Measure sweep path (Inventor 2021)

[steveh5]

Gang...long time user of Inventor.

Why do I struggle with measuring a sweep length every time I attempt to to do this in 2021?

Used to be kind of straight forward in prior versions (at least way better than it is now).

So, how do I get this length of path?

Best,

Steve H.

[JDMather]

If you Include Geometry into a 3D Sketch does it give you the length.

[steveh5]

@JDMather ..

Thanks JD for the quick response, but not sure what you mean.

I attached the file with the path.

Best,

Steve H.

[JDMather]

My memory was faulty...

Temporarily convert the construction line to object line.

Go to Region Properties and Calculate the Perimeter.

Subtract the 12".

Alternatively - 

close the sketch (construction to object line) and create a Patch.

Use the desired edges of the Patch as the Sweep Path.

Measure the Patch and subtract the 12" from the Perimeter...

I might model the part a bit differently...

[swalton]

Some years ago a kind person provided the attached iLogic code.  As I recall, the name of the sweep feature or the sketch has to match the one referenced in the code.

'Set a reference to the active part document
Dim oDoc As PartDocument
oDoc = ThisApplication.ActiveDocument

Dim oDef As PartComponentDefinition
oDef = oDoc.ComponentDefinition

Dim opath As Path
opath = oDef.Features.SweepFeatures.Item("TheSweep").Path

Dim TotalLength As Double
TotalLength = 0

Dim oCurve As Object
Dim i As Integer

For i = 1 To opath.Count
oCurve = opath.Item(i).Curve

Dim oCurveEval As CurveEvaluator
oCurveEval = oCurve.Evaluator

Dim MinParam As Double
Dim MaxParam As Double
Dim length As Double

Call oCurveEval.GetParamExtents(MinParam, MaxParam)
Call oCurveEval.GetLengthAtParam(MinParam, MaxParam, length)

TotalLength = TotalLength + length
Next i

Dim oparams As Parameters
Dim oparam As Parameter
oparams = oDoc.ComponentDefinition.Parameters
Dim exists As Boolean
exists = False

'Find out if parameter exists
For Each oparam In oparams
If oparam.Name = "Sweeplength" Then exists = True
Next oparam

'Change the value if the parameter exists otherwise add the parameter
If exists Then
oparams.Item("Sweeplength").Value = TotalLength
Else
oparams.UserParameters.AddByValue( "Sweeplength", TotalLength, 11266)
End If
oDoc.Update

Here are some more ilogic methods:

https://forums.autodesk.com/t5/inventor-forum/sweep-length-measurement/m-p/9567405#M791937

[johnsonshiue]

Hi Folks,

There is no need to use any workaround for this task. Start Measure tool. Right-click on the path -> Select Other -> Curve Loop. You will get the loop length. On 2017 or earlier, there was a dedicated Measure Loop command. On 2018 and later, it is combined in the same Measure command.

Many thanks!

[JDMather]

---

@johnsonshiue wrote:

…On 2018 and later, it is combined in the same Measure command.

---

…it was hidden…

@johnsonshiue 

Perhaps return to (more) easily discoverable. As in, hard to miss it.

[steveh5 · Accepted solution]

So...this is how you do it in 2018 and beyond. Initiate the Measure Tool and hover over one of the segments to get the "Select Other" dialog to pop up and scroll till you see "Curve Loop".

And....a quick video...

https://autode.sk/3kY4eJ0

HTH,

Steve Hilvers

[cadman777]

If it isn't a spline and it is subject to change during the design cycle, I place driven dimensions on each segment and then add them up in the Parameters dialog. That way the result can update when the loop changes. That's how I typically established the lengths for the BOM with railing made from bent pipe.

Otherwise, wish I had @swalton's iLogic rule in the past when I needed to measure splines!

[Tom.DiGregorio2DPCZ6]

I have a sweep comprised of multiple 2D sketches, Why wont inventor tell me the length the whole thing or of any one segment?

[johnsonshiue]

Hi Tom,

You could measure the path (enable loop selection) individually and add them up. Or the quickest way is to find the volume from physical iProperty and the divide it by the sweep profile area. It should be the length of the entire path.

Many thanks!