topic Re: ViewCube orientation on document create - Application Options revert back in Inventor Forum

ViewCube orientation on document create - Application Options revert back

Anonymous — Thu, 22 Sep 2016 20:49:48 GMT

Having some trouble understanding what is going on here. We needed to change the direction our assemblies/parts are oriented relative to XYZ. We were easily able to do this by setting the Front view and Home view in the template files to their proper orientations. The issue though, is that when creating a new document from these templates, XYZ is oriented correctly respective to the Front/Top planes, but the actual view starts out with the "old" View Cube orientation. You have to hit Home in order to get it be where you would normally expect it to be by default.

So the next area I looked at was the View Cube settings in Application Options. I set those thinking that would change how the model was oriented when first created. The thing is, once I apply the application options, and create a new document, the View Cube settings revert back to default settings. Anyone know what I'm missing here?

Re: ViewCube orientation on document create - Application Options revert back

blair — Thu, 22 Sep 2016 22:30:21 GMT

The "View Cube" only control the view orientation and not the Origin Axis.

In parts you can use the "Move-Body" command which will allow for re-orientation of the Origin Axis. For IAM files, it's best to unground your primary part and constrain it to the correct axis (the rest of the IAM will then follow the primary and re-align (assuming no other parts are grounded).

Really does it mater if the part isn't correctly aligned to any given axis, since you can orient the item when you place it in a drawing view.

Re: ViewCube orientation on document create - Application Options revert back

Anonymous — Fri, 23 Sep 2016 16:09:34 GMT

It has less to do with the drawing and more with how the models are oriented when transferring models to other clients/vendors. Some industries have standardized on how their coordinate systems are and so the expectation is that when STEP or any 3D cad models are exchanged, they are in the correct/expected coordinate system. For example aircraft coordinate system:

Re: ViewCube orientation on document create - Application Options revert back

Curtis_W — Fri, 23 Sep 2016 17:04:41 GMT

Hi bbuck,

I would expect that Application Options setting to persist as well. Can you confirm that it just this setting that is not sticking, or is it any change to the application options settings?

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

Re: ViewCube orientation on document create - Application Options revert back

Anonymous — Mon, 03 Oct 2016 16:57:58 GMT

Following up on this. Correct, the application option does not seem to persist. However, I'm getting conflicting information on what that setting does. I'm told this doesn't control what it is I'm trying to do. ~~I've tried to find in the registry but can't seem to pinpoint where exactly this option is controlled. Best I've been able to find is where the "Display" settings are located:~~

Update: Looks like these might be the registry keys that control this. So I may tinker a bit with these and see if that is what is going on:

Also, it appears that the axis listed in parentheses corresponds to the value in the registry key, in the format of x,y,z with negative values denoting negative axis direction:

Re: ViewCube orientation on document create - Application Options revert back

blair — Mon, 03 Oct 2016 17:08:54 GMT

You are looking to two completely different items.

The view-cube only controls the view orientation and has nothing to do with the Model Axis.

For a single part, you can use the Move Body command to correctly position the Model Triad Axis. For assemblies you will need to unground and reposition the parts in their correct orientation to the Axis Triad.

You could quickly position the items into a new IAM file and have them correctly positioned in this new IAM to their proper orientation.

Re: ViewCube orientation on document create - Application Options revert back

Curtis_W — Mon, 03 Oct 2016 19:38:23 GMT

Hi bbuck,

I think there is some confusion here. I'm not sure which points are being asked about, but I'll try to clarify:

Both the application option and view cube option called Default ViewCube Orientation are the same setting, there are just 2 ways to access it.
Default ViewCube Orientation , accessed by either methods should persist when you restart Inventor.
The Default ViewCube Orientation setting controls the default Front and Top views , not the initial view* . And this is only for the base template, not your custom templates. The base template is accessed by holding the CTRL + SHIFT keys and clicking the New file button, and then choosing part, assembly, etc.
To redefine the view in your custom templates, you select a face on the view cube that you want to be the Front (or Top) and then right click on the ViewCube and choose "Set Current View as..."
As far as I can tell the Front view, however it is defined will always be on the left side of the cube when we look at the Home view. I don't know of a way to control that.
When you start a new model from a template (any template), the initial view* will always be looking at YX (+Z), regardless of the template's view cube default for the Front and Top orientations. I don't know of a way to control that.
As blair mentioned, nothing in these settings controls the way the axes are defined, they only control how your model is viewed.

