The Default Setting From Hell

Inventor Tutorial image showing the Parallel and perpendicular constraint optionIf you want to save yourself a huge amount of grief, there is a default setting in Autodesk Inventor that you should change immediately!

The setting in question is the Parallel and perpendicular constraint for Constraint placement priority. By default, Autodesk Inventor sets the constraint as mentioned above, to Parallel and perpendicular (as seen in the image to the right) as opposed to Horizontal and vertical –the other choice in the Application Options. This default setting can screw you up big time –but it all depends on what you design. We’ll get into that a bit more later, and I hope others will weigh in the comments  as to why they have the setting from hell enabled.

My first run-in with this setting happened while creating a three dimensional floor plan for a yacht I was working on (now called Ingot –back then it was Hull 503). Basically I was designing four stacked decks ranging in length from 150’ for the main deck to 30 feet or so for the fly bridge. It was a huge improvement over the previous designs created in AutoCAD in many ways, but a nightmare in others.

The two biggest problems were the default Parallel and perpendicular setting and Inventor sketches running out of steam (more about this in a later post, but basically once you get to a certain point in a sketch, the program will bog down and your sketch will become very buggy). You can easily solve the first one –the second requires a lot of experience to work around it. But before you just go ahead and change the setting, let me show you what can happen.

The problem boils down to design intent. When creating a layout for a plant floor or, as In my case, a yacht floor plan, when I draw a line vertically, I expect the line to stay vertical. Which is what you get when the constraint priority is set to Horizontal and vertical. Not so with the Parallel and perpendicular. This setting applies a Perpendicular Constraint to the last line drawn in the same orientation!


An image of a vertical constraint glyph being created in an Autodesk Inventor Tutorial




In the image to the left, a line was drawn from the projected Center Point upwards—– a Vertical Constraint was added automatically by clicking while the Vertical Constraint Glyph was visible.


I then drew six more lines, five to the right and one to the left –which can be seen in progress in the image below. Notice the inferred constraint glyph is to place a Parallel Constraint between the new line and the last line –which happens to be on the other side of the sketch…


This Inventor Tutorial image shows automatic parallel constraints being added.

I can change the inference simple enough by scrubbing a different line…


An tutorial image that shows Autodesk Invetor's scrubbing maneuver

…and then clicking to accept that constraint, but for the purpose of this demonstration, I just let the last line on the left be constrained to the one on the right…


The final results of the scrubbing tutorial.

We now have seven lines that are constrained vertically via a daisy chain constraint. Right click in the sketch and choose Show All degrees of Freedom from the Context Menu. The degrees of freedom shows that the original line will be fully constrained with one more constraint on its length. The rest are free to move about in any direction except rotational –because they are constrained vertically via the daisy chain back to the original line…
This part of the tutorial shows how to show all degrees of freedom in Autodesk Inventor

Right click again and choose Show All Constraints


Showing all constraints in Autodesk Inventor

Now hover your mouse over the individual constraints. If you hover over the Vertical Constraint on the first line, the line and the constraint will highlight. Now hover over one of the Parallel Constraints on one of the middle lines. Notice how the line that the constraint is on, the previous or next line, and both constraints are highlighted (lines turn red)…


Tutorial section for hover mouse to expose constraint relationships

You can follow the linked constraints from the first line to the last. Give it a shot. Now select the second line and hit the delete button. Every line downstream has now lost its link to the only line that has a Vertical Constraint


Autodesk Inventors default constraints suck

If you have a large layout with many hundreds of lines, you now have a lot of lines that can rotate freely until they are re-constrained vertically –if they are re-constrained vertically! Remember, this is what you will likely be seeing onscreen…
Autodesk Inventor Tutorial

If we were to constrain the endpoint of any of the non vertically constrained lines and drag its top endpoint sideways, it, and all of the  lines that are parallel constrained to it will go batshit crazy…

This part of the tutorial shows how bad things can go with unconstrained sketches in Autodesk Inventor

In the real world, finding all of the missing constraints and re-constraining them correctly would be a total pain. There is a very good chance something will be missed and will likely be found while running iLogic rules. If it happens too far down the line, such as while the model is running in a headless environment in an ERP system, the results could be pretty catastrophic.

In addition to the daisy chaining problems, you can waste a lot of time drawing lines that are making themselves parallel to lines that are not parallel to the origin to begin with. I’ve seen entire sketches that were just a tad skewed, which will cause huge problems down the line in models that have features that are created using the origin plane to get right angles.

So without further adieu, set the constraint placement priority to Horizontal and vertical


Application Icon > Options > Sketch (Tab) > Constraint placement priority > Horizontal and vertical


With this kick-ass setting, lines that should be horizontal or vertical are horizontal or vertical –and they will remain that way because they are constrained to the Origin Planes –not each other!

With this setting you can still draw a line at an angle where needed, then if you draw another line at a similar angle you will get a parallel glyph in that instance (which seems to be a far more correct way of doing things). You can also cancel all inferred constraint glyphs by pressing Ctrl while drawing the line if need be.

The only exceptions to this rule (that I ever use) would be kinetic modeling where there are moving (arcing or rotating) parts (beyond just resizing), and when creating sketch blocks. In fact, one of the things they stressed in the official Inventor training was to never daisy chain constraints —— yet the program is set to do so right out of the box!

If anyone has other instances of where Parallel and perpendicular priority would be advantageous –or why you agree they are the spawn of the devil, I would love to hear them. I have a few horror stories that I may share in the comments.

Inventor Tips & Tricks

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