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Inventor Sheet Metal Drawings

Although we live in a 3D world, for many the 2D drawing still rules the roost. Inventor provides a set of tools specific to creating Inventor Sheet Metal drawings

Inventor Sheet Metal Drawings

When creating drawing views of sheet metal models you can select the Folded Model or the Flat Pattern. When creating views of Flat Patterns take note of the options to include the Bend Extents and Punch Centers.

Inventor SM Drawing Views

This means your sheet can contain views of both the model and its flat pattern

Inventor SM Base Views

Take a look at Don’t Misjudge the Flat Pattern for more information on Flat Pattern management. How you configure the flat pattern may impact how it appears in the drawing.

The colour and line weight of the bend lines and optional bend extents is managed within the styles

Inventor SM Bend Layer Properties


The Flat Pattern can be dimensioned with any of the dimensioning tools, including baseline, continuous, and ordinate.


Inventor SM Drawing Dimensioning

Ordinate comes in two options: Ordinate and Ordinate Set. 

With the Ordinate option, you first locate the origin marker marking the 0,0 point for all the dimensions to reference in that view. Next you select the geometry to dimension then pick the dimension location. Initially, all ordinate dimensions created will be aligned but they are actually individual meaning they can be moved and adjusted independently of the rest.

With the Ordinate Set option, the first object selected becomes the origin location, but this can be adjusted later. The biggest difference with this feature over the Ordinate option is that the dimensions are grouped together and are adjusted as a group.

Adding Annotations

Use Bend Notes to label bends including the bend’s radius, direction, and other information. It works by picking (or window selecting) the bend lines to label and it locates the note without leader. After placement (if required) drag the label to a new location and the leader is automatically added.

Inventor SM Drawing Bend Notes

The appearance and the contents are managed by the active style

INventor SM Bend Note Styles

Using the General Table feature, you can add a Bend Table to the drawing both listing and labeling each bend in the Flat Pattern. After starting the General table tool pick the Flat Pattern view. Use the Table dialog to configure the desired columns (bend properties).

Inventor SM Drawing Views

When you click OK and place the table Inventor additionally numerically labels each bend. As with the Bend Note you can drag the label to a new location and the leader is automatically added.

Inventor SM Flat Pattern Bend Table




Feature image “Music sheet” by Mari Ma

Converting Models to Sheet Metal with Inventor

You’ve started a new model, worked hard, and it’s looking good…. but then it happens, you realize it should have been made in the sheet metal environment! Or a different scenario, you’ve imported a model but its come in as a solid blob and you need to flatten it out.

This is my continuation of a series taking a deep dive into Inventor’s Sheet Metal environment. There isn’t really an order that they have to be read, but you can start with the first one here Holy Sheet Metal Batman!

Autodesk Inventor allows for converting models to sheet metal. Which means, regardless where the model geometry originates, you can convert it to sheet metal, add sheet metal features, and generate the flat pattern.

Let’s start with the rules of sheet metal

  • Rule #1 You must have a consistent thickness
  • Rule #2 Your sheet metal thickness parameter MUST match the thickness of the model
  • Rule #3 You cannot have one continuous face, there must be some type of gap
  • Rule #4 Although Inventor now supports sharp corners there still needs to be a round (fillet) on the outside edge

Say we start with something like this. I know what you are thinking…. “that’s simple, we don’t model anything like that“… but we’re going to use this shelled box to showcase the features required for the conversion.

Inventor SM Conversion Start

Converting Models to Sheet Metal with Autodesk Inventor

First step, activate the Sheet Metal Environment. This actually does more than just activate a set of tools, it automatically creates a set of parameters, the ones required for the sheet metal “magic” to happen

Inventor SM Parameters

I know as a shelled box we’ve got a model with a consistent thickness, I just need to tell Inventor what to use. Within the Sheet Metal Defaults dialog, I can either edit the rule to define the thickness or as in this example I override the rule thickness and specify the value to use

Inventor SM Defaults

Now lets add a Corner Seam using the Rip option. The Rip option is purposely built to work with part models converted to sheet metal. It creates the required break in the faces so that model can be flattened. One small problem, and I quote the help here “You can rip a corner seam to open an edge between faces. The resulting open corner typically leaves material that must be removed.

