At Autodesk University 2013, I was fortunate to be selected to present four classes. The class that had the best reaction and the most interaction was the class I presented on Autodesk Inventor® Sketching. I presented this class in a tips & tricks style, which went over well. After all, who doesn’t love to learn new things to shave some time off common, day-to-day activities?
[The class was MA1743 “Sketching with Autodesk Inventor” for those who want to look it up on the Autodesk University website.]
Before I dive into the content, the first question always asked is, “Where did you get all of these tips, tricks, and suggestions?”
First would be from my 14+ years of using Inventor. A person picks up a lot by just using the software for that length of time.
There’s an old saying: “It’s not what you know, it’s who you know.” But with Inventor, it’s really both. I’m always on the lookout for any step that will reduce the time or amount of work needed to get things done. I’ve gained significant insight by watching others using the software, across multiple industries.
I would love to give credit to each and every person from whom I was able to get a little “nugget” of information; unfortunately, I have forgotten most of the sources. However, here are some of my current favorite places from which to get information on using Inventor to its fullest:
- Autodesk Knowledge Network (AKN) – Replaces the Autodesk Wiki
- Design and Motion (Scott Moyse and John Evans)
- TEDCF Publishing: Autodesk Inventor Tips & Tricks
- CAD Geek Speak Blog
- Paul Munford (aka the CAD Setter Out)
- Inventor From the Trenches (Curtis Waguespack)
- Autodesk Digital Prototyping Blog
- IMAGINiT Manufacturing Solutions Blog (Mark Flayler)
Without further delay, here are the top tips and tricks from my presentation
Working with Sketch Planes
Quickly Creating an Offset Workplane
You can generate an offset workplane with a sketch on it in one step. With the Create Sketch command active, drag off the desired face and you will be prompted for the offset distance for the workplane.
Sketches Used to Define Work Features
Sketch geometry, especially lines, can provide an easier method for creating difficult-to-locate work features.
For an example, look at Ben Curtin’s example Inventor Holes at a Compound Angle on the Tata CAD Geek Speak blog
Project Flat Pattern
The Inventor Help feature defines this command as “Unfolds a disjointed face or faces into the sketch plane.”
Project Flat Pattern is great for the situations where you don’t need the overhead and advanced options of the Sheet Metal Unfold / Refold features—just wanting to reference existing geometry edges.
Dynamic Input is a way of working with sketch geometry that was originally introduced in AutoCAD®, but has been available in the sketch environment for the past few releases of Inventor. It “provides a Heads-Up Display (HUD) interface near the cursor to help you keep your focus in the sketching area.”
Input boxes will appear as you are creating 2D geometry showing transitional dimensional information about your geometry and it allows you to define the size of the object as you are creating it, evening creating the dimension.
A key aspect of working with Dynamic Input is the TAB key toggles between the various options, whereas ENTER will accept the sizes.
Values entered become dimensions when accepted [disable Persistent Dimensions if you don’t want dimensions created]. Dimensions are only created on the inputs for which you entered a value.
Some Things Work Like AutoCAD
There are many time-savers in Inventor that mimic AutoCAD, in a good way. Anything, big or small, that saves time is a good thing, as even the little time-savers over a day or week can add up.
- Just like AutoCAD, the spacebar repeats the last command.
- Just like AutoCAD, when drawing a line you can right-click and close the line.
- Similar to how with AutoCAD polylines you can switch between arcs and lines in the same command, you can, within Inventor, drag in the line command to create an arc
When sketching lines there are some press-and-hold options to generate constrained lines or temporarily switch into a tangent arc creation mode.
- If you press-and-hold off the end of any point, Inventor will generate a tangent arc from that point.
- If you press-and-hold and drag away from a line or arc, Inventor will create a perpendicular line.
If you press-and-hold and drag tangent-like from an arc or circle, you will create a tangent line. If you continue to press-and-hold as you create the line you can snap tangent at the other end as well.
Use Split to Adjust Geometry
We can use the Split feature to take a line or other curve and divide it into two or more sections.
When geometry is broken apart using the Split feature the geometry remains constrained, meaning it is a great method to generate construction geometry or to create points to snap to.
Text in the Sketch Environment
Text can be added to any sketch and then embossed or extruded to add features to your model. This can be used to generate things such as part numbers, dates, place of manufacture, brand names, and logos stamped, engraved, or etched into the component.
Sketched text can include model parameters, meaning that as the parameters update so does the text. The location of the text can be parametrically positioned by the insertion point or the text box can be enabled providing more fine-tuned positioning.
Geometry Text functions similarly, but will conform the text to a selected object—for example, wrapping the text to an arc.
Make Project Geometry Work for You
By default, when you project geometry from one part into another it is made adaptive and remains linked to the other component. While it is adaptive and associated with the other component, you cannot make changes to the project geometry because it will update as the other component changes.
You can override this behaviour by holding CTRL while you are projecting geometry. The geometry will be projected fixed in place opposed to adaptive.
Adaptivity has its pros and cons and can be a very powerful tool when you intend to use it. Unfortunately, the default behaviour makes it too easy to accidently or inadvertently make things adaptive.
You can disable the Cross part geometry projection options in the Application Options (Assembly tab) to flip the default behaviour. With these options disabled, you’d have to hold CTRL when projecting geometry to make it adaptive.
If you haven’t done so yet, I highly recommend disabling the two Cross part geometry project options so you do not accidentally create adaptive, cross-part associative geometry.
