Better way to create an adaptive pattern?

[Anonymous]

I need to pattern features that change slightly as I go.  Picture below explains it best.  I created an iFeature for each cut that parametrically shifts the shape based on its distance from the origin.  I had to insert the iFeature and constrain to the origin 29 times for starters.  But now I need to tweak the shape of the cut, and the features are no longer linked to anything.  My only option is to start over!  Or does anyone have a better idea / method?  Inventor 2018 has made their patterning placement more powerful ... but each instance is still identical.  Same with sketch blocks.  I need to make a pattern and have each instance evaluate an equation.  Thanks!

[johnsonshiue]

Hi! Currently, Inventor pattern does replicate the source feature. The patterened feature is the same as the source feature. I am not aware of a pattern workflow allowing you to create such adaptive pattern.

Many thanks!

[Anonymous]

OK, so no luck.  Is there a way to make the drawing adaptive?  If I could only take my current model with 30 iFeature instances and edit it (regenerate the part), it would save me much work.  Instead I have to start over each time - kind of defeats the benefits of CAD!

[johnsonshiue]

Hi! It would be wonderful if such geometry can be created easily. The geometry can be created but the workflow can be tedious. The issue here is that the so-called pattern is not even a pattern. How do you define the geometry? Is it driven by an equation? Are you aware of any tool on the market capable of doing this kind of pattern easily?

The thing is that this particular request does not seem common. You may want to add an idea to Ideas forum.

I am not sure what you meant by adaptive drawing. Inventor drawing views are associative to the model geometry.

Many thanks!

[Frederick_Law]

It could be done if you don't change number of slots.

[Anonymous]

I understand that complex pseudo-patterns are not common and not worth "automating" in Inventor. 

All I'm asking for is a way to create the model and be able to edit it without starting from scratch every time.  If I use iParts, I can edit the part file and regenerate those.  iFeatures are almost completely static as best as I can tell.  The only way I could figure out to "change" it was to delete the .IDE file, generate a new iFeature, and re-imbed it in my part.

[SBix26]

As others have said, no easy button method.  But it appears that both the top and bottom of these cuts are regular patterns, so it seems as if some automation should be possible.  I'd love to have a shot at it if you could post the part or something similar.  Also give an indication of which parameters might have to be tweaked.

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Sam B
Inventor Pro 2019.1 | Windows 7 SP1
LinkedIn

[Anonymous]

Hi Sam,
Thanks for your offer. The part is semi-proprietary and I don't feel comfortable sharing it. At this point I am changing so much geometry that I'll have to redraw from scratch. My concern is about the time after that - will I have to redraw everything AGAIN even if I'm just tweaking parameters? If there was a good way to do it, it would save me much work.
The geometry is less complex than it looks. The front is given by
Position * 1/ (front gauge)
The back is centered on
Position * 1/ (back gauge)
The rest is transitions and rounds.
I created an iFeature where I change "Position" each time I insert it. Maybe you have a better idea. I can add as many parameters to the iPart as possible so if I tweak one I only have to change 30 values, which beats redoing everything ...
Thanks again!
Patrick P.

[SBix26]

I really, really hope you're using Inventor 2018 or 2019; I produced this in 2018.  This is really labor intensive, but once it's done, it can be tweaked quite a bit (within reason).

As you can see from the browser above, I patterned the straight portions at both ends as separate patterns, then made a very complicated sketch to connect them and extruded that.  But it's nearly infinitely adjustable-- look at the user parameters for the pitch and radius numbers.  And feel free to ask questions.  But I'm not going to produce another one in a different version!

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Sam B
Inventor Pro 2019.1 | Windows 7 SP1
LinkedIn

[Anonymous]

Wow, thanks so much!  I'm using Inventor 2018 so we're good on that.  How did you generate the sketch for Extrusion 4?  Did you use any special tricks, like fancy scripting, or did you draw each arc and line segment manually? 

I should definitely be able to tweak your model to get what I need.  Just trying to see if there is anything I can learn for the future.  Thanks again!

[SBix26]

I started out just sketching arcs and lines individually, finally got smart and started copying the arcs.  But I still had to constrain each one (coincident, tangent, equal)-- lots of clicking involved.  I should have used a much smaller example, but I got stubborn!

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Sam B
Inventor Pro 2019.1 | Windows 7 SP1
LinkedIn

[Anonymous · Accepted solution]

Thanks again for your help.  If I may summarize for others reading this:

If possible, work within the regular part environment (pattern, sketch, extrude). 

You can draw sketch fragments (lines, arcs, constraints, dimensions) and copy-paste them within a sketch.  Nice trick to replicate features that are similar but not identical. 

Stay away from iFeatures unless you know the features will never change.  The iFeature functionality is extremely limited at this point (as of Inventor 2018).