UNDERSTANDING 2D CONSTRAINTS IN AUTODESK INVENTOR® - PART 2

/**
*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 non-Autodesk 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 table-of-content 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:

1. Explain the constraints settings: Constraint Inference, Constraint Persistence, and Persistent Dimension.
2. Confidently apply dimensional constraints, or dimensions in a sketch.
3. Confidently apply geometric constraints in a sketch.
4. Use the Automatic Dimensions and Constraints tool, and
5. Show and Hide Sketch Constraints.

CONSTRAINT SETTINGS

1. 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!

2. 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.

3. 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

1. While you are in the sketch environment, Go to the Ribbon > Sketch tab > Constrain panel.
2. Click the section of the panel that bears the name "Constrain" with a downward-pointing arrow beside it.
3. 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 fully-constrained sketch is stable and cannot be easily disorganized. A fully-constrained 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 fully-constrained 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:

1. 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.
2. 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.
3. Go to the Draw panel and click the arrow beside Arc; launch the Arc (Center Point option) tool.
4. Draw two arcs, one on each side of the circle as shown below.
5. Draw a horizontal line above the arcs.
   
   
   
   Now, let's start constraining.
6. 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.
7. Repeat step 6 to constrain the top endpoint of the left arc with the left endpoint of the line.
8. Repeat step 6 and 7 for the right arc.
9. 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.
10. Click the left arc and click the line. A tangent constraint is applied between the left arc and the line.
11. Repeat step 9 and 10 for the right arc.
12. Click Finish on the Exit panel. Save the file.

To edit the sketch and use the Automatic Dimensions and Constraints tool, do the following:

1. On the Model Browser, double click Sketch1 to open the sketch for editing.
2. 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 right-hand side of the Graphics Area.
3. 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.
   
   
   
   
4. 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.
   
   
   
   
5. Now, let's modify the constraints. Delete the 7.009mm dimension. Select the dimension and hit Delete on your keyboard.
6. Launch the Equal Constraint tool. Sketch tab > Constrain panel >
7. Select the 7.219-mm arc and select the undimensioned arc. Both arcs now have the same radius of 7.219 mm.
8. 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.
9. While the Dimension tool is still active click on the 7.724-mm dimension. Now click the 8-mm dimension of the left arc. d14 is input into the Edit Dimension box. Press Enter. We've just created a reference dimension. The 8-mm 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.
10. Click the linear dimension 10.379mm. Change it to 10mm.
11. Click Finish Sketch on the Exit panel.
12. 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:

1. Right click on the Graphics Area. On the shortcut menu, click Show All Constraints.
2. Alternatively, hit F8 on your keyboard.

To hide all constraints in a sketch, do the following:

1. Right click on the Graphics Area. On the shortcut menu, click Hide All Constraints.
2. Alternatively, hit F9 on your keyboard.

To show specific constraints apply to a geometry, do the following:

1. Go to the Sketch tab > Constrain panel >
   
   
   
   
2. On the Graphics Area, select the geometry for which you wish to display constraints.
3. The constraints will be displayed.
4. 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:

1. 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:

1. 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.

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UNDERSTANDING 2D CONSTRAINTS IN AUTODESK INVENTOR® - PART 1

/**
*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 non-Autodesk 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 table-of-content page for more topics in this series.

TOPIC: UNDERSTANDING 2D CONSTRIANTS IN AUTODESK INVENTOR® - PART 1

INTRODUCTION

Some of the questions that are usually asked by new Inventor users who are migrating from AutoCAD are:

1. How to do I perform object snap in Inventor?
2. How to do I perform object snap tracking?
3. How to do I calculate rectangular and polar coordinates in Inventor? Etc.

Well, in the lesson, I'll try to answer these questions.

The first thing you have know about Inventor is that it is a 3D parametric design software. It is called a parametric modelling software because the sizes of the geometry and the relationship of between the geometry in your sketches, the height or extent of your extrude feature, the relationship between parts in an assembly, etc, are all controlled and driven by parameters.

In AutoCAD, the familiar and common workflow is to create precise geometry by using the commands on the Draw panel or toolbar. So if you want a horizontal line of say 200mm, you have to use polar tracking to set the direction of the line to either 0 or 180 degrees, and then type the precise length of 200. So you must always create precise geometry from the word "go." When dimensions (AutoCAD) are placed in the drawing, the dimensions merely report the size of the line. You cannot use the dimension to control the length of the line. In AutoCAD 3D, you use 3D modifying tools like 3D Move, 3D Rotate, and 3D Align to assembly various parts to form an assembly. AutoCAD does not associate or define any strict relationship between those parts as they are being assembled.