When geometry is projected from another component but not made adaptive, Inventor applies Fix constraints to ground the component in place. You could Show Constraints and delete all the fix constraints, but there is a faster way. Select all the geometry you want to be free so you can dimension or constrain, then right-click and select Remove Fix Constraints. This will remove all fix constraints on the selected geometry.
Constraints & Dimensions
Constraints control the geometric relationships, such as parallel or tangent, between sketch entities.
Always follow the KISS rule (Keep It Simple, Stupid!)
- Stability before size. Add constraints and then add dimensions. Consider accepting the default dimensions if you are expecting “big” changes to the size of your sketch geometry. To help avoid sketch flipping issues, change the smaller dimension values first then move on to the larger ones. Remember that the first dimension sets the scale of the sketch.
- Use geometric constraints as much as possible. Apply constraints first, then dimension, which is more efficient and reduces the clutter. Constraints typically represent the things that are assumed on a drawing when not dimensioned.
- Be lazy and keep it simple. There is a fine line between efficiency and laziness: Don’t try to be everything to everyone with one sketch. Instead of making one sketch to be used for every feature in the model, follow one of the golden rules of sketching: KISS – one sketch per feature.
- Only create in the sketch what you can work with easily. The moment sketching becomes work to fully constrain, your sketch is too complicated.
- Fillets. These are best as features and should be avoided in the sketch—the same is true with chamfers, mirroring, and most patterns. These types of sketch elements over-complicate the sketch and are better controlled as features. [Why are these tools there then? You may run into rare cases where you have to use them.]
- Fully constrain your sketches! To quote Curtis Waguespack, “The importance of fully constraining your sketches in Inventor cannot be overstated. “ To make the behaviour of your Autodesk Inventor sketches more predictable, constrain your sketch to the ‘Origin’ (0,0,0).
- Bonus Tip: You can have Inventor auto-project the origin point by enabling “Auto project part origin on sketch create”—[Tools>Application options>Sketch tab]. Be careful with fix constraints—you should never need more than one.
Horizontal and Vertical Alignment
The Horizontal and Vertical constraints can be used to align points either horizontally or vertically. The center point shown in Figure 12 is constrained so that it lines up horizontally with the midpoint of the vertical line and vertically with the midpoint of the horizontal line. The circle will remain constrained to these points even as the rectangle changes in size.
Make Automatic (Inferred) Constraints Work for You
Constraints are automatically applied as you sketch, but you can make this work in your favour. This auto-constraining is referred to as constraint inference. What Inventor infers is dependent on the existing geometry, the type of object you are creating, the Constraint Options, and if Constraint Persistence is enabled.
You can adjust the geometry from which the auto-constraint is being inferred by hovering (rubbing) over another object. For example, if your new line is snapping parallel (without exiting the line) you can hover over a line 90 degrees to it and your new line will now snap perpendicular.
If your new geometry is inferring constraints in a fashion you do not want, you can hold CTRL as you sketch and no constraints (except for coincident) will be automatically created. You can then add the constraints of your liking. Additionally, you can disable Constraint Persistence on the Constrain Panel flyout.
Constraint Options (available on the Constrain flyout) control which constraints will be inferred during sketching.
Use Degree of Freedom to Find Under- Constrained Geometry
Use Degree of Freedom to help find unconstrained, partially constrained, or fully constrained geometry. The easiest method to access is via the right-click menu “Show All Degrees of Freedom.” The DOF symbols will update as you constrain your geometry.
Center lines can be used to create Revolved Sketch Dimensions, which is a great way to dimension revolved parts such as Shafts.
You can create tangent dimensions if you know where to pick (keep moving until you see the icon change).
Save a step and build more intelligence by naming your parameters on the fly.
Use Sketches and Sketch Points to Build Hole Patterns
Any point in the sketch can be used as a hole center (not just hole centers) and you can quickly change points to hole centers by selecting the points and adjusting their format.
There are many opportunities where using rectangles, polygons, and/or offset can create the basis of hole patterns more easily, smarter, or in cases where the hole pattern is non-rectangular or non-circular.
Similar to AutoCAD, blocks allow for the grouping of objects into a singular rigid-shape. But this isn’t AutoCAD. Why should I use sketch blocks?
- In some situations, especially with a lot of geometry, it is easier to move and rotate portions or the entire sketch by first grouping it as a block and completing the operation on the single block entity.
- Sketch blocks provide a great mechanism to test function before fit and form, even using the part sketch in an assembly.
- Sketch blocks are the basis for the Layout feature to generate an assembly and parts.
Creating a block with Inventor is similar to creating blocks in AutoCAD: You specify the name, objects, and insertion point. [The insertion point is the point where the block is inserted by when placed into your sketch.]
Note: AutoCAD Blocks can be easily translated into Inventor Sketch Blocks as well.
The block instances will appear with the sketch, and the block definitions will be listed at the top of the browser.
Blocks can be constrained as any other 2D Sketch object using the Constraints (Horizontal, Colinear, Coincident, etc.) and Dimensions.
Mike Thomas was honored as the Most Distinguished Graduate from CAD/CAM Engineering Technology at SIAST, Kelsey Campus. He is a specialist in the manufacturing industry with strong knowledge on the Autodesk mechanical products supplemented with a solid understanding of document management, hardware, networking, and other Autodesk technologies. He is now the Technical Services Manager for Prairie Machine & Parts and is responsible for overseeing the engineering department’s technical operations and the department’s strategic technical growth. Mike recently started contributing to Design & Motion (www.designandmotion.net) and can be found on twitter (@aurbis).