/**
*PROLOGUE
* I'm beginning a series of lesson tailored for my friends out there who are learning Autodesk Inventor from the scratch. The lessons are going to be arranged in sequence so that the reader can grow in confidence with each lesson.
*I'm assuming that the reader is new to the world of "digital prototyping" or is migrating from a nonAutodesk product. Whatever might be the case, I'm wishing you a happy learning experience.
*I would also encourage the readers to post comments about the articles. Comment about my methodology, content, useful, in fact anything on your mind. You are also free to suggest to me topics to write about. Thank you.
*/
PLATFORM: AUTODESK INVENTOR PROFESSIONAL 2012
LEVEL OF DIFFICULTY: BEGINNERS
AUTHOR: NDIANABASI UDONKANG
FOLLOW ME ON: Twitter  Facebook
Check out this blog's tableofcontent page for more topics in this series.
TOPIC: UNDERSTANDING 2D CONSTRIANTS IN AUTODESK INVENTOR®  PART 2
This is the second part of the lesson on Understanding 2D Constraints in Autodesk Inventor. You may be interested in the Part 1.
OBJECTIVES
At the end of this lesson the reader should be able to:
 Explain the constraints settings: Constraint Inference, Constraint Persistence, and Persistent Dimension.
 Confidently apply dimensional constraints, or dimensions in a sketch.
 Confidently apply geometric constraints in a sketch.
 Use the Automatic Dimensions and Constraints tool, and
 Show and Hide Sketch Constraints.
CONSTRAINT SETTINGS

CONSTRAINT INFERENCE
During sketch creation, Autodesk Inventor helps you infer or suggest constraints that will be created based on the orientation of your geometry or its position with respect to other geometry. For example, while sketching with the Line tool, if you sketch the line vertically, Autodesk Inventor will display a vertical glyph near the line telling you the constraint that is most likely to be created if you create the line segment. If you approach another line in the sketch perpendicularly, Inventor infers a perpendicular constraint. If you are creating a circle and the circumference is taken close to a line geometry, Inventor will infer a tangent constrain.
If Constraint Inference is turned off, Inventor will not infer constraints during sketch creating, thereby, leaving with an enormous task to carefully applying the necessary constraints after sketch creation. This is not a good workflow. Inferred constraints may or may not be actually applied to the geometry after the sketch operation. This depends on another setting known as Constraint Persistence. HOT TIP: You can temporarily disable constraint inference by holding down the CTRL key during sketch creation. Try it out! 
CONSTRAINT PERSISTENCE
Constraint Persistence is a setting that simply ensures that the constraints inferred while you are creating a geometry is actually applied after the geometry have been created. For example, if a vertical constraint is inferred while you are sketching a vertical line, constraint persistence ensures that the Vertical Constraint is actually applied to the geometry after it has been created. If Constraint Persistence is turned off, the constraints are merely inferred but not applied.
Also note that Constraint Persistence has nothing to do if Constraint Inference has been turned off, so it is automatically disabled if Constraint Inference is turned off.

PERSISTENT DIMENSION
Persistent Dimension setting allows you to easily define dimensional constraints, or dimensions for your sketch geometry during sketch creation. For example, while creating a circle, after specifying the centerpoint, you can quickly type in the dimension of the circle, say 20mm. This dimension is applied or persists after the circle has been created. So you do not need to apply a dimension to the circle afterwards.
LOCATING THE CONSTRAINT SETTINGS ON THE RIBBON
 While you are in the sketch environment, Go to the Ribbon > Sketch tab > Constrain panel.
 Click the section of the panel that bears the name "Constrain" with a downwardpointing arrow beside it.
 This expands the Constrain panel revealing the constraint settings.
AUTOMATIC DIMENSIONS AND CONSTRAINTS
Sketches in Inventor must be made as stable as possible throught the use of geometric and dimensional constraints. Most times, dimensions and geometric constraints are applied to the sketch geometry until the status bar showed the message "fully constrained" (just in front of the Capacity Meter). A fullyconstrained sketch is stable and cannot be easily disorganized. A fullyconstrained sketch also gives rise to a stable "sketched feature." Sketched Features are those features that are created from sketches through tools like Extrude, Revolve, Loft, Sweep, Emboss, Rib, etc. The other category of features is the "Placed Features." Placed Features are those features that do not "strictly" require a sketch for their creation e.g. Thread, Hole, Fillet, Chamfer, Shell etc.
There are times when you have carefully applied dimensions and geometric constraints to your sketch, but the Status Bar still shows you, for instance, "3 dimensions needed." This message means that you still have 3 constraints to applied, either dimensional or geometrical. Then, the Automatic Dimensions and Constraints tool comes handy. The Automatic Dimensions and Constraints tools allows the application to automatically apply missing constraints. Experienced designers use the tool as a hinting tool (just the way you use the Hint tool in computer card games). More often, you will find out that some of the constraints suggested by the Automatic Dimensions and Constraints tool are unnecessary.
Inventor displayed fullyconstrained geometry on your sketches with a color ( often blue) that is different from those that are not fully constrained. So once all the geometry in your sketch are displayed with this color, the message on the Status Bar could be ignored. However, to be on the safe side, use the Automatic Dimensions and Constraints tool to confirm.
The Automatic Dimensions and Constraints Tool can be found on the Sketch tab > Constrain panel as shown in Figure 2.
