Video: Understanding constraintsIn this movie we want to focus on Sketch Constraints. As we move closer to sketching, it's important to understand what constraints are and how they help build intelligence into your sketches, and in turn, your parts and assemblies. It's important because Inventor will automatically apply constraints during the sketching process. And if you don't know what constraints are, you could easily become confused or frustrated. A constraint by definition is something that confines or restricts within prescribed bounds. What that means is constraints are essentially rules that tell sketch geometry how it can and can't move, how big it can be, or how it is to react in relation to other sketch geometry.
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This course introduces you to the interface and key processes of Inventor, the parametric design system from Autodesk. Author John Helfen covers sketching, part modeling, assemblies, and drawings. These tasks work in conjunction, allowing you to create parts and assemblies and document them in a way so that the manufacturing process proceeds faster and more efficiently.
- Navigating drawings with the View Cube and other navigation tools
- Sketching geometry
- Dimensioning parts
- Creating parameters
- Drawing circles, squares, and other shapes
- Creating extrusions
- Creating and managing constraints in assemblies
- Setting basic drawing dimensions
In this movie we want to focus on Sketch Constraints. As we move closer to sketching, it's important to understand what constraints are and how they help build intelligence into your sketches, and in turn, your parts and assemblies. It's important because Inventor will automatically apply constraints during the sketching process. And if you don't know what constraints are, you could easily become confused or frustrated. A constraint by definition is something that confines or restricts within prescribed bounds. What that means is constraints are essentially rules that tell sketch geometry how it can and can't move, how big it can be, or how it is to react in relation to other sketch geometry.
In Inventor sketch constraints come in two flavors, Dimensional and Geometric. Dimensional constraints are just that, dimensions that tell a piece of geometry exactly how big it needs to be, and we'll cover dimensions in a later movie. In this movie we'll focus on Geometric constraints. I've created a simple practice file that will help you quickly understand how geometric constraints are used to control sketch geometry. To begin we need to edit the sketch. You can do that in a few different ways, and I'm going to walk you through each of those, because depending on the scenario you may need to use one or the other--you'll learn that over time--but at least I want to make sure you understand each of those options.
The first option and the one I use the most, is selecting sketch geometry on the graphic screen and using the Heads-up display to edit the sketch. That will rotate you into a normal view to the sketch, and you can begin the editing process. I'm going to finish this sketch and show you a couple of other ways to do it. Another way would be finding that sketch in the browser, right-clicking on it, and selecting Edit Sketch from the right-click menu. That also rotates you into a normal view and prepares you for editing the sketch.
The final way, which is also a very common way, is to double-click the Sketch icon in the browser. By doing that you activate the sketch environment, and you're ready to edit the sketch again. Normally I would not say that you have to look at sketch constraints when you begin editing a sketch, in most cases you're going to be the one creating the sketch, in that case you already know what constraints have been applied. In the case where you're getting a file from somebody else or an exercise file for this course, it's important that you look at what constraints have already been applied so that you don't try to duplicate that after.
To view the constraints that have been applied, make sure nothing is selected in the graphics window by hitting Escape on your keyboard. This will make sure nothing is selected, that way when you right-click you have a specific context menu that allows you to show all constraints. Now when I do that a bunch of stuff happens. Well, in this case it really is just showing me the constraints that are here, which is what it's supposed to do. But in this case at this point we've only applied fixed constraints, and these are constraints I applied in order to make this file work the way it's supposed to.
So, because we're not very interested in those lock constraints we're going to temporarily hide those. I'm going to right-click in the Graphics window and select Constraint Visibility. This will bring up the list of all the constraints and allow you to temporarily disable some of the viewing of those items. Now it's important to remember, after you apply this, that you've turned it off. When you're done, if you think you're going to need that moving forward, turn it back on. I've seen many cases where people said that their constraints aren't working come to find out that they have really just turn off the visibility. So it's important that you remember that Constraint Visibility is available from the right-click menu in the Sketch environment.
