Sheet Metal iFeature with Circular Pattern Unable to Save

[clamhaich]

Hi All,

I am running into an error when I try to extract an iFeature of the attached part. It appears to be the circular patterns which are causing the issue, and to be honest I am not sure why.

The iFeature is intended to be table driven, and part of that is altering the number of cuts in several of the patterns, so I am hoping to keep them in the iFeature (rather than creating multiple iFeatures with different numbers of occurences in the patterns) so as to reduce the number of possible punches which our users can choose from (thereby reducing the chance of a user error)

Any assistance on this would be much appreciated

[CGBenner]

@clamhaich 

Hello and welcome to the forum.

Are you trying to extract all of these holes as your iFeature?  I'm not sure that is possible.  Does anyone have any suggestions?

[clamhaich]

Hi @CGBenner,

Yes I am trying to extract all of the holes 🙂

We currently have 17 different punch tools in Inventor which I am trying to consolidate into a single tool, and each of them has the same number of holes except for the ones in the circular patterns.

Current solution I am tending towards is having the maximum number of holes that will be used, with a construction line from them to the point of rotation, and using a "Hole_Qty" parameter to give the angle between them (360 deg / Hole_Qty). This results in overlapping holes when I have for example 6 holes out of a total possible 20

[CGBenner]

@clamhaich 

In a very quick test with your part, I was able to get the "Save" button to activate as a standard iFeature, but as soon as I try to use the same geometry selection for a Sheet Metal iFeature, it greys out.  

@johnsonshiue do you know who could take a look at this?  Is this not possible with the Sheet Metal iFeature?

[johnsonshiue]

Hi! It looks like a bug to me. I don't have a good explanation. I need to work with the project team to understand it better.

Many thanks!

[kacper.suchomski]

Hi

I think it's easiest to create an iFeature for one hole and manage the pattern at the model level.

[clamhaich]

Hi @kacper.suchomski 

In an ideal world we would not need the iFeature for anything except the spacing and position of the 3 x 12 mm dia and 1 x 6.8 mm hole, but unfortunately we have had issues in our factory where holes are missed due to people referencing previous units of ours which are either outdated or significantly different in the quantity or size of the smaller holes

Some context for what this iFeature is trying to achieve:

We purchase in a large variety of fansets manufactured by different companies, and those fansets have a ring around them for mounting to sheetmetal plates. The fixing hole diameters and PCD varies depending on 1) the code of the fanset and 2) the orientation of the fanset

So the iFeature is trying to provide the cutout for the airflow, the fixing diameters and position, and additional cutouts for the fanguard

The working solution I have at the moment is having the position of the fixing holes on construction line "spokes" from the center point, and varying the angle between the spokes.. end result looks correct but does have holes directly on top of each other when the number of fixing holes is less than the maximum

[johnsonshiue · Accepted solution]

Hi! I have checked with the project team. Unfortunately, it is a limitation in Punch Tool. Because of the need to snap to a sketch point, the ability to select an axis in Punch extraction workflow is disabled (it is fine in an iFeature).

Many thanks!

[clamhaich]

Ah, not what I was hoping to hear, but we work with the tools available

I'll mark this as answered, thanks for looking into it