How to Share a Sketch in Autodesk Inventor

PLATFORM: AUTODESK INVENTOR PROFESSIONAL 2012

LEVEL OF DIFFICULTY: BEGINNERS

AUTHOR: NDIANABASI UDONKANG

FOLLOW ME ON: Twitter | Facebook

This is a continuation of the series of lessons for new Inventor Users. Check out this blog's table-of-content page for more topics in this series.

TOPIC: HOW TO SHARE A SKETCH IN INVENTOR

INTRODUCTION

For sketched features to be created, Autodesk Inventor require visible sketches. And more often, a sketch could contain geometry and loops that can be reused across many features. After the first sketch feature is created, the sketch is consumed by that feature and must be shared if other features must have access to the sketch. Sharing of sketches in the simplest way of reusing sketches and saving lots of time.

OBJECTIVES

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

1. Create a simple sketch in Autodesk Inventor,
2. Constrain the sketch with dimensional and geometric constraints,
3. Create an Extrusion feature, and
4. Share an existing sketch.

SHARING A SKETCH IN AUTODESK INVENTOR

CREATING THE SKETCH GEOMETRY

Let's begin this section by drawing a simple sketch with Inventor. Do the following (refer to Figure 1 for the completed sketch):

1. Launch Inventor. When Inventor is open, click CTRL + N, to launch the New File dialog box.
2. Go to the Metric tab of the New File dialog box, and select Standard (mm).ipt template. Click OK to create a new part file.
3. Press C to start the Circle tool. Create a circle of diameter 20mm that is centered on the sketch.
4. Start another circle that is centered on the upper-left side of the first circle (Refer to Figure 2). Draw the circle towards the circumference of the first circle. A tangent constraint is inferred. Click the circumference of the first circle while the glyph is still showing.
5. Repeat step 4 and draw another circle centered at the upper-right side of the first circle. (Refer to Figure 3 for guidance.).
6. Press L to launch the Line tool. Create a horizontal line above the two top circles.
   
   
   
   
   
   

CONSTRAINING THE SKETCH

1. Now, on the Sketch tab > Constrain panel, launch the Coincident Constraint tool.
2. Click the left endpoint of the line and click the left circle.
3. Repeat step 8 for the right circle.
4. On the Sketch tab > Constrain panel, launch the Tangent Constraint tool.
5. Click the line and the left circle.
6. Repeat step 11 for the right circle.
7. On the Sketch tab > Constrain panel, launch the Equal Constraint tool.
8. Click the left and right circles.
9. Press D to launch the Dimension tool. Click the left circle. Apply a dimension of 25 mm.
10. Click the line and the centerpoint of the center circle. Click the 25-mm dimension that was applied to the left circle. Press Enter. A reference dimension is created.
11. The status bar should be displaying "fully constrained."
12. On the Sketch tab > Modify panel, launch the Trim tool. Click the inner segment of the center circle to trim it off. (Refer to Figure 1 for guidance).
13. Press S to exit the sketch environment. Save the file.

CREATING THE EXTRUSION FEATURE

1. At the upper-right corner of the Graphics Area, click the Home icon on the Viewcube.
   
   
   
2. Press E to launch the Extrude tool. The Extrude dialog box is displayed. The sketch has three closed profiles (or loops). So Inventor can not automatically select anyone for you. Select all the three profiles. Note that you can remove a profile by holding down CTRL and reselecting the profile.
3. On the Shape tab > Extents area, type 10mm as the height of extrusion.
4. Click OK to create the Extrusion1 feature (confirm the name from your Model Browser). Sketch1 is now consumed by Extrusion1.

SHARING SKETCH1

1. On the Model Browser, expand the Extrusion1 feature. Sketch1 is seen to be located under Extrusion1.
2. Right click Sketch1. On the shortcut menu, click Share Sketch. (See Figure 5)
3. Sketch1 is shared and is now added as a first-level object on the Model Browser. (See Figure 6).