The next item I wanted to show, which is very helpful to those who new to Inventor, is the option for Show All Degrees of Freedom. This shows you what degrees of freedom are available to any piece of sketch geometry based on the constraints that have been applied already. In this case, no constraints have been applied. We've hidden the fixed constraint, but the geometry that's been created doesn't have any constraints at this point. We're going to begin by adding a horizontal constraint to the first item here. We're going to go to the Sketch tab, under the Constrain panel, and select the Horizontal constraint.
Now when you hover over an item in the Ribbon bar you will get an option that shows you tool tips. These tool tips are little more advance than what you might get in a typical application. When I hover over and pause for a moment I get an initial description of that item, and if I pause a little bit longer I get a full description and in some cases even video of how to apply these items. Once you've launched the command you can simply click on a piece of geometry to apply that constraint.
You'll notice that the sketch geometry is now horizontal, and it's also changed color. The color is important here, because it's providing information. It's telling you that this item is fully constrained from a geometric standpoint. The arrows that remain are actually telling you that a dimension is required to provide an overall size. I am going to get out of this command by right-clicking and selecting Cancel. You could also do this by hitting Escape on your keyboard, and I'm going to right-click again to add a Dimension. Now we're not going to get into the details of dimension, but I'm going to apply one simply to show you what happens when it's fully constrained.
In this case, all of the degrees of freedom are removed, and if I returned to my right-click menu and get out of my Dimension command, I can then right-click again and select Show All Constraints one more time, and you can see that the horizontal constraint has been applied. By hovering over that icon you can also see the geometry highlight which tells you what pieces of geometry are included with this constraint. To continue, I'm going to go ahead and hide all my degrees of freedom, and I'm going to Hide all my constraints. This will help just clean up the interface.
We can move forward, and we'll circle back and look at the constraints once we've applied to each of them. As we continue forward the next constraint is a Vertical constraint. Again, we're not going to touch all the constraints, but the key constraints that are most used in design are going to be covered. I am going to select the Vertical constraint from the Constrain panel and then select the line to apply the vertical constraint. You'll notice again the color changes and at this point I'm ready to move to my next constraint. I could hit Escape to get out of this command, but that's not required.
Next I can actually move to the Collinear constraint which is here on the top of the Constrain toolbar, and that will automatically cancel the Vertical constraint and begin the next command. In this command rather than selecting a single line, you need to pick two pieces of geometry. One item to start with and a second item that you want to make collinear. This will put the two pieces of geometry in line with each other. The next constraint is a Concentric constraint. By selecting each of the circles you have the ability to lock the center points so that they will always remain connected. The next constraint is the Tangent constraint.
By selecting the circle and then the line you'll add a rule that make sure that line will always remain tangent to that circle. And the final constraint is the Perpendicular constraint. If we want these two lines to be perfectly perpendicular--or 90 degrees from each other-- I simply select each of these lines while in the Perpendicular constraint command, and you can see that those two items are now locked at a 90 degree angle. I am going to hit Escape on my keyboard to get out of the Constrain command, and we will right-click in the Graphics window and select Show All Constraints again, and now you can see the constraints that we've applied to these pieces of geometry.
Again, hovering over any of these items will allow you to see which pieces of geometry are included in the constraint. In this case, in the tangent you see both the circle and the line highlight, in the collinear constraint both lines highlight. Now the reason that's important is perhaps I added this collinear constraint by mistake, or it's no longer needed, it's very simple to remove constraints as well. When I hover over either of these items, it shows me the geometry that's contained in this constraint. I can left-click to select the constraint-- indicated by the highlighting in red--and then I can right-click and select Delete from the Marking menu.
You'll notice that the colors change to represent that this item is no longer fully constrained, and I could apply some other constraint if I chose to. Hopefully at this point you have a solid understanding of what constraints are and how they work to control geometry in a sketch. We'll cover constraints a little bit more in each of the following sketch movies, but it's important that you have a solid understanding from this point.
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