Sheet-Metal Shenanigans (Avatech Tricks Tutorial)

Feed Inventor the information it needs to solve flattening equations.

In this column, we will focus on two tips to help you understand Inventor's prompts and needed input. The first tip addresses the non-tangent curves message. The second explains the error ASMFlatPattern: Could not build this ASMFlatPattern that is produced when you try to flatten a cone. Both resolutions are very simple once you understand what Inventor needs to solve the equations for flattening.

Use the Contour Command
In our first example, let's model a simple clamp.

In this first example, we're going to model a clamp.

We will use the Contour command to generate the part, but we will add two additional geometric entities to allow Inventor to solve the flat pattern. Start a new sheet-metal part and sketch this rough geometry. (You don't need to use the exact dimension shown here, just get close.)

To begin, start a sheet-metal part and sketch geometry similar to this one.

Once you create the geometry, next use the Contour command.

Start the Contour command.

Once the Contour dialog opens, select the profile.

Once you select the profile and press OK, you receive the following message:

Once you select the profile and press ok, this warning appears.

You may interpret this as an error and be frustrated, but I think of it as a communication of required information. When you see this warning, you only need to provide Inventor with more accurate information. In this case, the application is saying that it needs tangential connection points at the curves. Note that Inventor will create this 3D part! The message is only informing us that Inventor will not create the flat pattern unless we provide tangential connection points.

To resolve this issue, let's go back to the original sketch and add the tangential curves using the Fillet command found in the 2D Sketch menu.

Next, use the Fillet command and add tangential curves.

We used a fillet value of 0.25 here, but once again the dimensional values are not important. Just enter something close for this example.

When we follow the same steps this time around, the Contour command does not prompt us with the flattening message and Inventor creates the accurate flat pattern.

Flatten a Sheet-Metal Cone
Our second example shows one way to create a sheet-metal cone that we want to flatten.

Start a new sheet-metal part and sketch this rough geometry. You do not need to use the exact dimensions shown here; just get close. Note that we used metric for this example.

Sketch a sheet-metal part similar to this one.

Use the hot-key R to issue the Revolve command and change the Extents to Angle with a value of 359-degrees and press OK.

In the Revolve command's dialog box, change Extents to Angle with a value of 359.

Select the face of the cone and then start the Flat Pattern command.

Inventor now gives a failure message containing the solution. Note that the last line states that we need to check the Thickness setting. In this example, I used the Align Dimension with a value of 2mm. Inventor's Sheet Metal needs this value to be set to the Parameter value: Thickness.

This message points out the problem and tells you what to check.

Activate the Sketch and edit the 2mm dimension and type in the parameter Thickness and press the green check mark, Right Mouse Button and Finish Sketch.

Now, select the Face of the Cone again.

Next, issue the Flat Pattern command, and Inventor should generate a similar result.

Finally, the flat pattern works.

You may now continue to design your part, or begin your 2D annotation.

Generate Useful Geometry
Providing Inventor with the proper information enables you to generate useful flat pattern geometry. Luckily, Inventor not only tells you when there's a problem, but also gives you clues as to where the problems are.