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
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 )
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 )
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.
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.
The Final result will look like this:
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‘.
Paul,
When you get the “0” dim for the foreshortened arc length…. you are picking the arc rather than a point on the arc reference point.
Watch this clip…http://screencast.com/t/IabpUtITOZA
Cheers,
Kirk
Hi Kirk,
Thank you so much for clarifying this!
People – watch Kirk’s screencast!
Paul
This strays a little away from the intent of the original piece, but it still relates to arc length, so here goes:
I have a view of a cylindrical tank and have an accessory welded onto it at 18 degrees down from the horizontal center. I was hoping I could add an arc length dimension from center by selecting the horizontal center, the centerline of the accessory (which would give angle) and then the outside of the cylinder (which would give radius), but that doesn’t work.
Is there any way to show arc length dimensions of portions of a circle (as above) by using intersecting lines or similar? I don’t want to have to create an extra arc somehow just to get an arc length.
In case you’re wondering, the guys building the tank find it much easier to just grab a tape measure and measure down from center (or the edge of another feature), so it’s easiest way for me to communicate placement instead of using angles and radii.
Hi Chris,
I totally get where you are coming from about giving the guys the dimension they need, rather than the only dimension you can give them!
I had an experiment. By selecting both axis and right clicking I got the ‘Arc length foreshortened’ dimension type. Unfortunately this give me a 0 measurement :/
try it out and see if it works for you.
if not, I am afraid that you will either have to split the surface to get something to dimension to, or create a sketch over the top of your view…
Paul
Is there a way to display arc length symbol in annotated text?
Hi there,
You can display any symbol you can find with the windows character map This may vary depending on which font you use).
With Arial Font ‘Combining Inverted double breve’ seems to be the one you want – ͡͡
Here’s a good post:
http://forums.autodesk.com/t5/inventor-general-discussion/general-table-question/m-p/2932742
And here is the ALT code:
http://www.fileformat.info/info/unicode/char/1dfc/index.htm
Does that help?
Paul
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
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…