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Tag Archives: Inventor

Autodesk Inventor Sheet Metal Contour Rolls

This is a continuation of my series “Holy Sheet Metal Batman“, taking a deep dive into Autodesk Inventor’s Sheet Metal Environment. Let’s look at probably the least utilized feature, Contour Rolls. Why is it not utilized? Just because it is not needed by most users as it creates shapes not always doable with standard press brakes.

Contour Rolls are used to create rolled sheetmetal feature. Like the Contour Flange, it creates complex models with a very simple process. Think of Contour Flange as extrusions and Contour Rolls are revolutions.

The Contour Roll starts with a sketch. The sketch can only contain lines and arcs and must be an open profile. Depending on the unroll method (see below) the sketch may need a center line. Like all Inventor Sheet Metal features, Inventor will automatically create bends at line intersections.

Inventor SM - Contour Roll Sketch

After initiating the feature, it should automatically locate the profile and the center line (if a center line exists). Using the Shape options you can select the profile / centerline or make adjustments if the wrong objects are selected. The direction options set the direction for the thickness offset: Inside, Outside or Midplane.

Inventor SM - Contour Roll Initial

The Rolled Angle Section defines the rolling angle and the direction. The Rolled Angle defines the amount of rotation (Revolution).
Inventor SM - Contour Roll Rolled Angle

Set the Unroll Method by picking one of the four options: Centroid Cylinder, Custom Cylinder, Developed Length, and Neutral Radius. This specifies how the feature should be unrolled when the flat pattern is generated. All four produce similar results but differ in the input required. All methods derive the Developed Length by multiplying the Rolled Angle by the Neutral Radius.

  1. Centroid Cylinder uses a parallel axis to the revolute axis which passes through the evaluated Centroid location. This is the default method.
  2. Custom Cylinder requires a sketched line representing the surface of the cylindrical neutral surface
  3. With Developed Length specify the amount that “drives” the developed length of the flattened rolled segment
  4. The Neutral Radius option parametrically determines a value for the neutral radius

Inventor SM - Contour Roll Unroll Options


As with all Sheet Metal features additional features can be applied to form the final results. In this example, I project the end face into a new sketch and use Contour Flange to add length

Inventor SM - Contour Roll Base Model

Inventor SM - Contour Roll Base with Flange

See the feature in action!

Feature Image “Contour 3” by Bodie Strain

Inventor Sheetmetal Corner Seams

The Corner Seam feature within the Inventor Sheet Metal environment really has lost a lot of its luster with how Flanges auto-miter corners. And lets also not forget that you can override the corner conditions for each flange intersection. The Corner Seam feature is still there, just waiting for the opportunity to show you what it can do. With Corner Seams you create  seams (gaps) between faces that intersect or are coplanar.

Inventor SM - Corner Seams

After starting the feature the first step is to pick two edges from existing flanges, hems, or faces. Once selected a preview is generated, which helps in picking the right options. The Seam (aka the gap between edges) is configured as Maximum Gap Distance or Face / Edge Distance. Both options have there own specific options.

  • With Maximum Gap distance the seam gap is created so that it could be measured with an inspection gauge or calipers. The biggest “bang for the buck” with this option is with non-square corners.
  • Face / Edge distance is exclusive to the Corner Seam feature and is not used by the Flange Auto mitre feature. With Face / Edge Apply the seam gap sized is based on measurements from the flange.

With the Seam measurement type selected next specify the type of seam… Symmetric / No Overlap, Overlap, or Reverse Overlap. Use the Gap textbox to set the desired gap size. Corner Seam works with Hems too

Inventor SM - Corner Seam with Hems

The second method of using Corner Seam is for creating rips in connected corners, typically when converting a 3D model into a Sheet Metal component. By selecting the Rip option you then select the intersecting corner edge and Inventor creates a seam to rip the faces apart

Inventor SM - Corner Seam Rip

Feature Image PROJlhopgood Sackboy’s Corner

Lofty Goals with Inventor Sheet Metal (on Mechanical Advantage)

The Inventor Sheet Metal Environment provides many tools and features. It is really a robust environment for building and working with sheet metal models. With all that is in there, the most impressive is probably the Lofted Flange featureWhy? A few reasons… but you’re going to have to read it somewhere else! 

