This article was originally published in the November/December issue of AUGIWorld magazine for the Brazil and India markets only. However, I feel that the content is important enough to make the information available to everyone.

The goal of every user of 3D solid modeling software is to create models that are stable, predictable, and easy for others to modify in the future. All too often, users will take shortcuts in design, generate features without regard to how the feature may need to be modified, or create feature dependencies that affect the stability and editability. In this article I will explore some of the ways that we can improve our modeling skills.

Plan your model
For good design, everyone must plan out their model structure before making that first sketch. When planning a model, visualize the end product. If the part will be symmetrical, then a logical approach will be to model bidirectional from an origin workplane. A good example of this would be an engine connecting rod, where both sides of the part are essentially identical.

How will this part be built?
My connecting rod will be initially created as a forged blank. To assist in removal of the blank from the forging die, I will want to provide a bidirectional taper from the center of the part. As a result, I plan on using midplane extrusions with a taper. After the forged blank has been cooled down and trimmed, it will be machined. Since heated material expands, I will need to allow for the fact that the cavity in my forging die will need to be somewhat larger than the final forged blank. Therefore, I will be planning to create a scaled, derived tool body once the rough forge part is completed and before the planned machined features are created.

Keep it simple!
Try to reduce the number of features that you create in any one part. Quite often, we create far more features than are needed to complete the design. A complicated part will make modification or troubleshooting much more difficult.

Create sketches
Next, determine what objects should exist in that first sketch. Every sketch should reflect the design intent of the part being created. In my connecting rod example, my first sketch will include the major features of this symmetrical part. This allows me to rapidly create the main portion of the part in three simple steps. Midplane extrusions can then be used.

Figure 1: Connecting Rod Sketch1

Figure 2: Connecting Rod Blank

Fully constrain sketches
In order for a model to be stable, and behave predictably when changes are made, all sketch objects must be fully dimensioned and constrained. When sketching, make sure that the end result of the sketch will be a fully constrained sketch. Inventor indicates this in the bottom right corner of the Inventor graphics window.

If you cannot locate the constraint or dimension that is missing and preventing you from fully constraining the sketch, use the Automatic Dimensioning command, first with Dimensions unchecked, while selecting all sketch objects. If the result of this first pass with automatic dimensioning fails to fully constrain, then try again with Dimensions checked.

Reuse sketches
This sketch consists of three closed shapes. I have decided to create three extrusions using sketch1 by sharing the sketch. This will preserve design intent and the relationships of the three major features of the part.

I will use three separate bidirectional extrusions with a taper of minus 2°. Each extrusion distance will be different, corresponding to the design needs of the part. After creating the first feature, I will locate the consumed sketch in the browser, right-click on sketch one and select Share Sketch. I can then create the other two features using the same sketch. Once all three features have been created, I change the visibility of Sketch1 off.

Add sketched features
Before adding placed features such as fillets, chamfers, holes or other features that do not necessarily rely upon a sketch, you will want to add any additional sketched features to your design. By adding the sketched features before placed features, you will retain original edges to use for anchoring the sketched feature. Remember that in order to assure stability in your design, all sketches must be fully constrained and anchored within the part.

Watch dependencies
Sketch1 is always dependent upon the originally selected origin plane. Origin planes, axes, and origin point are the only permanent objects within any part file. Sketches based upon or anchored to any other created object are dependent upon the existence and location of those user created objects. User-created objects made be defined as user work planes, axes, and points, projected geometry, existing sketches, or created features. Work planes, axes, and points created by referencing origin features are generally safe to use as long as they are not deleted at some point in the design. These created work features may be turned off within the design, while still providing anchors for dependent features that reference them.

Sketched and placed features that reference previously created features such as extrusions, revolves, sweeps, lofts, holes, shells, chamfers, and fillets will be dependent upon the existence of the referenced features. If one of the referenced features is deleted from the design, then the dependent feature will either be deleted or it will lose its anchor to the original location.

You can determine feature dependency by trying to drag any created feature up or down the browser tree. Almost all features will fail to move at some point in the tree, revealing the dependent reference. Sometimes moving the dependent reference up or down the tree can reveal its dependent parent.

