Inventor: Make a circular pattern for a sheet metal cut be a closed loop?

[llorden4]

I've known for some time that making patterns for features is far more stable than making patterns within a sketch.  I've finally come across a situation where I've got to create the pattern in the sketch.  I need to make a cut with a polygonal shape that varies with size, number of sides, starting angle, and degree of tilt.  As I'm using this as a template for use with automation, I also need to be able to rely on the part to self-manage and avoid the various tasks such as the wizards to go through and manually select all the edges to force a closed loop.  Surely there's a process by now that'll accommodate such a need?

Can't pattern the "Cut Feature" because it only patterns the "result" and not the cutting tool.

Creating sketch patterns on floating planes & axis is far more effective if I can just get a closed loop.

     

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@llorden4,

marius.gildehaus has edited your subject line for clarity
Original: Re: How to make a circular pattern be a closed loop?

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[TheCADWhisperer]

No file Attached?

[llorden4]

My file is full of propriety algorithms and I'm unable to share.  I figure anyone unable to create a simple sketch circular pattern is probably not going to be able to help me anyway.  The photo's are simply to satisfy the usual first response of "why did you do it that way?"

[TheCADWhisperer]

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@llorden4 wrote:

Can't pattern the "Cut Feature" because it only patterns the "result" and not the cutting tool.     

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Sounds like a simple Adjust issue.

Too bad you can't model a simple mock-up that exhibits the behavior of your proprietary data.

[marius.gildehaus]

Hello @llorden4!

Pleave provide a sample dataset, can also be a simplified one, in which we can see what you want to achieve. Maybe we can even find a better solution then doing it with a sketch pattern.

Thanks!

[llorden4]

The test file, looking for a solution on creating a closed sketch pattern.

[kelly.young · Accepted solution]

Hello @llorden4 instead of patterning within the sketch could you utilize the single shape and then pattern the Extrude Cut based on your Sides parameter? It helps simplify the pattern and doesn't need to identify closing loops.

Not sure why you need the pattern inside the sketch as opposed to outside, see if the screencast helps.

Please select the Accept as Solution button if a post solves your issue or answers your question.

[johnsonshiue]

Hi! This behavior is related to how Inventor recognize a profile from sketch geometry. The process currently is based on constraints. To "connect" two lines, you will need coincident constraint between end points. The issue here is that the patterned sketch does not allow inter-occurrence constraints. So, you end up with 6 separate lines, although you clearly have the intent to make is a hexagon. We are working on a solution to recognize this profile as a hexagon. But, it will not be available on existing release. If you are interested, you can sign up Inventor Beta to try it.

In the meantime, you can use Boundary Patch command and select the 6 lines to create a patch surface. Then create a sketch on the same plane and project the edges. The workflow is awkward for sure. But, it should work more reliably.

Many thanks!

[llorden4]

This is the method I attempted to start but failed to get this result.  The main difference in operations between us was that I used the sheet metal cut feature vs extruding as a cut solid as you did in this video.