I am very fortunate to guest blog for Kevin Ellingson on Kevin is not new to the industry, just his company is, and many of you might already follow him on twitter @kellings. You can now also follow Mechanical Advantage on Twitter @mechvantage

Here is my post on mechanical advantage

Mechanical Advantage


Kevin Ellingson is a technical specialist at Mechanical Advantage based out of Minnesota, North Dakota, and South Dakota. He has been using Autodesk products for over 15 years with a background in fabricated metal components, sheet metal, and CNC programming. Mechanical Advantage provides high-quality passionate training and services for the Autodesk family of mechanical design products specializing in AutoCAD, Inventor, and Autodesk CAM.

Featured Image Lofty by Jonny Hughes

Inventor Sheet Metal: All Together for the Greater Good

Every superhero team has those members who are just not as strong as the rest, some might even make you question why they are even part of the team. For every Captain America there is the Wasp, for every Superman there are the Wonder Twins, for every Superboy there is Bouncing Boy, and for every Wolverine there is the Toad. However, no matter how weak or how out of place these members might seem, they always find a way to help fight evil and save the day.


Dragon*Con 2013: JLA vs Avengers Shoot

Within the Inventor Sheet Metal environment, these members are Corner Rounds, Corner Chamfers, and Cuts. On their own they don’t have the same “wow” factor as Contour Flanges or Lofted Flanges, but in the overall picture of making the sheet metal model they hold their own.

Corner Rounds and Corner Chamfers

The key feature about Corner Rounds and Corner Chamfers? the “Corner” component of it. The advantage of these two features is they only allow for the selection of corners, those tiny edges that you’d have to zoom right into to select with the regular fillet and chamfer features. The fact alone that you do not need to zoom in and out saves oodles of time

Corner Rounds


The Cut feature has a couple advantages over the regular modeling extruded cut. First, it defaults to the thickness – meaning you don’t have to enter the extrude depth, nor switch to All (although you always have the option to set the depth)

Sheet Metal Cut

By enabling Cut Across Bend, Inventor wraps the sketched profile across the faces and bends the cut intersects with. The “wrapping” respects the active sheet metal style, meaning the resultant cut in the flat pattern is exactly the same size as the sketch geometry.

Cut Across Bend

Cut Normal is used when you want the feature cut perpendicular to the face(s) that the extrusion intersects.

Sheet Metal Cut Normal 1

Using the above model here is the difference between Cut and Cut Normal

Sheet Metal Cut Normal 2

Don’t discount the little guy!

Feature Image  Toying With The Men by JD Hancock

Autodesk Inventor: Bolted Connection Generator Irritation

There is a bug in the Autodesk Inventor Bolted Connection Generator that needs to be addressed. While there are work-a-round’s that can permit the use of the generator with curved faces, these are not convenient or sane, leaving the user to add respective hole features in each part manually. This should be corrected.

Autodesk Inventor Bolted Connection Generator

I am working with an assembly that contains numerous components, two of which have continually curved faces. These need to be fastened together, and I decided that simple threaded bolt option would work well. I wanted to use the Bolted Connection Generator at the assembly level in order to automate the fastener work in all respective components; Grand idea.

Knowing that I needed some feature to seed the generator’s path and start point, I opted to use a pilot hole, having used that successfully in the past. Simply add a small pilot hole in the part which the generator can later ‘latch onto’; this will guide the foundation of the generator process. Furthermore, the pilot hole is nice when you are not sure what size the fastener will ultimately be, but know where you want the hole at the part level. This was opted for in lieu of a point added at the assembly level. I prefer the assembly to be as clean and free of clutter as possible.

