How to Measure, Dimension and Specify Arc Length In Inventor Sketches.

By default Autodesk Inventor will dimension the Radius of an Arc in a sketch. So how do you find the Length of the Arc? And what if you want to specify the Arc Length to drive your sketch?

Measuring the length of an Arc in an Inventor Sketch is easy. Just use the ‘Measure Loop’ tool.

Inspect Tab > Measure Panel > Loop

Measuring a sketched Arc with Inventors Loop tool

 

 

But this won’t allow you to use the Arc’s length in Parameter’s and Formula’s.

A Parametric Arc Length?

Unfortunately Inventor doesn’t have an ‘Arc Length’ type of Dimension Parameter in sketches. But it is pretty easy to grab the length of an Arc using a Formula.

To Get the Length of an Arc

To get the Length of an Arc to use in your Equations you will need:

  • A Model Parameter for the Included Angle of the arc - Angle
  • A Model Parameter for the Radius of the arc - Radius
  • A user Parameter for the Arc Length - Arc Length
  • A User Parameter to convert Degrees into Radians – Radians

The Formula is:
Radius * ( Radians / 1 rad )
Finding an Arc's Length In Autodesk Inventor with a Parameter

 

To Drive the Length of an Arc

To drive the Length of an Arc you will need:

  • A Model Parameter for the Included Angle of the arc – Angle
  • A Model Parameter for the Radius of the arc – Radius
  • A user Parameter for the Arc Length - Arc Length

The Formula is:
ArcLength * 180 deg / ( Angle * PI )

Driving an Arc's Length In Autodesk Inventor with a Parameter

Visual Feedback

If you want visual feedback of the Length of the Arc you could add some sketch text, and pull in the Value you are looking for.

Adding an Arc's Length in Autodesk Inventor with Sketch Text

 

Annotating an Arc’s length in an Inventor drawing

You can add a dimension annotation in an Inventor drawing to give the length of your arc using the ‘General Dimension’ tool.

Annotate tab > Dimension Panel > Dimension Tool

Inventor will automatically pick the radius of the Arc. Just right click to get the ‘Length’ option.

Annotating an arc in an Autodesk Inventor Drawing File

The Final result will look like this:

Dimensioning an arc in an Autodesk Inventor Drawing File

 

I hope that you enjoyed this sketching tip!

Read this post to find out my Top Tip for creating Inventor sketches ‘Sketching – Keep it simple‘.

 

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Comments

  1. Inventorexpert says

    how dumb is that, it has the ability to give you the dimension in a drawing but not the ability to give you the exact same thing in a sketch. impressive inventor

    • says

      I have to agree. Arc dimensioning seems like an easily solvable oversight. I would love to hear from the Inventor team why this has never been added to the package…