If we skip ahead and look at the final result (Corner Rip + 2 Bends) I can see a small remnant that must be removed. It’s not really a problem, just a bit of extra work.

Inventor SM Conversion Extra Material

Is there a way to do this without needing a sketch and extrusion after? How about when I create the Corner Rip I specify the overlap option instead, even though my final result is to not overlap in the corner

Inventor SM Corner Seem Rip2

Next I add Bends in the corners. I could do this with fillets, but the Bend feature takes care of rounding both the inside and outside edges, as well as setting the radius to the BendRadius parameter. In my example, I need to apply two Bends.

Inventor SM Bend

The resultant corner is not ideal but is exactly what I asked Inventor to create.

Inventor SM Conversion Unwanted Corner

To produce the desired condition I apply another Corner Seam, but this time using the Seam option

Inventor SM Conversion Corner Seam

I now can produce the flat pattern

Inventor SM Conversion Flattpattern


Data Conversion

Here is a model originally modeled with Solidworks that I opened (and converted) into Inventor. As it was modeled using the Solidworks Sheet Metal tools the conversion process is very straight forward. It’s not just with Solidworks files though, you’ll probably find any sheet metal modeled solid transfers into the Inventor sheet metal environment seamlessly.


Inventor SM SWx Conversion

After initiating the Sheet Metal environment, Inventor prompts to select the Base Face. Upon selecting the base face, it extracts the thickness of the selection as the thickness parameter

Inventor SM SWx Conversion Pick Base Face

And with this model that is all that is required. I can now create the flat pattern

Inventor SM SWx Conversion Flat Pattern

I can guarantee that it will not always be this simple, although Inventor 2016 seems much better at translating data.

I have seen many Solidworks models that for whatever reason just don’t flatten, even though it follows all of the Sheet Metal rules. The trick I have found is to copy the imported solid into the construction environment, delete the original model, and then copy the construction solid back out. Whatever Inventor does during this process I do not completely know, but who am I to question something that works?


Feature image sheet metal and nature by Robert Bejil









The ForceEffect Awakens in Inventor 2016 R2

Inventor 2016 R2 is upon us. If you haven’t heard about R2, it’s the first of what’s promising to be quarterly releases for Inventor. Autodesk has announced that every quarter we should be seeing these bonus packs of new features, updates, fixes, and other goodies. You can read more about R2 in John’s post Inventor: October Update and Move Away from Annual Releases and my previous post Autodesk Inventor 2016 R2 – Shape Generator

The theme for R2 is Open | Connected | Professional Grade and Autodesk has a goal to “help you innovate, collaborate, engineer and make great products”

Great products start with good concepts, strengthen by good concept engineering tools. Have you taken a look at Autodesk’s collection of mobile apps lately? It really has exploded, where they now provide a full breadth of tools (and games) for every industry. These tools are available online in your browser or on your smart device. One of these is Autodesk ForceEffect.

Unlike the traditional approach of using paper, pencil, and a calculator to develop equations for design options, Autodesk ForceEffect does all the simulation and engineering calculations for you right on your mobile device, enabling you to quickly and easily simulate design options during the concept phase to determine the viability of a design.

What does this have to do with Inventor? Well, drum roll please,….. with R2 ForceEffect is embedded right in the Part and Assembly environments! That’s right, without leaving the comforts of Inventor use ForceEffect for creating free body diagrams, to test your design concept early in the process. When you finish with ForceEffect you can link the geometry into Inventor as a skeleton sketch.

Inventor 2016 R2 + ForceEffect

After applying R2, the ForceEffect panel will appear on the Add-Ins tab, with options for New and Open.

Inventor 2016 R2 - Add-ins tab

Before diving in I recommend a couple things… #1 I know ForceEffect is simple to use, but take the 60-seconds and take a look at the GettingStarted (Help Panel). #2 take a gander at the Tutorials. Not saying you need to actually work through them, but take a read as you might pick up a few tips.

Inventor 2016 R2 - GettingStarted

Another resource touted by Autodesk is the free ForceEffect iBook available in iTunes (here). I’m not an Apple person and it doesn’t seem to be available anywhere but iTunes…. I’ll just have to take Autodesk’s word that it’s a great resource! But if you’ve got access to iTunes, don’t let my apple-less-ness stop you from using this resource.