All options (which are only a portion of the possible ways to attack this) are ultimately pointless, as the Bolted Connection Generator must have a flat face in which to start the fastener from.

I could have provided a plane at the axis-surface intersection, but that would be a bit clumsy, and the generator will not accept a plane type work feature as an input. However I am not saying that I want that as my solution because that is still junky and awkward.  Also, I could have opted to prime the surface with an extruded tangent face, perhaps the diameter of the aforesaid pilot hole. That would have worked, but would have been a bear to duplicate throughout the design as needed.


What we need is for the system to recognize that I need a ‘Bolted Connection’ along an axis (or hole), originating the start point at the axis to surface intersection. Better yet, for the system to recognize the offset differences along the curve, and compensate a tad bit deeper for the mid-ordinate offset. This would be useful in countersunk and spot-faced applications to ensure the fastener sits perfectly flush. (It’s not difficult to calculate the mid-ordinate offset, but if anyone needs that reference, we have it here (Shameless plug):

Autodesk Inventor Assembly Threaded Hole

As I have written numerous times in the past, I love the Bolted Connection Generator, but this type of awkwardness needs to be addressed as more and more organically-shaped features are being introduced into production.

Beware my power, Inventor’s Contour Flanges!

Growing up I was into comic books, nothing out of the ordinary, but I loved getting the new issues of my favorite titles and reading and re-reading them. I had favorites, but one of my all time favorites was (is) Green Lantern. I had dozens of them. They were mostly of the Hal Jordan Green Lantern, but I had some from all of them…. Alan Scott (Golden Age – JSA), Hal Jordan (Silver Age – JLA), John Stewart, and most recently Kyle Rayner. The attraction? Hal Jordan was cool, he was a fighter jet pilot, and knew how to kick butt. Plus the concept of Green Lantern is inspiring, their only limit to their powers is the colour yellow and the limitation of their minds. Using their rings they can build “constructs” which are solid green objects that the Green Lantern controls telekinetically. These constructs can literally be anything.

In Blackest Night

In the Blackest Night by JD Hancock

When working in sheet metal it’s often advantageous to work with the side profile and “construct” the model by extruding the profile. With Contour Flanges, you sketch a thin profile and use this to generate the model. The Contour Flange is either extruded as the base feature or set to follow existing edges.

“In brightest day, in blackest night, No flat sheet escape my sight. Let those who worship non-bent metal’s might, Beware my power, Inventor’s Contour Flanges!!!”

Extruded Base Feature

The first step is a sketch, as the Contour Flange is a sketched feature. The key is to create an open loop, just the edges representing the shape you want to create.

Contour Flange Sketch

With the sketch created start the Contour Flange and pick the sketch. As the base feature in the model, Inventor will automatically offset the sketch to create the thickness. The amount of offset (aka the thickness) is set within the Sheet Metal styles. The Offset Direction toggle is used to set the direction of the offset, including in both directions to use the sketch as the centerline of the new model. Within the Bend Extents section set the desired extrusion length and set the extrusion direction, very similar to the extrude command. Like most Sheet Metal features you can override the style settings on the Unfold Options, Bend, and Corner tabs of the dialog

Contour Flange Extrusion

Inventor automatically applies bends to the intersections of the connected faces

Contour Flange Bends

Now that you have the base feature use flanges, folds, hems, etc to further develop the model

Secondary Swept Feature

The second application of the Contour Flange is to follow (sweep) along existing face edges. As with any sketched feature, the first step is to create a sketch. In this instance though sketch on the side face of the existing model, creating the desired profile.

Contour Flange Sketch 2

After starting the Contour Flange feature select the sketch and then the edges to apply the profile. The Sketched profile is swept along the selected edges, bend radius applied to the edges, and mitred corners automatically applied.

Contour Flange Select Edges

Use the onscreen glyphs to make adjustments to individual flanges

Contour Flange Glyph Overrides

The results

Contour Flange Swept Result

See it in action…

Feature Image: “… with my power ring.” via photopin (license)

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