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    By Luke Davenport

    A customer had this question recently:

    I have a flat circular ring, with concentric grooves on the top surface. The grooves are equally spaced and have the same profile, but are different diameters. I want to be able to resize this ring parametrically. What do you think?

    Well my thoughts went something like this:

    • Can you just show the grooves as a decal, not actually machine them? No, they need to be machined.
    • Can you model ALL of the grooves, and then just suppress/activate the ones you need with iLogic? No - There could be 100+ grooves and that will make for a cumbersome model.
    • Circular pattern of a feature – will that work? No.
    • Rectangular pattern of a feature – will that work? No.
    • Rectangular pattern of a sketch block, and then revolve all the profiles – will that work? Almost, but when the diameter changes you’d have to re-select each block profile for the revolve feature.

    It’s actually a bit of a trickier problem than it seems initially (unless I’ve missed something obvious – which is more than possible!)

    But thinking more about thought number 5 above; if we had some iLogic to automatically update the revolved feature with ALL of the sketch block profiles every time the diameter changes? That would work.

    So I got to work. Here’s the sketch with a single groove drawn. As you can see the important parameters are renamed to help me out later….

    (also important to make the centreline a ‘Centreline’ line type)

    Rectangular patterning these sketch lines gives this. I’ve used the parameter ‘GrooveQTY’ for the pattern quantity, and ‘GrooveWidth’ + ‘GrooveSpacing’ for the pattern spacing.

    Then I created a user parameter called ‘OD’ and gave it a sensible value like 80mm.

    Then I can use this iLogic rule to control the quantity of sketch blocks in the sketch pattern. 

    GrooveQTY = Ceil(((OD-ID)/2)/(GrooveSpacing+GrooveWidth)) -1

    RuleParametersOutput()

    InventorVb.DocumentUpdate()

    Then I can revolve all the current profiles in the sketch

    Nothing fancy up to this point. If I adjust the ID, OD, GrooveWidth or GrooveSpacing parameters, the sketch will update. But the revolve feature won’t pick up on the extra patterned blocks…. Hmmmm…

    So this iLogic rule will help us out. It does the following:

    • Updates the feature called ‘Revolution1’ to use all of the sketch profiles found in the first sketch in the part.
    • That’s it!

    So now if we change any of our 4 important parameters, the profiles for ‘Revolution1’ are recalculated.

    Job done!

    You can download the Inventor part HERE

    Note: It’s an Inventor 2016 part - you’ll need to download the code below instead if you haven’t upgraded to 2016 yet.

    Also Note: If you’re using this part you’ll need to have the outside diameter trimmed or extended to the actual OD value you enter. At the moment the OD can’t be finely adjusted, as it’s based off the sketch pattern. You’ll just need a simple extra extrude feature to ‘chop’ off the outside of the ring or add a bit on if the outer diameter doesn’t exactly match the groove qty. Makes sense?

    Here’s a quick video of the model in action. It’s a resizable ring! Wooohooo!