USING THE AUTOMATIC DIMENSIONS AND CONSTRAINTS TOOL
Let's start this section by creating a simple sketch. This sketch will help us learn how to use some of the geometric constraint we learnt in Part 1 of this lesson.
The sketch should look like this (Figure 3) after creation.
To create the sketch do the following:
 With Inventor opened, Press CTRL + N to launch the New File dialog box. Go the Metric tab and select the template Standard (mm).ipt. A new part file is created and a sketch labelled Sketch1 on the Model Browser is created and opened for editing.
 Press C to launch the Circle tool. Click the center of the sketch as the centerpoint of the circle and draw a circle of approximately 8 mm. If you are using Inventor 2011 and above, do not type in 8mm right now. This is will apply a dimensional constraint of 8mm.
 Go to the Draw panel and click the arrow beside Arc; launch the Arc (Center Point option) tool.
 Draw two arcs, one on each side of the circle as shown below.
 Draw a horizontal line above the arcs.
Now, let's start constraining. On the Constrain panel, launch the Coincident Constraint tool. Click the bottom endpoint of the left arc and then click the the circle. This makes the end of the arc to coincide with the circle.
 Repeat step 6 to constrain the top endpoint of the left arc with the left endpoint of the line.
 Repeat step 6 and 7 for the right arc.
 On the Constrain panel, launch the Tangent Constraint tool. Click the left arc and click the circle. A tangent constraint is applied between the left arc and the circle.
 Click the left arc and click the line. A tangent constraint is applied between the left arc and the line.
 Repeat step 9 and 10 for the right arc.
 Click Finish on the Exit panel. Save the file.
To edit the sketch and use the Automatic Dimensions and Constraints tool, do the following:
 On the Model Browser, double click Sketch1 to open the sketch for editing.
 If the sketch is not oriented normal to your screen, click the View Face tool on the Navigation Bar and click Sketch1 on the Model Browser. Sketch1 should be normal to the screeen now. Note: The Navigation Bar is found at the righthand side of the Graphics Area.
 Launch the Automatic Dimensions and Constraints Tool (see Figure 2). The Auto Dimension dialog box is launched. Inventor displays that there are 4 missing constraints.
 In the Auto Dimension dialog box, you can specify whether to automatically apply dimensions, geometric constraints or both. Click Apply. Four constraints are applied and Inventor now displays that the sketch is fully constrained. Click Done to close the dialog box.
NOTE: You can always remove the constraints that were automatically added by relaunching the Auto dimension dialog box and clicking Remove.
 Now, let's modify the constraints. Delete the 7.009mm dimension. Select the dimension and hit Delete on your keyboard.
 Launch the Equal Constraint tool. Sketch tab > Constrain panel >
 Select the 7.219mm arc and select the undimensioned arc. Both arcs now have the same radius of 7.219 mm.
 Launch the Dimension tool by hitting "D" on your keyboard. Click the 7.219 mm dimension. Change it to 8 mm. The other arc also updates.
 While the Dimension tool is still active click on the 7.724mm dimension. Now click the 8mm dimension of the left arc. d14 is input into the Edit Dimension box. Press Enter. We've just created a reference dimension. The 8mm dimension of the bottom arc references the dimension of the left arc, making them equal. So dimension of the left arc is changed, that of the bottom arc also changes.
 Click the linear dimension 10.379mm. Change it to 10mm.
 Click Finish Sketch on the Exit panel.
 Save the File
.
SHOWING AND HIDING CONSTRAINTS IN A SKETCH
You can show display constraints globally or specifically in your sketch. The global method displays all the constraints applied in your sketch. You can also choose to display only some specific constraints.
To show all constraints in a sketch, do the following:
 Right click on the Graphics Area. On the shortcut menu, click Show All Constraints.
 Alternatively, hit F8 on your keyboard.
To hide all constraints in a sketch, do the following:
 Right click on the Graphics Area. On the shortcut menu, click Hide All Constraints.
 Alternatively, hit F9 on your keyboard.
To show specific constraints apply to a geometry, do the following:
 Go to the Sketch tab > Constrain panel >
 On the Graphics Area, select the geometry for which you wish to display constraints.
 The constraints will be displayed.
 Press F9 to hide the constraints.
CONSTRAINT VISIBILITY AND CONSTRAINT OPTIONS DIALOG BOXES
Inventor provides a way of disabling the display of some constraints and what constraint is inferred if Constraint Inference is active.
CONSTRAINT VISIBILITY DIALOG BOX
The Constraint Visibility dialog box allows you to select which constraints you want to display when you launch "Show All Constraints."
To launch the Constraint Visibility dialog box, do the following:
 Right click on the Graphics Area, click Constraint Visibility... to launch the dialog box.
CONSTRAINT OPTIONS DIALOG BOX
The Constraint Options dialog box allows you to choose which geometric constraints will be inferred during sketch creation when Constraint Inference is active. You can also select the scope of the Inference, i.e. choose which geometry you want Constraint Inference to infer constraints for.
To launch the Constraint Options dialog box, do the following:
 Right click on the Graphics Area. Click on Constraint Options... to launch the dialog box
I hope you learnt a lot from this lesson. If you have any questions, please drop a comment, and I answer ASAP. Thank you.
Very helpful. Just started learning Inventor.
ReplyDelete