Someone can correct me on any of these points (particularly 5 & 6 ) if I've missed something.

* "initial view" being the first view orientation when a new model is created from template

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

Re: ViewCube orientation on document create - Application Options revert back

Anonymous — Tue, 04 Oct 2016 18:04:09 GMT

Thank you both for the clarification and insight. I was wondering then if there was a way to have the part template file invoke the ViewCube Home command upon opening through iLogic. In this example posted online it appears that they have (invoke ViewCube commands through iLogic), however when I recreate the code he's written I get errors.

Re: ViewCube orientation on document create - Application Options revert back

blair — Tue, 04 Oct 2016 18:21:37 GMT

If you set your default views in the view cube with the orientation required, then use the "Save as Template" your settings will be there each time the template is used.

You can have a number of templates with different settings.

Re: ViewCube orientation on document create - Application Options revert back

Anonymous — Tue, 04 Oct 2016 19:04:17 GMT

Yes, we've done that and it's working great, like I mentioned the issue was the orientation the model was presented on document creation.

Someone helped me figure out what was wrong with my code, so here is some iLogic that works

SyntaxEditor Code Snippet

Sub Main
    Dim invApp As Inventor.Application = ThisApplication
    
    invApp.CommandManager.ControlDefinitions.Item("AppViewCubeHomeCmd").Execute
End Sub

The downside to this is that if you're in an assembly and use the Create command, it will also perform the home command, but at least on black assembly/part creation you can have the model be presented in the correct orientation.

Thanks again for all your help guys.

Re: ViewCube orientation on document create - Application Options revert back

Curtis_W — Tue, 04 Oct 2016 20:36:55 GMT

Hi bbuck,

It looks like you figured it out as I was looking at this, but here's a rework of the original as well. I'm guessing this issue was with the file type, so this one works with assembly and part.

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

Sub Main

Dim oSele As SelectSet
Dim oWP As WorkPlane
CmdMgr = ThisApplication.CommandManager.ControlDefinitions
docType = ThisDoc.Document.DocumentType

If docType = DocumentTypeEnum.kPartDocumentObject  Then
	Dim oDoc As PartDocument 
	oDoc = ThisDoc.Document
	oWP = oDoc.ComponentDefinition.WorkPlanes(3) 'XY plane
Else If docType = DocumentTypeEnum.kAssemblyDocumentObject Then
	Dim oDoc As AssemblyDocument 
	oDoc = ThisDoc.Document	
	oWP = oDoc.ComponentDefinition.WorkPlanes(3) 'XY plane
End If

oSele = ThisDoc.Document.SelectSet
oSele.Clear
oSele.Select (oWP)

CmdMgr("AppLookAtCmd").Execute
CmdMgr("AppViewCubeViewTopCmd").Execute
CmdMgr("AppPreviousViewCmd").Execute

End Sub

Re: ViewCube orientation on document create - Application Options revert back

tmxkn1 — Thu, 28 Apr 2022 19:15:35 GMT

The marked solution does not seem as a solution at all!

I solved this by editing all the template *iam and *ipt files found under

C:\Users\Public\Documents\Autodesk\Inventor <inventor_version_number>\Templates\en-US

Steps:

go to this folder
Open standard.ipt
Change the viewcube orientation to whatever you want
Save the file
Repeat 2-4 for each of the template files.

The template files are only empty assembly or part files that have all the customisation saved already.

Re: ViewCube orientation on document create - Application Options revert back

WillL84 — Thu, 21 Jul 2022 14:20:34 GMT

This doesn't work for me. I've set the viewcube orientation and set Z to up using "Set current view as front" on the viewcube, also set the home position and saved that as an IPT template. It still creates a new IPT with that template looking top-down, or looking in the -Z direction. Nothing I do will get it to start a new IPT looking at the front (+Y) orientation. My template has +Z as up, +Y as directly away and +X as to the right.

Re: ViewCube orientation on document create - Application Options revert back

johnsonshiue — Thu, 21 Jul 2022 16:38:59 GMT

Hi! Please make sure the template file resides in the default template folder. You will need to make such change to all ipt and iam template files you want the orientation to persist.

Another option to ensure view does not rotate is to turn on origin planes visibility. This will avoid the auto-rotating behavior when you create the first 2D sketch.

Many thanks!