How to create an Inventor Sheet Metal template with a Material Gauge Table.

To showcase the power of what iLogics bring to the table within Inventor we will create a sheet metal template that contains a material based gauge table. This will enable us to quickly change the material and gauge value and have our model update accordingly.

We start by opening the default steel metal template within Inventor and go straight for the parameters dialog box. We will then create three (3) user parameters we will use to drive the gauge table. The first is a Numeric parameter called “Gauge_Value”, the second is a Text parameter called “Gauge.” Our third and final paramter is also a Text parameter that we will call “Material_Type.”

Next we will make the “Gauge” parameter a Multi-Value parameter and add the gauge numbers we want included in our template. For the sake of simplicity we will use two values, let’s say 10 and 12. We will also make our “Material_Type” parameter a Multi-Value parameter and add values of “Steel” and “Aluminum” to it.

We will then edit the default Sheet Metal style’s Thickness and assign “Gauge_Value” to it. This can be done in an individual style or overridden in the main defaults.

After we will create an iLogic rule that we will name “Gauge Table” and we'll add the following code to it.

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Sub Main()

iLogicVb.UpdateWhenDone = True

Parameter.UpdateAfterChange = True

Select Case Material_Type

Case "Steel"

TypeSteel()

Case "Aluminum"

TypeAlum()

End Select

iProperties.Value("Custom", "Gauge")=Gauge

InventorVb.DocumentUpdate()

End Sub

Sub TypeSteel()

iProperties.Material="Steel"

Select Case Gauge

Case "10"

Gauge_Value=0.1345

Case "12"

Gauge_Value=0.1046

End Select

InventorVb.DocumentUpdate()

End Sub

Sub TypeAlum()

iProperties.Material="Aluminum"

Select Case Gauge

Case "10"

Gauge_Value=0.1019

Case "12"

Gauge_Value=0.0808

End Select

InventorVb.DocumentUpdate()

End Sub

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This iLogic code will allow us to pick a Material Type and a Gauge and it will assign the proper gauge thickness to our model. It will also create a custom iProperty called “Gauge” that we can use to port into your Drawing Part List.

To finish this template up we will add a Form to enable us to easily modify these parameters as needed. Let's create a form and call it “Setup,” then add the “Gauge” and “Material_Value” to it. As they are Multi-Value parameters the form will be populated with ‘Pull-Downs’ for both values. As an added measure we will add our “Gauge_Table” rule to the form and it will appear as a button. Then we will rename the parameters to whatever we like and rename the rule button to “Update”.

This is a very simple example of what can be done with iLogics to create models with embeded design intent. A link to a more complete example I've created can be found on GrabCAD.

I hope you enjoyed this tutorial and let me know in the comments if you have any questions.