Building Your Inventor 2016 Diagram

Everyone’s workflow is probably a little bit different, but I typically start by selecting the analysis type, either Static or Kinematics. If I’m going to be using an image as the background, I set that initially as well.

Inventor 2016 R2 - Start

Next comes the geometry in the form of elements or construction objects. As you click-and-drag to generate the element, dimensions appear to aid in setting the right length. After locating the second point double click the dimension to set to a specific value. Snapping occurs automatically, both to end points and in relation to existing geometry. Kinematic expands the geometry types to include Free Hand elements

Inventor 2016 R2 - Adding Elements

At any time, you can switch back to selecting objects to make existing elements. As you select the element the dimension appears and with a double click you adjust the length. With the object selected, right-click and use the marking menu to delete the element, change its length, or set its weight.

Up in the right corner of the modeling window is the Degrees of freedom icon, a visual indicator of the current state of your diagram.

  • Red = indeterminate state [Elements can move & the static calculations cannot execute]
  • Green = equilibrium state [diagram is optimized… aka good-to-go]
  • Blue = overdeterminate [over-constrained]

Inventor 2016 R2 - Marking Menu

With the elements defined, now add supports including Sliding Pin, Fixed Pin, Grounded Support, and Piston. The goal with Static diagrams is to use a combination of supports and joints to reach 0-degrees of freedom.

To add joints select the end connector of an element and right-click, the marking menu provides the joint options. The Joints listed in the menu is dependent on the selected geometry.

Inventor 2016 R2 - Add Joints

To check remaining degrees of freedom drag the elements within the modeling window. The elements will only move within their open degrees of freedom

Finally, add the desired loads (known, unknown, variable distributed) and moments


As your diagram moves into the equilibrium or overdeterminate states ForceEffect calculates reaction forces and moments. Via the right-click marking menu toggle the displayed force vectors between combined and X & Y component.

Inventor 2016 R2 - Result TypesWhen satisfied the results, select Report from the ribbon. The generated HTML based report, compiles the inputs, outputs, and visual elements to create an extensive report

Inventor 2016 R2 - ForceEffect Reports

ForceEffect Diagram = Inventor Sketch

Now, this is where it gets very cool… select Part Skeleton or Assembly Skeleton to open the diagram as an Inventor skeleton sketch. The ForeEffect elements are converted to Inventor sketch lines, constrained with the reference constraint. Until you remove the reference constraints, the sketch geometry remains associative with the diagram.

Inventor 2016 R2 - ForceEffect Associative Sketch

Use the new ForceEffect panel within the Sketching environment to open the diagram. When changes are made update the geometry within the sketch. Completely round trip!

See it in Action!

Using this will really make you wonder how you’ve survived this long without it. ForceEffect is so easy to use, yet still supplies a robust set of tools.

Feature Image 110716-1240498-i by Walfer X

Autodesk Inventor 2016 R2 – Shape Generator

As per John’s recent post (“Inventor: October Update and Move Away from Annual Releases“), subscription customers are in for a treat with the availability of what I like to call the R2 Subscription Bonus Pack. This update provides new tools and features to Inventor’s already extensive “Professional Grade” toolkit.

By claiming Inventor is Professional Grade, Autodesk is aiming to have it be an “end-to-end product development environment.” Part of the reason they are able to accomplish this is by leveraging technology from other products in their ever-growing product portfolio. R2 contains three main “buckets” of enhancements:

  • ForceEffect integration for upfront concept engineering
  • Shape Generation to build structurally efficient parts
  • Improved IDF import

Shape Generation

The Shape Generator was a real “ah-ha” moment for me in that I realized that topology optimization wasn’t just for 3D printing and plastics. There is a potential here for any industry using Inventor. To read more about Autodesk’s path to introducing Shape Generation, take a look at my recent article “The more things change: Generative Design”

Inventor 2016 R2 - Welcome To Shape Generator

According to Autodesk, Inventor is the first product to offer Shape Generation inside the CAD application.

