Display option: thread feature - off by default in Inventor 2015

[mrattray]

I've started playing around in the trial version of 2015 while I wait for my SN. I've discovered that for some reason, in the drawing environment, all views come in by default with the display option "Thread Feature" turned off. This is different from previous releases and is EXTREMELY annoying. There are times when I don't want to show threads, but that is not common.

[mdavis22569]

It seems that there is a lot more "set up" in this version .... I already changed my 2 template from Dwg default to idw... that was noticed earlier. I think they really like to keep people on their toes.

[mcgyvr]

Autodesk motto..

"Two mouse clicks are always better than one"  

pfft... who needs to see threads anyways 

[mrattray]

Also, pressing "T" for general text note in a drawing creates a sketch.

[mrattray]

Also, the parts list auto-sort functionality is a great idea, but when the BOM doesn't also auto-sort it ends up being another half implemented feature.

[mrattray]

A VBA macro that was working fine in 2015 yesterday suddenly doesn't know what a FileSystemObject type is. I made no changes to the IVB file whatsoever.

[ChrisMitchell01 · Accepted solution]

The issue with Threads not being displayed in part drawing views by default, was the result of a project to make various drawing view settings become persistent across Inventor sessions.

The default of "off" can be remedied by setting 

[HKEY_CURRENT_USER\Software\Autodesk\Inventor\RegistryVersion19.0\Applets\DrawingLayout\Preferences\DrawingFormat]
"BaseViewDefPart"=dword:01111501

After that it will be remembered. This might be useful for use in a team type situation where you want to preset/deploy this.

Other values that are now better persisted are:

1. Thread Edges

2. Interference Edges

3. Tangent Edges/Foreshortened

4. Hidden Line on/Removed View

5. Shaded View

Each of these is stored by view type, (Ortho, ISO, etc), as well as by filetype, (iam, ipt, ipn).

Regarding the issue with "T" now starting a new sketch & creating sketch based text, that seems to be an artifact of the fact that the sketch tab is now always active in 2015, in part modeling, & it seems we missed that duplicate "T" command alias - I've created a defect for further investigation & will let you know if I find a workaround.

Thanks,

Chris

[mrattray]

Thanks, Chris, much better now!
This feature would really only be useful to me if I could set different defaults for sheet metal flat pattern views versus folded views, as flat patterns are usually when I want to hide threads.

[mrattray]

It appears that export flat pattern as DXF (RMB on flat pattern node > save copy as) now no longer holds my custom ini file as the default. I never had this problem before in earlier versions.

[dan_inv09]

I've had that with every release.

You have to place a view before you can change it (and remember to delete that view before you "save as Template").

[Fori123]

Chris,

i have tried to turn on the threaded feature to on by default. is this the correct spot to make the change? i tried it once but it did not appear to save.

[mrattray]

That looks right, Fori. Here's a screen shot of mine with the new value showing the full path:

Edit: Make sure you have Inventor closed when you do this, I don't think it would be happy with you hacking the registry while it's running.

[Fori123]

i think my issue was io had the leading 0 in place. thank you for your help that worked now.

[jmlip]

Hi Chris,

How about setting the default for assemblies?  What is the dword for that?

Thanks,

Joan

[ChrisMitchell01 · Accepted solution]

Please see this article for additional info about this:

http://beinginventive.typepad.com/being-inventive/2014/06/persistent-drawing-view-options-in-2015-th...

Thanks,
Chris

[jmlip]

Thanks Chris!

[Airlake]

I'm not quite sure how to change this setting of the default thread feature. can you give it to me step by step?

[HKEY_CURRENT_USER\Software\Autodesk\Inventor\RegistryVersion19.0\Applets\DrawingLayout\Preferences\DrawingFormat]
"BaseViewDefPart"=dword:01111501

[ChrisMitchell01]

Jim,

Setting this through a registry setting is only really necessary now, if you want to roll this out as part of a larger scale deployment. If you just want to set this to be your default on your own machine, you can create a drawing & when placing a view you can go to the Display Options tab & check the box that says Thread Feature & then it will be remembered going forward.

There's quite a bit more info in http://beinginventive.typepad.com/being-inventive/2014/06/persistent-drawing-view-options-in-2015-th...

Hope this helps,
Chris

[Airlake]

Chris, i have tried this several times and it still defaults back to an unchecked box. 

i have tried to change it in the registry but mind looks like this?

[ChrisMitchell01]

Looks like you created it under HKEY_LOCAL_MACHINE instead of HKEY_CURRENT_USER\Software\Autodesk\Inventor\RegistryVersion19.0\Applets\DrawingLayout\Preferences\DrawingFormat

-Chris