Dimension Belt length in IDW

[Retselnitram]

Is there anyway I could dimension the length of a belt in IDW?

For conveyors I would like to dimension the length of the belt.

I can measure a loop in a part file but can't find away to do it in IDW.

[-niels-]

Not sure how exactly you want to dimension your belt, but maybe you're looking for the "arc length" function?

(right-click after selecting the arc, but before placing it.)

[Retselnitram]

Thanks For the reply.

This only measures the length of the arce.

I was hoping for a single dimension for the length of the belt. Like measure length of loop.

[coreyparks]

Take a look at the atached file sand see if this will work for you.  I dimensioned the length of all the arcs and lines on the belt pitch then added them together in a user parameter called belt length.  In the IDW create a leader an point to the belt then insert the user parameter called belt length.  This way it stays parametric and you could create a template already setup this way for your belts.

[Retselnitram]

Thanks

That might be what I have to do.

Hoping for a single click dimension but I guess not.

[Cadmanto]

If you are looking for a one stop shop when it comes to dimensioning a belt, it does not exist.  Best option is what has been outlined above.

Feel free to submit an idea to add this to the software here.  Inventor IdeaStation

If this solved your issue please mark this posting "Accept as Solution".

Or if you like something that was said and it was helpful, Kudos are appreciated. Thanks!!!! 

     

[mdavis22569]

For my belt conveyors ...when I need to measure, I save the IDW down to a Inventor dwg or Autocad dwg and click List for the properties of the belt ...and I get my length

[mcgyvr]

hmm.. I would have simply picked from an ipart in the assembly when placing the belt that has the length already defined and have a parts list showing a "200" x 12" wide belt" or whatever it is.

I wouldn't need to dimension the belt at all in the idw. 🙂 

[johnsonshiue]

Hi! Is the belt itself a part? If yes, does it have uniform thickness (cross-section)? I am wondering if you could use a leader text referencing the value of volume divided by cross-section area. In theory, it should be the length of the belt, right?

Thanks!

[Retselnitram]

I thought this was a great idea until I tried to do it.

I can get the volume but I can't get it to Divid in the leader command. Then I tried in the parameters to set up a user parameter but can't get the volume there.

And being this conveyor usually has a 3 or 4 rollers this would have work reasonalbly well.

[coreyparks]

This gives you the width of the belt not the length.

[Retselnitram]

I will give you the length.

The volume of a piece of belting 1/4" thick x 24" wide x 100" long has a volume of 600 cubic inches

volume / (thickness x width) = length

600 / (.250x24)= 600

[johnsonshiue]

Hi! I am sorry to provide a solution without much detail. Actually it is doable via iLogic. What release of Inventor are you using? I can provide a simple example for you to follow.

Thanks!

[Retselnitram]

Inventor 2015

Would be greatly appreciated

Thanks

[johnsonshiue]

Hi! Attached is a simple example of the workflow I talked about earlier. The trick is to capture "volume" in an iLogic rule, triggered by any geometry change. Then create a user parameter to equate to "volume" divided by cross-section area. Next, create a drawing view of the part and a leader text pointing to the part with user parameter shown as value.

Let me know if you have any question.

Thanks!