Automated view annotation - styles for sheet metal extents not supported?

[christian.mcdonald]

Just a quick question about the styles editor feature in inventor.  I would like to automate my view preferences annotation text so that it shows sheet metal extents length, width and thickness automatically when I place a base view.  I know this is able to be done directly by selecting the base view on the drawing sheet and clicking the edit view label button - then Type = Sheet Metal Properties - Property = FLAT PATTERN EXTENTS LENGTH.  This feature does not seem to be available in the styles editor..Could you help me out?

[cadman777]

I realize this is a bit late, but I just figured out how to do this yesterday.

Here's what I do to get the sheet metal properties into the Flat Pattern View Label:

1. Create a custom iprop in the ipt file, in "iProperties" "Custom" tab.

For thickness, I use "G_T" (= Autodesk's own "geometric thickness" label).

2. In the "IProperties" dialogue box, "Summay" tab, create a "Parameters" expression in the "COMMENT" field.

For thickness I use "=<G_T> THK", which shows up in my View Label as "1/4 THK" (or whatever the thickness value is).

3. Now create a Style in the idw file:

In the "Style and Standard Manager", pick a "Standard", and go to the "View Preferences" tab.

In "View Type", go to "Base", and click on the pencil icon to the right of the "Display".

In that dialogue box, under "Type" dropdown box, pick "Properties - Model"

Under "Properties" drop-down, pick "COMMENTS".

In the area where you type, put your cursor where you want this iProp to appear, and then click on the "X" (= "Add Text Parameter"), to add "COMMENTS" to your text box.

Then click on "OK" at btm right of the dialogue box, and Save that "Style", closing out the "Style and Standard Manager".

4. Make sure this new Style is selected as the Standard when placing flat patterns.

5. Now make a view of a part that is a "Flat Pattern".

You should see the flat pattern extents value for thickness show up in the view label.

You may be able to use other ipt "iProperty" fields to do this.

I would use iProperties in the ipt file that are unused on a regular basis in your job, and that you are certain will never be used.

I used "COMMENTS" this time around as a test-run to see if this would work for me.

I'm sure glad it does!

Now, if only I can find a way to make a part's total quantity (for a given assembly) show up in the view label w/o using "iLogic".

[wrw0007]

Sorry to bring this up multiple years later. Seems Adesk still hasn't figured this one out.

First of all... Thank you!

Secondly, I am using this to display plate thickness values. The way that I am doing it is to rename a model paramenter. For example taking dimension d4 and entering "THK=3/8"

I am then inputting in the comments: "=<THK>"

What I'm running into is that the display on the view label shows in decimal rather than fraction. How can I change this? It's not a "problem" per se, but clashes with the rest of the style.

Has there been any updates in regards to this on AutoDesk's side? I'm on 2020.

[wrw0007]

In regards to my last post. I found that if I go into the model parameters I can right click and select "custom property format" and change to fractional.