship for Inventor to manage is a mathematical one.
Parameter1 Drives Sketch1 Geometry.
If you can’t express a relationship mathematically, and you need to express it geometrically, the safest way is to relate a sketch to another sketch. This is known as a Horizontal relationship—both sketches are on the same level. We are minimizing the number of feature relationships Inventor must calculate, and therefore reducing the opportunity for error.
Parameter1 Drives Sketch1 which drives Sketch2.
Creating a sketch on the face of an existing feature is a common workflow. It’s not wrong to do this, but it’s worth recognizing what you just did.
Parameter Drives Sketch1 which drives Feature1 which drives Sketch2.
We have now created a far more complex sequence of events which Inventor must calculate to get a result.
Powerful, certainly, but frustrating if we unintentionally created a relationship we weren’t aware of.
Feature-to-feature relationships are the most complicated relationships for Inventor to calculate, because it must calculate two ‘branches’ of features before it can compare the two branches to get a result.
Feature-to-feature relationships can be the trickiest type of relationship to edit parametrically, because you must make sure that all the contributing features make sense in order for the final feature to make sense.
Parameter Drives Sketch1 which drives Feature1 which drives Sketch3 which drives feature 3.
Parameter2 Drives Sketch2 which drives Feature2 which also drives Feature 3.
Paul Munford is a laugher, dreamer, bon vivant, CAD geek and technical marketing manager for Autodesk in the UK. Paul's background in manufacturing items for the construction industry gives him a foot in digital prototyping and a foot in Building Information Modeling (BIM). Paul was a speaker at Autodesk University for the first time in 2012, and he says it's the most fun anyone can have with 250 other people in the room.
Luke Mihelcic has been involved with design, engineering, and analysis since 1995. His career started in telecommunications designing mobile production equipment for TV and radio. As the technical marketing manager for the core manufacturing solutions at Autodesk, he is responsible for the development, creation, and implementation of relevant content and tools that help users understand and utilize the Autodesk Design and Manufacturing Portfolio.
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