Loop measurement

[mohamed.abichou]

Hi,

I have a question in the drawings to measure the full curve length is that possible?

Since it can be done with the loop function in the 3D sketch i was wondering if it can be done in drawings also or maybe there is another method if anyone knows please let me know.

Thanks in advance.

[Murat.Sözen]

You can just measure 3d sketch curve , if you make visible it you can measure. If you want to measure near curves you should measure and addition each one by one.But it will not get the right result. For example in my part , right side curve lenght is wrong i think.

[johnsonshiue · Accepted solution]

Hi! The loop measurement is not available within drawing environment. In modeling environment, you can simply select an edge or a piece of sketch geometry -> right-click -> Select Other -> Loop. You don't need to create a 3D Sketch.

Many thanks!

[phlyx]

We have a similar situation.  We created a surface body by extruding a single line sketch representing a material flow path. 

We needed to know the total length of this and we could not find any way to easily do this.  Looked like we had to find the length of every segment and add them together.... with our abacus?  😕

So instead we made a quick drawing, inserted a view of the item and saved it as an AutoCAD drawing.  Then in AutoCAD we turned it into a polyline (PE and then Join) and then did a LIst and we can get this much information:

Feel a little silly that lil' ol' 2D AutoCAD can whip this information out super quick but Inventor didn't offer a way to do this.  Are we missing something or is this true that Inventor falls short of what AutoCAD can do with this?

[gmwi]

Use measure perimeter of the face and divide by 2.

[phlyx]

There is no perimeter, the extrusion is done on a single line so it is just a surface with no depth to have a perimeter on.  A 2D flat surface following a path.

[gmwi]

Sorry about that. Use your original

 

sketch to get the total length.

[phlyx]

This is the model, saying use the sketch doesn't say "how" to use the sketch.  🙄  When I select Measure it only selects one edge at a time.  If I edit the sketch, highlight the whole thing and pick measure it unselects it.  If I am in the part and select the sketch and then hit measure it unselects it.  

[gmwi]

It should look sumpt'n like this. If you don't have starting sketch then make one with projection.

 

[phlyx]

When I am in the original sketch, if I highlight the entire sketch and hit measure, it un-highlights the sketch and I can only select things one piece of sketch at a time, not the whole thing.   We only have the measure command on the tools tab.  Seeing the final result of what you did doesn't help us get there without knowing "how" you got there as we seem to be missing something.  Can you please post step-by-step of how you got to the thing you screen captured?  

[phlyx]

Also, AutoCAD on the original sketch says the length is 974.7926mm but what you screen captured shows the length is 1007.451. That's over 32mm different. I honestly trust AutoCAD over Inventor for this one.

[gmwi]

You can use either the origin plane or create a plane. Then either use "projection cut" or "projection" of the edge depending on which plane you use. I get the same measurement in Autocad.

 

 

[jonSYAXG]

EDIT-This is not relevant to the original question about measuring in drawings. This solution is for modeling mode. apologies.

Jumping in here - as I was just trying to learn the same thing (if I interpret this convo correctly)

It seems that opening the 2d sketch to edit lets you get this info.

Steps-

1) Edit 2d sketch that you have drawn

2) start a measurement (press "m"?)

3) hover over an element of the path and wait for much longer than you would think (like 1 sec +).

4) use the drop down menu that appears to select "curve loop". Then you get the total length of the connected path.

Not sure why it's so well hidden, but there you go.

[phlyx]

Thanks and here's the real problem.  I have always hated having the "select other" pop up by itself so I have that set to "Off" so on the super rare occasion I want to pick something else, I RMB and pick something else from the popup menu. 

When you have that set to "Off", the popup menu for the measure loop never pops up no matter how long you wait.  And if you RMB and click on "Select other" then you can pick "Curve loop".  Did not know that "Select other" was where the measure loop option was hiding.

And thanks @jonSYAXG, very glad to have someone reply with a step by step method of doing that.  Posting a picture of a properly rebuilt carburetor doesn't tell someone how to rebuild a carburetor (for anyone old enough to even know what a carburetor is)   😁

[gmwi]

Please review your technique for using Autocad. This forum is not the place for Autocad tutorial.

[SBix26]

Something you may not have known/remembered: Select Other can be invoked by the keyboard combo Ctrl-A.

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Sam B

Inventor Pro 2023 | Windows 10 Home 21H2