Based only on this file as evidence I would recommend that you get more training. You may very well have 999 other files that better demonstrate your techniques.

I can't imagine how someone can use the software since R4 designing thousands of parts can start out on a part of this complexity and not even bother to constrain the first sketch. (Some of the arcs in Sketch1 aren't even tangent - Inventor does this for you, no extra work.) Especially considering the mirrored symmetry from left to right.

I offer many industry classes on using Inventor. Where are you located? I could suggest this book as well http://www.amazon.com/gp/p roduct/0470293144?ie=UTF8&tag=mc02c-20&linkCode=as2&camp=1789&creative=9325&crea tiveASIN=0470293144 there are many tips in there about creating robust parts. Seems to me I recall Sean having something to say about constrained sketches. You might also read this document http://home.pc t.edu/~jmather/AU2007/MA105-1L%20Mather.pdf

There is nothing inherently wrong with using adaptive parts, but building a house of cards on top of quicksand is probably not the best way to ensure a robust part. It might sound like the comments here are "kicking sand" but more like an attempt to lend a helping hand out of the quicksand.

I'm quite sure I could sit down with you and demonstrate how less than disciplined modeling techniques are costing your company thousands of dollars. You should be able to easily recoup my fee on the first project.

So Autodesk is demonstrating a, "lack of foresight to produce something that can work no matter how poorly... ...laid out", but you seem to be rejecting the same principle in your work.

GIGO is always relevant. Your part is garbage. Nice looking garbage, but all the same garbage. Yes you should have been given a warning much sooner. (Sketch16 has sick geometry.) Maybe we will see something like SolidWorks has in a future Inventor. In SolidWorks there is a switch that can be set to not allow features to be created from unconstrained sketches. Of course for the most part very few unconstrained sketches should make it out of a first parametric modeling class.

When professional people ignore GIGO we have bridges collapse into rivers, cranes collapse onto apartment buildings and school buildings collapse onto children. Your designs might not have such concern for GIGO, but it is no less relevant.

I agree that I learn much about the program from unconventional techniques and I would encourage you to submit problems such as this one. But at the same time I would listen to the comments. An open forum like this brings together many different experiences that enlighten us all. Sometimes it is a little messy and argumentative but in the end there should be something of value within the arguments.

In my experience all the evidence I have seen is that constraining most sketches and using a disciplined modeling technique saves time.

I took a look at the file. As indicated earlier in the thread no other changes other than adding the fillet after Extrusion15 the part would rebuild without errors. I don't believe I ever indicated that there was a cause and effect between the unconstrained sketches and the fillet. I believe I did indicate that this was an interesting file because a fillet feature caused errors earlier in the history tree.

I frequently take interesting problems from this discussion group and analyze them see if I can reproduce the geometry in a more efficient manner - particularly those problems that might reveal a re-producible bug or feature missing from Inventor. I identify with the book iWoz by Steve Wozniak on how I enjoy these challenges.

It was pointed out recently that while I might post a more elegant, robust solution I never take the time to explain why it is more robust or elegant. It would probably take a book to go much beneath the surface, and I am basically a machinist, ill equipped for the task. The first thing a machinist does when making a part is identify data for reference.

I checked iProperties and it indicated the file was started in Inventor 2008 and last saved in Inventor 2009.

I opened your file and created a new user Workplane Inventor assigned Workplane23.

On the workplane I created a new sketch Inventor assigned Sketch107.

In the new sketch I created a rectangle and added a dimension, Inventor assigned d872.

I Project Geometry a Loop, Inventor assigned Project Loop60.

I Project Geometry a Cut Edges, Inventor assigned Cut Edges28.

I extruded the sketch and Inventor assigned Extrusion87.



When I go through a problem I try many many iterations in quick succession getting to understand the geometry. I start many new files rather than building on top of the earlier garbage that I have accumulated and then discarded. A couple of interesting reads along this line are Seymour Papert's Mindstorms: Children, Computers, and Powerful Ideas, and The Children's Machine: Rethinking School in the Age of the Computer. To paraphrase Papert, "I need the unsuccessful early trials to get a feel for the later successful solution."

Workplane23

In your file there remains 9 user workplanes. Three of these are duplicates of the origin workplanes.

The only time I duplicate the origin workplanes is if I need to Flip Normal or if the design indicates that I might want to offset later for some reason. In other words, very very rarely. I feel like I might be mis-interpreted here, I didn't say I don't create user workplanes, I said I don't duplicate workplanes that already exist.

Sketch107

In your file there remains 42 sketches and 3 suppressed sketches. Many to most are under constrained, often lacking auto constraints or any dimensions at all. It would actually take me more time rather than less time to do the unconstrained/undimensioned sketches. To me this is the "quicksand" that can lead to even inadvertent changes to the model even if you were very careful in the initial construction. Even if you will have absolutely no need to change later. Within those sketches is evidence that is of more concern to me than the dimensioning/constraining - after all we didn't have constraints or driving dimensions on the drawing board or even AutoCAD.

Project Loop60

I failed to record how many projected loops you have remaining, but I almost never ever use projected loops. They are particularly prone to failure if the underlying geometry changes too much. Do an experiment. Project a loop on a face and then sketch a circle. Extrude the circle. Now try to Copy the cylindrical extruded feature. You cannot copy a feature that contains projected loop. (Projected Loop is generated when the Project Geometry is used on a part face rather than on the edges.) It gets even more fragile if build a child feature whose parent has a projected loop. Only use projected loop on top level features that will never change and no use as iFeature or Copy in the future.

Cut Edges28

I failed to record how many projected cut edge sketches you have remaining. Similar to projected loops, projected edges are prone to failure if the underlying geometry changes too much. But unlike projected loops which can be entirely avoided in any case that I can think of off-hand, projected cut edges are sometimes very valuable. They should be used only where absolutely needed and with caution. Until recently they weren't eve associative in Inventor. (I feel the need to point out to the less experienced Inventor user that Cut Edges28 does not mean there are 27 previous entities created - each instance of a project cut edge usually (always) results in multiple entities created - each of which could fail).