Paul Normand's Tips, Tricks, and cool links

Use control vertex splines in a guitar design

New 2013 spline functionality is used to create an acoustic guitar body.

Use equation curves to model complex geometry

2013 functionality that allows you to precisely model airfoils, cones, variable pitch threads and other complex geometry.

One of our developers provided the following examples for using Equation Curve functionality to create variable pitch helixes. Thanks Glenn!!

Create a new 3D Sketch. Start the Equation Curve command.

Here are equations that I use to create helical curves. Many other variations exist, but the following should give you some basic ideas.

Cartesian coordinates:

x(t) = radius* sin(360 * num_turns * t)

y(t) = radius* cos(360 * num_turns * t)

z(t) = height * t

      = num_turns * pitch* t

Cylindrical coordinates:

r(t) = radius

theta(t) = 360 * num_turns * t

z(t) = (same as Cartesian)

• To make the radiusvariable, replace radiuswith radius * t(or any radius function of t).
• To make the pitchvariable, replace pitchwith pitch * t(or any pitch function of t).

Examples:

• radius= 3or 3*t
• num_turns = 5
• height = 10
• pitch= 2or 2*t
• t ranges from 0 to 1.

1. Constant radius, constant pitch

Cartesian coordinates:

x(t) = 3*sin(360*5*t)

y(t) = 3*cos(360*5*t)

z(t) = 5*2*t

Cylindrical coordinates:

r(t) = 3

theta(t) = 360*5*t

z(t) = 5*2*t

2. constant radius, variable pitch

Cartesian coordinates:

x(t) = 3*sin(360*5*t)

y(t) = 3*cos(360*5*t)

z(t) = 5*2*t*t

Cylindrical coordinates:

r(t) = 3

theta(t) = 360*5*t

z(t) = 5*2*t*t

3. variable radius, constant pitch

Cartesian coordinates:

x(t) = 3*t*sin(360*5*t)

y(t) = 3*t*cos(360*5*t)

z(t) = 5*2*t

Cylindrical coordinates:

r(t) = 3*t

theta(t) = 360*5*t

z(t) = 5*2*t

4. variable radius, variable pitch

Cartesian coordinates:

x(t) = 3*t*sin(360*5*t)

y(t) = 3*t*cos(360*5*t)

z(t) = 5*2*t*t

Cylindrical coordinates:

r(t) = 3*t

theta(t) = 360*5*t

z(t) = 5*2*t*t

Note: In the Equation Curvecommand, you can use t^2 instead of t*t above.

When you sweep a profile along a helical path, use the plane normal sweep (instead of perpendicular sweep) to orient profiles suitable for coilor spring. 

In the example below, the sweep path is a constant radius, variable pitch helix. 

Use part file view reps

More 2013 functionality very useful when you are creating and documenting multi-body parts.

Enable the Browser Display

"How do I turn the Inventor browser display back on after someone turns it off?" is a common question on forums.

To restore the Browser to the display:

1. Click the View tab on the ribbon.
2. Click User Interface .
3. Click the drop-down menu and check the Browser entry.         

TIP: Use Clean Screen (Ctrl+0) to toggle the display of the browser, ribbon, document tabs, and status bar on and off.

iFeatures, iParts, and iAssemblies

Table driven features, parts, and assemblies are often a great solution to creating configurations. The link below is the handout I created for an Autodesk University class I taught last year.

/@api/deki/files/56612/=MA327-4P.docx

Freeform edits for Inventor

The form editing tools for Inventor 2011 have been moved to Fusion for the 2012 release. To use the freeform edit tools, click Edit Form or Edit Copy of Form in the Inventor Model tab, Fusion panel. These images show the transition from a prismatic block shape to an organic shape using the shape manipulation tools.

The following video shows editing a cylindrical extrusion with the Alias edge manipulation tool in the 2011 release. These tools were moved to Fusion for the 2012 release, but the edit steps are nearly identical.

Inventor Fusion and Moldflow Simulation Video

 Watch this video to see a sample workflow using Fusion and Moldflow.

View Representations

Once you discover view reps, you will want to know the answer to these 3 questions:

1. How do I keep new components from being added to existing assembly view reps?
2. How do I keep new components from being added to drawing views created from a view rep?
3. How do I get rid of this annoying message?

1. To prevent new components from showing up in a view rep, right click the view rep(s) in the browser and select Lock. If you have already inserted the parts, you will have to modify each view rep. It may be faster to delete, lock, and re-insert.
2. To prevent new components from appearing in a drawing view, lock the  view rep in the assembly as previously noted and check the associative box in the drawing view dialog box.
3. This message is displayed because the view rep default is set to Master (Locked). To reset the default, go to Application Options>File, scroll to the File Open area and click Options. In the File Open Options dialog box, select Last Active and then save your changes. The default for view reps is now unlocked. >Fil>- and andand and  and and

Watch the following video for an overview of View Reps.

Positional Representations

Watch the following video for an overview of Pos Reps.

Level of Detail Representations

Watch the following video for an overview of LOD Reps.

Animating Positional Representations

Have you been frustrated trying to simulate a mechanism using Drive Constraint to show movement? Did you know you can use Inventor Studio to create complex movement? The following video was created by driving multiple positional representations in an Inventor Studio animation.

Inventor Tooling Jig and Fixture

A very nice fixture design module is live on labs. Automated fastener placement, cloud assets and more - check it out!

Download the Inventor 2012 Jig and Fixture module from Autodesk labs here:

http://labs.autodesk.com/utilities/inventor_jigs_fixtures/

The two instructional videos posted on the labs site use the datasets included in this zip file.

/@api/deki/files/55288/=Jig%2526FixtureFiles.zip

Tooling part and mold fill analysis

The following animation shows the steps to create a part or mold fill analysis. You can display defects in the fill such as air traps and weld lines.

Spline and Surfacing Skill Builder

A new Skill Builder has been posted that uses the following functionality:

• Multi-body
• Splines
• Surfacing
• Plastic Features

Click here to access:

http://usa.autodesk.com/adsk/servlet...linkID=9242016

Mold Base Author Skill Builder

A three part video skill builder and downloadable dataset has been posted on the Community Tutorial page. This skill builder leads you through the process of creating a mold base that is Inventor Tooling friendly.

Check it out here: Tooling - Author and use a Mold Base