iLogic for Sheet Metal Gusset Suppression in Flat Pattern

[janelson33]

The wonderful @Anonymous has created an add-in for the sheet metal environment that allows gussets to be inserted into sheet metal parts relatively easy. The main concern, which I know Tri was trying to work on whenever he could, is that they cannot work with flat pattern models yet.

I'm thinking iLogic can help me instead, but I'm not 100% sure. If I have a set of features in the folded model that I wish to suppress in the flat pattern, is that possible with iLogic? Where do I figure out how to do this if coding is not my forte?

[blandb]

Can you post a part to see what you are dealing with? There are feature suppression snippets in iLogic you can use to suppress features.

[janelson33]

Here's a pic of the gusset in question; and it's file. Idk if you'll need Tri's add-in installed either.

[GeorgK]

iLogic:

Feature.IsActive("Round Gusset1 - Solid") = False
Feature.IsActive("Round Gusset1 - CutBend1") = False
Feature.IsActive("Round Gusset1 - Cut") = False
Feature.IsActive("Round Gusset1 - Fillet") = False

[janelson33]

@GeorgK That worked for feature suppression, thanks for that! Can iLogic, in general, work for only suppressing those features for the flat pattern specifically?

[Curtis_Waguespack]

Hi @janelson33 ,

If you're needing the flat pattern to be on a drawing view at the same time as the folder view, then there is not a good solution (although it might be able to be done with a bit of a messy workflow).

But if you're looking to export a DXF of the flat pattern, then you can suppress the features, save out the DXF flat pattern, and unsuppress the features, quite easily.

Which do you need? just a DXF of the flat pattern, or a view of the flat pattern on a drawing?

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[janelson33]

@Curtis_Waguespack I figured I might be asking for something that can't be done haha, I have a habit of things like that for this software.

I am indeed looking to use it for drawing views.

Since I use iProps to auto-fill most of my title block (part number, revision, material, finish, etc.) I just have to make sure I input the part number that is correct first. Once I do that, then I can make a workaround part that will be used for the folded model views that show the gusset.

It just sucks taking extra time because this really isn't that new of a thing and should be supported this far along into Inventor.

[Curtis_Waguespack]

Hi @janelson33 

Well it can be done, it's just a messy process.

• First move the End of Part (EOP) marker  above the feature called "Round Gusset1 - Solid"
• Then create a drawing and make a flat pattern view, it will be shown without the gusset
• Return to the part file and right click on the Flat Pattern in the browser and choose "Defer Update"
• Then in the Folded model move the EOP marker back to the end of the part. 
• In the drawing create a view of the folded model (ignore the message about the flat pattern)

Now you will have a view of the flat pattern without the gusset and a view of the folder model with the gusset. 

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com