However, in Autodesk Inventor, the story changes. In Inventor sketch environment, you do not need to bother yourself by creating precise geometry from the start. That is why it is called "a sketch." You simply sketch approximate sizes and orientations of your geometry and then use Inventor 2D Constraints to define strict sizes and relationship between the sketch geometry. In the assembly environment, you use Inventor 3D constraints to define strict relationships between parts, or components in the assembly. This way, the sketch, model, or assembly is stable, and cannot be easily rearrange or scattered deliberately or inadvertently. The only to rearrange or edit the sketch, model, or assembly is to edit or redefine the constraints that were applied to the sketch geometry or part (or components). These constraints that help define these sizes and relationships are known as parameters.

It is worth noting that parametric design was introduced into AutoCAD from AutoCAD 2010. So, you can redefine constraints in AutoCAD just like you can do in Inventor. But I can tell you, you may use them easily unless you have worked with a parametric design application like Inventor.

In Autodesk Inventor, we have two types of constraints, namely:

1. 2D constraints, and
2. 3D constraints.

2D constraints are only available in the Sketch Environment. They are used to define the sizes of geometry and the relationship between them in the Sketch Environment - which is Autodesk Inventor 2D environment.

3D constraints are only available in the Assembly Environment. They are used to define the relationship between parts, or components in an assembly.

OBJECTIVES

At the end of this lesson, the reader should be able to:

1. Explain the concept of constraints in Autodesk Inventor
2. Differentiate between drawing in AutoCAD and sketching in Inventor.
3. Explain the types of 2D constraints.

USING 2D CONSTRAINTS IN THE SKETCH ENVIRONMENT

Before we continue, Let me say, for the records, that 2D constraints can perform what Object Snaps, Object Snap Tracking, and Polar Tracking does in AutoCAD and even more. By the time you begin sketching with 2D constraints in Autodesk Inventor, you will be amazed by their sheer power! So let's continue.

There are two types of 2D constraints in Autodesk Inventor, namely:

1. Dimensional constraints, and
2. Geometric constraints.

Dimensional constraints are simply parametric dimension. The dimensions drive or determine the sizes and orientations of geometry in the sketch. For example dimensional constraints (or simply dimensions) can set a line to be 200mm. Nothing can make that line become 200.0001 mm unless the parametric dimension is edited. You can also apply a dimension that makes the angle between two lines to be 60 degrees.

Geometric constraints defines the geometric relationship between geometry in the sketch. For example, an horizontal line, a circle centered at the endpoint of a line geometry, a line that is perpendicular to another line, or a circle that is tangent to another circle.

The goodies for working with 2D constraints in the Inventor Sketch Environment are located on the Sketch tab > Constrain panel. In this lesson, we are going to focus on Geometric Constraints only. Dimensional constraints will be treated in the second part of this lesson.



We have the following geometric constraints in Inventor: Coincident constraint, Collinear constraint, Concentric constraint, Fixed Constraint, Parallel constraint, Perpendicular constraint, Horizontal constraint, Vertical constraint, Tangent constraint, Smooth constraint, Symmetric constraint, and Equal constraint.

The dimensional constraint is simply the Dimension tool.

OVERVIEW OF THE GEOMETRIC CONSTRAINTS

1. COINCIDENT CONSTRAINT.
   
   Symbol:
   
   Access: Sketch tab > Constrain panel >
   
   The coincident constraint is use to constrain a point on a geometry to touch other geometry in your sketch. For example, you may want to constraint the endpoint of an horizontal line to meet the center of a circle. The coincident constraint glyph is shown at the point where the endpoint of the line coincides with the center of the circle.
   
   
   
   HOT TIP: To see the constraints that are currently applied to the geometry in your sketch, simply right click in your sketch and click Show All Constraints on the short-cut menu, or press F8 on your keyboard. The constraints are displayed as glyphs. When you hover your cursor over a glyph, the sketch geometry associated with that glyph are highlighted.
   
   
2. COLLINEAR CONSTRAINT.
   
   Symbol:
   
   Access: Sketch tab > Constrain panel >
   
   The collinear constraint constrains two or more line segments or ellipse axis to lie on the same line. In Figure 3, the top-most line is constrained to be collinear with the right-hand line of the closed geometry.
   
   
   
   
3. CONCENTRIC CONSTRAINT.
   
   Symbol:
   
   Access: Sketch tab > Constrain panel >
   
   The concentric constraint is used to define a concentric relationship between any two circles or arcs. Concentricity means that both circles or arcs have the same centerpoint. In Figure 4, the 2-diameter circle is constrained to be concentric with the 4-diameter circle.
   