“This release is more than just an update. It’s the future of true ‘computer-aided’ design”

Shape Generation is a conceptual design tool that relies on finite element methods to optimize material for a defined set of criteria. You specify the boundary conditions, the loads, and the target and it figures out how to remove or deform the material to hit the target. The result is a 3D mesh, which you can reference back into your model to refine your design.

Shape Generation in Action

The process of Shape Generation follows the typical FEA process…

  1. Start the Environment
  2. Assign / adjust materials
  3. Apply constraints
  4. Apply loads
  5. Preserve Regions
  6. Adjust the Settings
  7. Generate the shape

To start the process, with the desired part model open, select Shape Generator from the 3D Model ribbon tab. Alternatively, Shape Generator is now an option from the New Study dialog within the Stress Analysis environment… same toolset, just two ways of getting there.

Inventor 2016 R2 - Shape Generation Ribbon Location

The material will default to the material assigned from the modeling environment. To adjust this select Assign from the Material panel and make adjustments as required.

Inventor 2016 R2 - SG Materials

Three options are available for constraints: Fixed, Pin, and Frictionless. These are exactly the same as you would find within the Stress Analysis environment. Use Fixed to remove all degrees of freedom from the selected edge / face / vertex. Pin is used to represent a hole on a cylindrical support.  Frictionless prevents a surface from moving (deforming) in the normal direction… aka, it stays flat (parallel)

Inventor 2016 R2 - SG Fix Constraint

Loads contain many options, that can be applied to vertexes, edges, and faces. The point is to load the model as it will be in the real-world, using whichever combination of loads required.

Inventor 2016 R2 - SG Force

Preserve Region is a tool specific to the Shape Generation Study environment. With this, you specify features that you do not wish to change during the shape generation process. The selected regions are specified as boxes or cylinders.

Inventor 2016 R2 - SG Preserve Shape

Within the Shape Generator Settings specific the target mass reduction and the mesh density. Remember that the greater the density of the mesh, the longer the process will take to run. [Cloud processing is not included in this release, hopefully in the future]

Inventor 2016 R2 - SG Settings

With everything set it times to click the Generate Shape button and wait for the magic to happen. Depending on the density of the mesh and the complexity of the model, this may be a get-up and go-and-get-coffee opportunity.With the analysis complete, you can promote the shape either as an exported STL file (for 3D Printing) or into the active model to compare against the existing model.

If you are interested in more about the theory of Shape Generation the Inventor help includes a section (“Validation Problems”) for reference.

Inventor 2016 R2 - SG Help

Feature Image: Wire mesh” by haru__q

Wax On – Wax Off… Unfolding and Refolding with Inventor Sheet Metal

If you are a child of the 80’s like me you probably remember the classic movie the Karate Kid…  and I don’t mean the sequels, reboots, remakes, or any of the other stuff… I’m talking the original one. It was the story of using determination and heart to accomplish your goals and come out on top. It also gave us one of the most quoted dialog ever:

Miyagi: First, wash all car. Then wax. Wax on…
Daniel: Hey, why do I have to…?
Miyagi: Ah ah! Remember deal! No questions!
Daniel: Yeah, but…
Miyagi: Hai!
[makes circular gestures with each hand]
Miyagi: Wax on, right hand. Wax off, left hand. Wax on, wax off. Breathe in through nose, out the mouth. Wax on, wax off. Don’t forget to breathe, very important.
[walks away, still making circular motions with hands]
Miyagi: Wax on, wax off. Wax on, wax off.

As we continue the deep dive into Inventor Sheet Metal let’s explore Inventor’s own Karate Kid… Unfold and Refold!

Using Unfold you can unfold portions (or all) of your sheet metal model to reveal the flat pattern, and unlike when working on the flat pattern, changes you make will be applied to the model when you Refold the unfolded bends. This means you can construct the model with whichever tools you want, without needing to be concerned about how to incorporate pre-bending features into the model

Inventor SM - Unfold Dialog

With Unfold, you start by selecting a Stationary Reference… aka the face that doesn’t move. All selected bends will unfold relative to this selection. In the above picture, I select the longer horizontal face as the stationary reference. Next you select the bends to unfold. Unconsumed sketches do not automatically unfold with the bends, but they can be selected with the Copy Sketches (C) option.

