Curve Loop Dimension

[iUser]

Would save a lot of time if we could have a curve loop dimension in the sketch environment. My current work around is giving each line / arc a length dimension and adding them in the parameter table to give you a total length. We constantly use this for conveyor belt, chain length etc. and I am sure we are not the only company having to do this. We require these lengths so that we can order the correct length material and this dimension needs to update as the model changes. I am aware that you can measure the loop, but that can cause problems if you manually enter a total length and the model changes at a later stage.

This is what its should look like:

Belt ShetchProposed Loop Dimension

This is my current work around:

Give each line/arc a length dimensionAdd all parameters together for total length

[jtylerbc]

If the length is the resultant of the other dimensions (rather than driving the sketch), there might be a better option for you using existing tools.

In iLogic, you can measure the perimeter of a sketch, and set your Length parameter equal to the result.  You could then set that rule to run every time a parameter changes.  This would take only a single line of iLogic code to do.

Length = Measure.Perimeter("Sketch1")

This would get you results very similar to what you are doing now, but much more easily (no need to write an equation to sum up all of the dimensions).  It's also much more forgiving to model changes, since it doesn't care if a dimension gets added or deleted.  You might get some weirdness if you had multiple closed boundaries in the same sketch, but that doesn't seem to be the case for you.  (Technically you do have multiple boundaries, but they are separated by construction lines, which the code ignores.  So it's no problem for your example)

However, even while suggesting a current-tool workaround for your application, I see other possible usesfor the idea.  I have created some models where the total length was a user-supplied value.  Other dimensions in the sketch were user-entered, and there was a formula to figure out the leftover length.  Think of a rope wrapping over a pulley - the user supplies the total length and the pulley diameter, and the formula figures out the remaining straight lengths.  Your idea would be a great way to deal with situations like that.

[CMyers]

I have situations similar to iUser.  It would be helpful if the user could get what Inventor calls "curve loop length" in the sketch environment without having to put on their programmer hat and create an equation manually or create an equation(s) in parameters to do something the software is clearly capable of returning already. 

I used to use a different CAD package the allowed the user to create a parametric sketch dimension of the "curve loop length"  (program was Creo, parameter is "perimeter").  The user could then put in other dimensions and constraints to define the path, make select dimensions "driven" and, if the "loop length" is driving, when a parameter changed (such as the distance between pulleys) the driven dimension(s) were updated automatically to keep the desired "curve loop length".  This would be a valuable tool in Inventor when considering a belt of a fixed length and trying to optimize pulley positions.

I have been doing the same work-around that iUser has been doing, and having a second curve with another parameter equation for that length, then yet another to calculate the difference and I manually adjust the dimension of choice to try to bring the difference to zero.  This is math that could be automated for the user, and not require iLogic programming to extract it.  Inventor has already defined rules for the "curve loop length", driven and driving dimensions and constraints.  Would it really be that much of a stretch to allow "curve loop length" to be put in as a dimension, give us the option to make it driving or driven, and allow us to manage constraints and dimensions to achieve a design requirement with a constant curve loop length?