Add placed features
In my connecting rod design, I will want to add fillets to the rough part before I create the scaled, derived tool body for the forging die.

Mimicking the machining process is a good way to determine how to add features. Placed features such as fillets, chamfers, and holes are generally machined last. You will want to add these features to your design at the same stage. Once the final forged version is complete, we will be ready to make to derived parts.

Once the fillets have been added to one side of my connecting rod part, I am able to mirror the fillets to the other side by referencing my original origin plane where the first sketch was created.

When to derive a part
A derived part is a solid body without named features that is created from an existing Inventor feature-based part. A link is maintained with the original Inventor part so that any changes to the original part will be updated in all derived parts that are linked back to the original.

Derived parts have the ability to combine assembly components into one part, mirror or scale a single original part, or to derive specific areas of the original design.

In my example, after creating the complete forged based part, I will create two derived parts. One will be a simple non-scaled derived part where machined features will be added. The second derived part will be scaled to adjust for shrinkage during cooling. The standard derived part will scale in equal percentages in the X,Y and Z directions. For nonlinear scaling, an add-in may be installed that is located in the Program Files\Autodesk\Inventor Version\SDK folder.

Patterns
Inventor provides two different types of patterns. You may pattern within a sketch, or you may pattern features such as holes and sketched features. How you use patterns can significantly affect your productivity.

Sketch patterns should be used sparingly, as the additional geometry further complicates your sketch and the solving of constraints. In addition, you may not use this part feature created from the patterned sketch to pattern components in an assembly file.

The pattern feature will pattern an existing part feature such as a hole, extrusion or other created features. The pattern feature may then be used within an assembly file to place additional components automatically without constraining.

User work planes
User created work planes allow placement of sketches on non-planar faces. These work planes allow unlimited freedom in creating features that would otherwise be impossible. However, wherever possible, they should reference origin work geometry, to avoid losing dependencies when other features are modified or deleted. Remember that it is not necessary to create a workplane on a plane or face before selecting that face to create a new sketch.

Copy sketches and features
This is one of the most powerful as well as one of the least used and understood capabilities within Inventor. Within a single part file you have the ability to copy any sketch or feature, and paste it to another location within the part, or place it in a second open part, in effect creating a new feature on the destination part.

Copied sketches are independent of the original sketch. Copied features that are placed on the same part may be either independent of the original, or dimensionally dependent upon the original feature sketch.

Feature copies placed on a second part will always be independent, and not based upon the source part. As always, remember to fully anchor each copied feature after pasting to a new location.

When is a revision a new part?
While this final section in this article does not really apply to a good modeling workflow, it does bear repeating over and over again. Virtually every engineering department struggles with this issue at some point in time.

Altering an existing released part should trigger a revision. Any revision to a released part should not affect the replacement of that same named part on any design that the company has created in the past.

If the revised part will not fit or function on the original design where it was used, it must be given a new part name and number. At this point, the new part will be at revision level 1.

It is my hope that this article will inspire you to look at your design workflow with a critical eye toward design stability and productivity.

(Discuss this Article! in the HotNews Discussion Forums.)

Submitted by Dennis Jeffrey, an Autodesk Inventor Certified Expert and Autodesk Implementation Certified Expert. Dennis is the founder of Tekni Consulting LLC, a firm specializing in Autodesk Manufacturing Solutions implementation, training and consulting. Dennis has been using Autodesk Mechanical 3D Products since 1987. Dennis has been training and supporting manufacturing customers with Autodesk products since 1986. He is also the author of Creative Design With Mechanical Desktop™ and Creative Design With Autodesk Inventor, with a new co-authored book, "Mastering Autodesk Inventor 2009..." now available at Sybex.com. He returnined this year to Autodesk University 2008 as a seventh year Power Track instructor. Dennis is also a moderator for the AUGI manufacturing forums as well as an AUGI wishlist reviewer and columnist. Dennis has released a Live Web Training version of Creative Design With Inventor 2009. You can contact him at djeffrey@teknigroup.com and visit his website at http://teknigroup.com.