Inventor SM - Unfold Dialog 1

With the bends unfolded, add features as you normally would as now you are basically working with the flat pattern

Inventor SM - Unfold Add Features

You now have two options to Refold; Refold or Refold Feature. The Refold opetion works exactly the same as Unfold, except you can only select bends previously unfolded

Inventor SM - Refold Dialog

The second option, which is the most efficient when you want to refold all the unfolded bends, is the Refold Feature option. To do this locate the Unfold feature in the browser, right-click it, and from the menu select Refold Feature…. and voila! The model is back to its folded state

Inventor SM - Refold Feature


As you can see from the example you can create some very crazy results. However, Inventor is applying the proper corrections meaning everything is theoretically correct!

Now, there is one thing that I get asked a lot about Unfold that, unfortunately, is not achievable out-of-the-box. There is no way to stage the model to create drawing views of the various bends unfolded and then folded. It would be great if we could use Level of Details at the part level to manage feature suppression. We’d then be able to suppress the unfolds / refolds to create various drawing views, showing the order of operations for manufacturing the component.

Thanks and a big fist pump go to Adrian S for sharing a great trick on generating stages within the model. The trick… use iParts!

Inventor SM - iPart with Unfolds

By creating an iPart, you can generate multiple versions, managing the suppression of the unfold features. Using a iPart version per drawing view, you can show the desired order of applying the bends

Inventor SM - Staged SM Drawing with iPart


Feature Image Karate Summer Camp by Flavio

Breaking it down – Limits and Fits in Inventor / HSM

In this article, I’ll explore a workflow for utilising the Limits / Fits tools in Inventor, to maximise the benefits of using an integrated CAM system for precision machining. To start off with though, I’m going to explain a bit about Limits / Fits for the uninitiated.


When a particular design calls for a precise fit between two components, every engineer I know usually pulls out his/her copy of Machinery’s Handbook (or Boundy) and looks up the table of Limits/Fits. Inventor has these fits built in, so as long as you know what you’re looking for, it will put the correct tolerance limits on dimensions in the drawing environment, for you, once you have specified the appropriate fit. A slightly lesser known feature, is that tolerances can be used in the modelling environment as well. These model dimensions can then be retrieved and placed on the drawing.

Limits / Fits

For those of you who may not have dealt with Limits / Fits in a CAD environment, you typically dimension the part with a nominal dimension, and then specify a tolerance by listing upper and lower limits for the specified quantity. This allows the machinist a range to work within, that ensure the correct clearance or interference between the two components, regardless of whether he/she is at the upper or lower limit.

The limits/fits that everyone uses today, were conceived a long while ago, by clever people who are now probably long dead. Their age doesn’t make them any less useful today.

Broad fits categories

  • Clearance – There is always a gap between the 2 components, regardless of whether each part sits at it’s upper or lower size limits.
  • Transitional – Depending on where each part sits between upper and lower limits, there may be a gap between the two components, they may be identical in size, or material may even need to be deformed/displaced to fit them together.
  • Interference – There is always material required to be deformed or displaced in order to get the parts to fit together.

Within those categories, sub-categories of fits are often described using descriptive names such as “Loose-Running,” “Close-Running,” or “Sliding.”

You can choose to base the fit on either the hole or the shaft, and the codes for the fit are either upper or lower case to designate this.

Now obviously, if you have a range of possible sizes for the shaft, and a range of possible sizes for the hole, then there are an infinite number of permutations between the extremes. To deal with this, we often just look at the best and worst case scenarios and decide if they are suitable.

If the hole diameter is at the upper limit, then the component (with the hole in it) has less material than one with the hole diameter at the lower limit. In other words, a bigger hole removes more material. Conversely, a shaft whose diameter is at the upper limit has more material, than one whose diameter is at the lower limit.

So we have two combinations which form the extremes of the fit between these two components. The first is the biggest possible shaft in the smallest possible hole, and the second is the smallest possible shaft in the biggest possible hole. In a clearance fit scenario, they give the smallest possible clearance, and largest possible clearance respectively. We call the first scenario the “maximum material condition,” and the second, the “minimum material condition.”