4. Click the Home icon on the Viewcube. (See Figure 4).
5. On the Navigation bar, launch the Orbit tool. (See Figure 7)
   
   
   
   HOT TIP: You can also execute the Orbit tool by Holding down the Shift key and Press and drag the mouse wheel on a 3-button mouse.
   
   
6. Click and drag the center of the reticle ( See Figure 8) and reorient the model to appear as shown in Figure 9
   
   
   
   
   

CREATING ANOTHER EXTRUSION FEATURE

1. Press E to launch the Extrude tool. Sketch1 has been shared, so we reuse it for creating another sketched feature.
2. Click the central profile, and use 20 mm as the height of extrusion. Click the direction 2 button to flip the direction upwards if it's directed downwards.
   
   
   
3. Click OK to finish the Extrusion2 feature.
4. Right click Sketch1 on the Model Browser, and click Visibility to turn off the visibility of the sketch. Save the file.
5. The model is completed.
   
   
   

This method can be used for creating very complex parts from one sketch. But it's also a good workflow to create the sketches when needed.

I hope you learnt a lot from this lesson. If you have any questions, please drop a comment, and I will answer ASAP. Thank you.

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Creating a Cylinder at an Angle to a Hemisphere

PLATFORM: AUTODESK INVENTOR PROFESSIONAL 2012

LEVEL OF DIFFICULTY: BEGINNERS

AUTHOR: NDIANABASI UDONKANG

FOLLOW ME ON: Twitter | Facebook

This is a continuation of the series of lessons for new Inventor Users. Check out this blog's table-of-content page for more topics in this series.

TOPIC: CREATING A CYLINDER AT AN ANGLE TO A HEMISPHERE

INTRODUCTION

This article was written as a reply to a question asked by one of my blog readers. He wanted to know how to draw a cylinder at an angle to a hemisphere as shown below.

So this was the reply:

CREATING THE CIRCULAR BASE

1. Create a new part file. A new sketch should open by default.
2. In the Sketch environment, sketch a circle (say diameter 100mm). Use the center of the sketch as the center of the circle.
3. Immediately press E to initiate the Extrude tool. Extrude to a height (say 5mm).

CREATING THE HEMISPHERE

1. Press S to launch the Sketch tool immediately. Click the top face of the circular base as the sketch plane. Sketch a semicircle (say of diameter 80mm). You can use the Arc tool(Center Point option).
2. Join the endpoints of the semicircle with a line. Constrain the line to pass horizontally through the center of the sketch. If necessary, use the Trim tool to clean up the sketch.
3. Make the line a centerline geometry. You can do this by selecting the line and clicking on the Centerline tool on the Sketch Tab> Format Panel.
4. Press R to launch the Revolve tool immediately. Set the angle of revolution to 180 degrees. Click Ok.

CREATING THE INCLINED CYLINDER

Now I'm assuming that you followed my procedure. By constraining the circle that was used to create the circular base to the center of Sketch1, I ensured that the feature is entered in the graphics area. So I can reuse some of my default work planes and work axes without creating unnecessary new ones.

1. On the Model Browser, expand the Origin folder. Right click the XZ Plane and click Visibility to make the XZ plane visible.
2. Repeat step 1 above to make the X Axis visible.
3. Press ] to launch the Work Plane tool. Click the XZ Plane and the X Axis (they should be visible on the graphics area). You can also select them through the Model Browser. This technique is used to create a work plane at an angle to a plane about an axis.
4. Now set the angle of rotation to say 125 degrees. Click OK. A work plane is created (let's call it Work Plane 1).
   
   Now we are going to create an offset work plane parallel to Work Plane 1.
   
   
5. Press ] to launch the Work Plane tool. Click and drag Work Plane 1 upwards above the hemisphere. Set the distance to say 50mm(Check if the distance is +ve or -ve. Also ensure that the new work plane is slightly above the hemisphere to your desired distance). Click OK. A new work plane is created. (Let's call it Work Plane 2.)
6. Now press S to launch the Sketch tool. Select Work Plane 2 as the sketch plane to use.
7. Create a circle of say diameter 25mm at the center of the new sketch.
8. Press E to launch the Extrude tool. On the Extrude dialog box > Shape tab > Extents Area, set the Extents to "To Next". Click Ok. A cylinder is created from the Work Plane 2 to the hemisphere.
9. Save file.

