Being Inventive

Calculating developed length for sheet metal bends larger than 90 deg

This question comes up regularly as users want to double check the developed length of their sheet metal parts.
The Inventor wiki help shows all kind of nice pictures and formulas for the developed length but if you look more closely you will notice that all the images provided in the wiki are for situations where the bend angle is smaller than or equal to 90 deg.

For bend angles larger than 90 degree, calculating the developed length proves to be a bit more involved.

The general formula of the developed length is: 

L = L1 + L2 - d

With

d = delta value as found in the bend table

b = bend angle  as measured in the image below

L1, L2  = the flange lengths measured to the tangency point.

   

   

 
Fig 1: Parameters needed to calculate the developed length of a bend

The most important aspect to understand in Fig 1 is how the L1 and L2 length values are measured.
They are measured "tangent" to the bend (see also the blue lines in Fig4).

Let's take an example. We start out with a 90 degree flange with L1 = 30 mm and L2 =20 mm (= flange height).

 

Fig 2: Initial 90 degree flange definition

We use a 2 mm bend radius. For that radius we use following bend table in the sheet metal unfold style:

Fig 3: Our bend table definition

We now modify the 90 degree flange to a 95 degree flange.

The most common mistake is to calculate the developed length as

L = L1 + L2 – d = 30 mm + 20 mm – 3.71045 = 46.289 mm

Our L1 and L2 values have changed of course and the L value is incorrect!

Fig 4: Measuring the L2 value

When we measure the L1 and L2 values appropriately, to the tangent line to the bend, filling in the values in the formula is uneventful.

L = L1 + L2 – d = 29.635 + 19.635 – 3.710405 = 45.559595 mm

The calculated result corresponds nicely with what can be measured on the flat pattern

Fig5: Developed length as measured on the flat

Hopefully this gives you an idea on how to reverse engineer Inventor's developed length and assures you a better night sleep, knowing that Inventor does an accurate job in calculating the length J

Bob

Creating non-perpendicular sheet metal cut-outs

A question that regularly pops-up is about how to create cut-outs in Inventor for a part that is sticking through a sheet metal part.

When the penetrating part is perpendicular to the sheet metal face it penetrates, there is no issue as you can use the regular "Cut" command.

But what if the penetration happens under an angle like in below image of a cylindrical part?

The cutout will have to be wider than the cylinder diameter to avoid interference.
It is relatively easy to determine mathematically what the width W of the opening needs to be.
I'll spare you the gory details on how exactly I got to these formulas but here they are:

 
 

 

Width of opening = d1 = Thickness / tan(TOOLANGLE) + TOOLWIDTH / sin(TOOLANGLE)

Height of opening = d7 = TOOLWIDTH (the Height of the opening is rather arbitrary and can even be made smaller if required).  

With

TOOLANGLE = the smallest angle between the penetrating tool and the sheet metal face. This angle is always <= 90 deg and > 0 deg.

TOOLWIDTH = maximum cross-sectional dimension of the tool when it penetrates the opening

 

With this knowledge, I decided to create three iFeatures. The three different cutout shapes are circle, oblong and rectangle.

You can download the metric 2012 part that I used to create the iFeatures here (so you can build more shapes if you like)

You can download the finished 2012 iFeatures here and use the "Insert iFeature" command rather than the "Cut" command for situations where the regular sheet metal "Cut" command is not giving the results you want.

Here is a snapshot of the 3 cutout shapes in action. Note that the cross-section of the penetrating parts can be an irregular shape different from circle,oblong or rectangle.

Cheers

Bob

Sheet metal extents used as custom iProperties

Inventor 2009 and 2010 can use the length, width and are of the sheet metal flat in a drawing text.

However there exists no easy way to extract and use these extent values in the sheet metal part itself through the UI. The Inventor API comes to the rescue.

Open the VBA editor and paste below code in a module of an APplication Project.

Save the project in the VBA editor so you can reuse it in other Inventor documents.

To use the macro, make sure you have a sheet metal part open as your active document.

Run the macro called extents_to_custom_props with Alt-F8.

This will create two custom text properties  "length" and "width", expressed in the document units.

Note that each time your sheet metal part changes,  you will need to rerun the macro to get up-to-date extent values injected in the custom props.

The "length" and "width" custom properties can of course also be used in the partslist on a drawing.

'--------------------- Cut here ---------------------------
Public Sub extents_to_custom_props()

 

    Dim objpartDoc As PartDocument

    Set objpartDoc = ThisApplication.ActiveDocument

    Dim objCompDef As SheetMetalComponentDefinition

    Set objCompDef = objpartDoc.ComponentDefinition

    Dim fpBox As Box

    Set fpBox = objCompDef.FlatPattern.Body.RangeBox

    Dim width As Double

    Dim length As Double

 

    length = fpBox.MaxPoint.X - fpBox.MinPoint.X

    width = fpBox.MaxPoint.Y - fpBox.MinPoint.Y

 

    Dim objUOM As UnitsOfMeasure

    Set objUOM = objpartDoc.UnitsOfMeasure

 

    Dim strLength As String

    Dim strWidth As String

 

    strLength = objUOM.GetStringFromValue(length, UnitsTypeEnum.kDefaultDisplayLengthUnits)

    strWidth = objUOM.GetStringFromValue(width, UnitsTypeEnum.kDefaultDisplayLengthUnits)

 

    Call MsgBox("Width = " + strWidth + vbCrLf + "Length = " + strLength, vbOKOnly, "Sheet Metal Flat Pattern")

 

    Call Create_ext_prop("width", strWidth)

    Call Create_ext_prop("length", strLength)

   

End Sub

 

  

Sub Create_ext_prop(prop As String, prop_value As String)

 

Dim opropsets As PropertySets

Dim opropset As PropertySet

Dim oUserPropertySet As PropertySet

 

Set opropsets = ThisApplication.ActiveDocument.PropertySets

 

For Each opropset In opropsets

    If opropset.Name = "Inventor User Defined Properties" Then Set oUserPropertySet = opropset

Next opropset

 

' If Property does not exist then add the new Property

On Error Resume Next

        Call oUserPropertySet.Add(prop_value, prop)

' Try to set the Property value if it already exists

 

 For i = 1 To oUserPropertySet.Count

   If oUserPropertySet.Item(i).Name = prop Then oUserPropertySet.Item(i).Value = prop_value

 Next i

 

End Sub

'--------------------- Cut here ---------------------------

A possible future enhancement to the code is to add  custom rules to calculate the material stock required.

You could very easily add rules similar to this one:

approximate number of parts that can be punched out of the raw plate=

<area of the raw sheet metal plate > /(length * width) 

No patience to copy & paste above macro?  You can download the code of this article here.

Unzip the .bas file and import it in your VBA project.