   
   
   
4. FIXED CONSTRAINT.
   
   Symbol:
   
   Access: Sketch tab > Constrain panel >
   
   The fixed constraint is used to fixes points and curves in position relative to the sketch coordinate system. For example, when you apply fixed constraint to a circle, the circle can no longer be translated. That is, its position is fixed relative to the sketch coordinate system.
   
   
   
   
5. PARALLEL CONSTRAINT.
   
   Symbol:
   
   Access: Sketch tab > Constrain panel >
   
   The parallel constraint is used to define parallel relationships between line segments in your sketch. In Figure 6, parallel constraints are applied to opposite lines in the sketch in addition to a horizontal constraint applied to the top line.
   
   
   
   
6. PERPENDICULAR CONSTRAINT.
   
   Symbol:
   
   Access: Sketch tab > Constrain panel >
   
   The perpendicular constraint is used to define perpendicularity between two lines. In Figure 7, the inclined line is constrained to be perpendicular to the horizontal line.
   
   
   
   
7. HORIZONTAL CONSTRAINT.
   
   Symbol:
   
   Access: Sketch tab > Constrain panel >
   
   The horizontal constraint is used to constrain lines, ellipse axes, and pairs of points to lie parallel to the X axis of the sketch coordinate system. In Figure 8, horizontal constraint is applied to the left line. Horizontal constraint is also applied to constrain the left endpoint of the right line horizontally to the midpoint of the right-hand line of the rectangle.
   
   
   
   
8. VERTICAL CONSTRAINT.
   
   Symbol:
   
   Access: Sketch tab > Constrain panel >
   
   The vertical constraint is used to constrain lines, ellipse axes, and pairs of points to lie parallel to the Y axis of the sketch coordinate system. In Figure 9, a vertical constraint is applied to constrain the top vertex of the triangle to be vertical with the midpoint of the lower line of the triangle.
   
   
   
   
9. TANGENT CONSTRAINT.
   
   Symbol:
   
   Access: Sketch tab > Constrain panel >
   
   The tangent constraint is used to constrain lines, arcs, ellipses, ends of splines, and other geometry to be tangent to other geometry in the sketch. Figure 10 demonstrates the capability of the tangent constraint with the help of other constraints. It is quite interesting to see how the four disjointed geometry have been brought together parametrically through constraints.
   
   This is a how the geometry to the right of Figure 10 was achieved.
   
   1. Coincident constraint applied between arc 1 and circle, and also between arc 2 and circle.
   2. Tangent constraint applied between arc 1 and circle, and also between arc 2 and circle.
   3. Horizontal constraint applied between centerpoint of arc 1 and centerpoint of circle, and also applied between centerpoint of arc 2 and centerpoint of circle.
   4. Equal constraint applied between arc 1 and arc 2.
   5. Coincident constraint applied between the free endpoint of arc 1 and the left endpoint of the line.
   6. Tangent constraint applied between arc 1 and the line.
   7. Step v and vi repeated for arc 2 and the line.
   8. The line is dragged upwards above the circle.
   
   
   
   
   
10. SMOOTH CONSTRAINT.
    
    Symbol:
    
    Access: Sketch tab > Constrain panel >
    
    The smooth constraint is used to apply a G2 continuity condition between a spline and a line or arc. G2 continuity condition smoothens out the curvature of the spline as it joins the line. Smooth constraint is important during complex-shape design which can be done with Inventor or better with Autodesk Alias Design.
    
    
    
    
11. SYMMETRIC CONSTRAINT.
    
    Symbol:
    
    Access: Sketch tab > Constrain panel >
    
    The symmetric constraint is used to constrain curves to be symmetrical to other curves about a line of symmetry - which could be a line geometry or a work axis. Symmetric constraint is also established between curves when you use the Mirror tool. In Figure 12, symmetric constraint is applied between the two circle with the center horizontal line as the line of symmetric, also between the two arcs with the center vertical line as the axis of symmetry.
    
    
    
    
12. EQUAL CONSTRAINT.
    
    Symbol:
    
    Access: Sketch tab > Constrain panel >
    
    The equal constraint is used to constrain one geometry to be equal in size to another geometry in your sketch. Equal constraint is inferred when you use the symmetric constraint.
    
    
    
    

In the next lesson - Understanding Constraints in Autodesk Inventor - Part 2, we are going to do a little practical on what we have learnt in this lesson.

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