I hope you learnt a lot from this lesson. If you have any questions, please drop a comment, and I will answer ASAP. Thank you.

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TYPES OF FEATURES IN AUTODESK INVENTOR

PLATFORM: AUTODESK INVENTOR PROFESSIONAL 2012

LEVEL OF DIFFICULTY: BEGINNERS

AUTHOR: NDIANABASI UDONKANG

FOLLOW ME ON: Twitter | Facebook

This is a continuation of the series of lessons for new Inventor Users. Check out this blog's table-of-content page for more topics in this series.

TOPIC: TYPES OF FEATURES IN AUTODESK INVENTOR

INTRODUCTION

Autodesk Inventor is a feature-based parametric modelling application. Inventor is said to be feature based because each modification that is made to a component is regarded as a feature. So in a design workflow for a component, you would most likely make use of extrusion, swept, lofted, revolved, threaded, hole, rib, fillet, shell, and chamfer features . If you are also experienced with surface modelling, you would likely use features like sculpt, thicken, patch, and trim. Learn more about Inventor in the Lesson: What is Inventor?

There are three types of features in Inventor, namely:

1. Sketched Features,
2. Placed Features, and
3. Work Features.

OBJECTIVES

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

1. Explain the following: sketched features, placed features, and work features.
2. Differentiate between sketched featues, placed features, and work features.

SKETCHED FEATURES

Sketched Features are those features that are built, or constructed from 2D or 3D sketches. A sketched feature is always the starting feature when you want begin a new part. The first sketched feature that is added to a part is called the "base feature." Sketched features can be used during standard part modelling, surface modelling, and plastic part modelling. The table below shows some examples of sketched features.

#	Type of Modelling	Examples of Sketched Features
1.	Standard part modelling	Extrusion, Revolution, Sweep, Loft, Emboss, Rib, and Coil.
2.	Surface modelling	Extrusionsrf, Revolutionsrf, Sweepsrf, and Loftsrf.
3.	Plastic part modelling	Grill, and Rest.

Sketched features always require visible sketches. Visible sketches are those sketches that can be seen on the Graphics Area. They should not be consumed by other features. If you have a sketch that is consumed by another feature, simply share the sketch to make it visible and available for use by other sketched features. Consumed sketches are those sketches that have been used to create sketched features. A consumed sketch is always located under the sketch feature in the model browser.

Sketched features can be located on the Create and Plastic Parts panel of the Model tab of a part environment.

PLACED FEATURES

Placed features are those features that do not strictly require sketches for their creation. They are mostly used for modifying (or adding features) to an existing the model - the reason they are called "Modifying Tools." Examples of placed features are Hole, Fillet, Chamfer, Shell, Draft, Thread, Split, and Combine features for modifying standard part models, and Thicken/Offset, Stitch, Sculpt, Patch, and Trim for modifying surface models.

Placed features are located on the Modify and Surface panels of the Model tab of a part environment.

WORK FEATURES

Work features are modeling aids. From the first sketch to the last feature of your model, work features are used to aid the modeling process. And as the design becomes more complex, you will need the help of work features to find your way out! These work features can be used for creating sketches, for constraining of components in the assembly environment, for feature termination (in both part and assembly designs), and for creating other work features.

There are three types of work features in Autodesk Inventor, namely:

1. Work planes;
2. Work axes; and
3. Work points.

There are about four lessons dedicated to work features. Please check them out below:

Using and Understanding Work Planes in Autodesk Inventor

Using and Understanding Work Axes in Autodesk Inventor

Using and Understanding Work Points in Autodesk Inventor

Using and Understanding Grounded Work Point in Autodesk Inventor

 

I hope you learnt a lot from this lesson. If you have any questions, please drop a comment, and I will answer ASAP. Thank you.

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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.

Jump to the Top | Index

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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