If we have, say, a pin that needs to fit into a boss, but slide in a smooth fashion and remain co-axial to a high degree of accuracy, we may choose a Close Running fit. This has corresponding codes of H8/f7 in the hole basis system, and f8/H7 in the shaft basis system.

We’ll be using the hole-basis system, which means that the nominal size lies on the lower limit of the hole diameter. Another way to think about this, is if we have a perfect hole, exactly at the nominal diameter, then we will have to remove material from the shaft to get a clearance fit.


The nominal diameter is 50mm, and the H8 limits for that size give a range of 50.000mm to 50.039mm. This means that if the finished part comes out anywhere between these values, we would consider it a “pass” and it will give the desired fit when the shaft is inserted into the hole, as long as that is within it’s acceptable range too.


The nominal diameter is 50mm, and the f7 limits for that size give a range of 49.975mm to 49.950mm.

So when the parts are assembled, you can see that there could be a maximum clearance between them of 0.089mm, and a minimum of 0.025mm, depending on where the individual components sit within their tolerance range.

So how do we represent this information in our CAD model, and how do we go about conveying this information to the machinist you ask? Good question, I’m glad you asked….

Well, the way it has generally been done for as long as I know of, is that components are usually modelled or drawn at the nominal size. Tolerance notes are then added to the dimensions on the drawing, to show the machinist the acceptable range for dimensions of the finished component.

Toleranced DimensionAn example of a nominal diameter dimension with a fit code, and size limits

This is all well and good if the machinist is making this component by hand, and can adjust the size to suit, but what if we want to control a CNC machine using the modelled part? We can’t just toolpath everything at exact size, otherwise fits won’t work. Sometimes CNC operators adjust the offset parameters in the machine control to cut slightly bigger or smaller, but this is not a very good way to manage things. Even worse is hand-editing the machine code, as it gives opportunity for error and is slow.

A skilled machinist can definitely achieve very high accuracy on manual machines, but usually it is a case of removing material until close to size, and then taking a series of small cuts, with measurements in between, until the finished size is reached.

With CNC machines, this is not an easy or efficient process to use, as you have to wait for the program to complete, then create new code or make adjustments, before starting a program again. A much nicer way to work, is to have a good program, that you know will produce a part of the required dimensions.

So how do we create a model that can be toolpathed to give exactly the required result?

This is where the fun stuff starts. In Inventor, when you specify a value for a parameter, you can click the little arrow to the right side of the input box and select “Tolerance.” This will bring up a dialog that allows you to add tolerance information to the parameter.

Inventor Tolerance SettingsThe tolerance settings for an Inventor Parameter

By changing the “Evaluated Size” you can change where in the tolerance range, the actual model sits. You have 4 options, shown below.

Inventor Tolerance DialogThe tolerance dialog – What the various options do

So you can have the model represent either the maximum material condition, minimum material condition, nominal size, or half way between upper and lower limits. This gives a great deal of flexibility for use in the CAM environment (Inventor HSM), but also for visualising the fits, which I’ll show in more detail below.

When creating the CAM program, the software uses the actual geometry of the solid, to calculate the toolpaths. If you model it at the nominal diameter, then the CNC machine will machine it to close to the nominal diameter. I say close because all machines have some degree of error.

If however, you pick a tolerance that is at least twice the known potential machine error, then by selecting the “Median” value for the “Evaluated Size” option in the tolerance box, your finished part should end up within tolerance, because the toolpath will be calculated on the median value.

To illustrate what I mean, have a look at shaft diameter in the model, with each of the “Evaluated Size” settings selected:

Options to give maximum material conditionUpper Limit (Click to zoom) Options to give median material conditionMedian (Click to zoom) Options to give Minimum Material ConditionLower Limit (Click to zoom)

Proving it out

To prove it out, I created the following turning toolpath in HSM, with the “Evaluated Size” option in the model set to “Lower Limit.”

Turning Toolpath

I then posted the code and inspected the X-axis coordinate of the final cutting pass (i.e. the finished diameter.)

G-Code Example

I hope this has given you some ideas for utilising the Inventor tolerance capabilities in a machining context. I think it’s a really neat way to keep the manufacturing information inside the CAD model, and helps to create a richer digital representation of the component that is being manufactured.

Until next time…

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