Autodesk Inventor Sheet Metal, Flat pattern success – Every time!

Autodesk Inventor Sheet Metal, Flat pattern success – Every time!

Seven tips to guarantee that Your Autodesk Inventor Sheet Metal models will flat pattern without errors.

'Failure in creating flat pattern'. Who needs it? Autodesk Inventor Sheet Metal Flat pattern success  Every time 1 No-one wants to create an Autodesk Inventor sheet metal part that won't unfold!

The Inventor sheet metal environment is designed to flat pattern developable geometry. Think of the shapes you can make from a flat sheet of metal and a brake press.

Inventor will not flat pattern 'pressed' shapes - for example a car door.

Inventor has its own modelling environment for creating sheet metal parts and Inventor will also develop flat patterns for imported components from other CAD systems.

In this blog post I'll give you my top seven tips for making sure that your Sheet metal parts will flat pattern every time :)

Click this link to download our Autodesk Inventor Sheet Metal training agenda.

#1 Model with Autodesk Inventor's sheet metal environment.Flattening-Complex-Shapes

OK. This one is kind of obvious. We rarely receive support calls from people who have created models in Inventor's Sheet Metal environment that won't develop.

In the past we have received lots of support calls from people using derived or multibody workflows to create their Sheet Metal assemblies from multibody parts.

Now that we have multi-bodies support in the sheet metal environment (Inventor 2016), this shouldn't be so much of an issue!

The tools in the Sheet metal Environment allow you to model some forms that will develop in the Sheet Metal environment that Inventor won't develop if you try to flatten the same shape as imported or derived geometry.

Check out the 'twisted' component in the image included that was built with the contour roll tool.

If you have the choice, use the Sheet metal tools to model your Sheet Metal parts. If you don't, please consider the tips below.

#2 leave a gap

Your model cannot be completely continuous. Make sure you leave a gap to allow unfolding.

Inventor's 'Rip' tool can be used to add a gap to parts that don't have one.


#3 No overlapping folds

The Autodesk Inventor Sheet Metal environment has a great tool for detecting overlapping folds.

Although you can develop a flat pattern that has overlapping folds, Inventor will complain about it, and won't stop complaining until you fix it!

If you are using the Sheet Metal environment, you can adjust your flanges to suit.

If you are working with imported files, you could use Autodesk Inventors direct modelling tools to fix up the problem component.


#4 Consistent Thickness

To develop a flat pattern, Autodesk Inventor must start with a model that has a consistent thickness – just like a sheet of metal in real life.

This issue often arises when you build a multibody component and then split it up and derive the bodies into Sheet Metal parts.

My top tip here is to model using surfaces and then use the thicken command to model a solid with a constant thickness.


You can thicken the surface in the Multibody part and derive the body into a sheet metal part, or derive the surface into a Sheet Metal part and then Thicken in the Sheet Metal part file.

Note: The Thickness of your model must be the same as the Thickness in the current Sheet Metal Style that you are using.

Inventor will have a stab at guessing the Thickness of an imported component. To set this manually – measure your parts thickness, and then override the thickness in the Active Sheet Metal Style to match your model.

#5 Perpendicular edges


Inventor doesn't like developing flat patterns of parts that have wobbly edges!

To make sure that your models edges are perpendicular to the face, use the Thicken tool to build your model from surfaces, as outlined above.

When building Sheet metal components, make Graitec-Autodesk-Inventor-Split-and-Thicken-for-Perpendicular-Cuts sure that your cuts are perpendicular to your faces using the options available in the cut tool's dialog box.

One tip to create perpendicular cuts is to use the split face and thicken method.

#6 External fillets

Inventor won't develop parts that have 90 degree external corners. Inventor will develop flat patterns from components that has a 0 degree internal corner, but the external corner must have a radius.

Zero degree internal corners were added for customers using Inventor's Sheet Metal tools to develop designs from material such as cardboard that 'crush' a lot more on the internal corners that Steel does!

#7 Developable Surfaces

To flat pattern a Sheet Metal component, your design must be 'Developable'.

A developable surface is a single curved surface that can be flattened out without distortion.

A developable surface will always be a ruled surface - that is surface on which you could hold a rule against at any point and by twisting the rule, find a direction where the straight edge of the rule would touch all the way along the surface.

However - a Ruled surface is not always a Developable surface, such as in the case of a double ruled Hyperboloid.

Developable surfaces include planes, cylinders and cones. Non-developable surfaces would be those that have compound curves, such as Spheres and Nurbs surfaces.

Here's a really good post by Gaetan Kolher that shows the difference.

Autodesk Inventor Sheet metal modelling tips

If Inventor has trouble flat patterning a part, select a face on the part before you use the flat pattern tool. The 'A' side tool is equivalent to making this section permanent.

Use the sheet metal bend tool to add bends to square corners. Right click on a bend and edit to turn it into a corner.

If you have imported a component from another software package and you are really struggling to get a flat pattern, use Inventor's curvature inspection tools to look for areas that are not flat, faces that are not parallel (Equal thickness) or edges that are not perpendicular to the faces.


Check out this article by Mike Thomas for more tips on working with imported files in the Sheet metal modelling environment.

10 Design tips for Sheet Metal fabrication


Before you start modelling parts for sheet metal fabrication, talk to the fabricator to see what they can achieve for the budget you want to spend!

Here are some basic rules of thumb for sheet metal design that have stood me in good stead over the years.

1. Speak to your fabricator before starting your design.

2. Make sure that the material thickness you are using is available in the material you want!

3. Allow bend relief.

4. Inside bend radius equal to material thickness (Minimum). This may need to be increased with materials like aluminium that are subject to cracking. Manufacturers typically have dies in a limited number of sizes – so check first.

5. Minimum hole size equal to material thickness.

6. Keep holes at least one material thickness from edges.

7. Keep holes at least 3 x Material thickness away from bends to prevent the holes from becoming distorted.

8. Avoid short flanges (four times material thickness)

9. Maximum boss depth = three times thickness.

10. 'U' channel legs but be equal to or geater than the base dimension.

If you are interested in purchasing Autodesk manufacturing Software or you want to find out about training then contact your local Graitec office today or request a quote!

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