View Cube

[Anonymous]

Hello,

When starting a new sketch for creating a part can the view-cube be set to display the workplanes in a specific view

How do i set the view-cube when starting a new sketch like the picture 

Ray H

[cbenner]

@Anonymous

Welcome to the forums!

I'm a little confused about what you're asking.  When you start a new sketch, is this not what you see?

What version of Inventor is this? (standard question)

[mcgyvr]

If you mean having the origin workplanes visible then just open your template file.. Turn their visibility on then save..

Now they will be visible when you start a new part using that template..

If not please use words to describe what you need vs an image so its very clear..

[Curtis_Waguespack]

Hi Ray_H,

I think what you're asking about is Inventor's habit of rotating the part over to the Y up orientation at the beginning of a new sketch, even when the view cube has some other direction defined as the top. This issue is demonstrated in the video below.

As far as I know there are not any settings to control this, and there is not a solution to this issue, other than having at least one origin plane visible in your template file.

When one or more plane is visible, Inventor will not do this at the beginning of a new sketch. However, leaving planes visible creates other issues, so in my opinion this is not a good solution.

This is one of those bothersome behaviors that someone programmed in to Inventor to "help" new users, but it can often be a pain. There really should be an option to disable this.

A recent related discussion:

https://forums.autodesk.com/t5/inventor-forum/origin-plane-issues/m-p/7384283#M659638

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

[cbenner]

@Curtis_Waguespack

I've never seen Inventor behave this way.  My viewcube opens in the "Home" orientation and stays there when I begin a new sketch. 

[Curtis_Waguespack]

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@cbenner wrote:

I've never seen Inventor behave this way.  My viewcube opens in the "Home" orientation and stays there when I begin a new sketch. 

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Hi cbenner, 

If your template is set up with the home view being Y = Up, X = Right &  Z = Left then you will not see this. Or as mentioned, if you have a work plane visible, Inventor won't tip it over on new sketch creation.

But for those people that set their templates up so that Z = Up, this is the behavior they have to deal with. 

There are several different industries that use Z = Up. And the importance of the orientation comes into play more when collaborating with others, where the Inventor model is exported, to be used in another system. 

Attached is an Inventor 2017 file that you can open and create a new sketch in, in order to see this issue.

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

[johnsonshiue]

Hi Ray,

I am sorry if this is a repeat. This is quite simple. Just open any of the template part file of interest. Then make all origin planes visible. Save the template file. Next, go to Tools -> Application Options -> Sketch -> uncheck both boxes for "Look at sketch plane when create or edit a sketch." Next, start a new part based on the template. Create a new sketch and pick one of the origin planes. You will see the view no longer rotates.

Many thanks!

[Curtis_Waguespack]

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@johnsonshiue wrote:

... Then make all origin planes visible...

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@johnsonshiue

 hmmmm. I feel like Inventor is functioning inconsistently here due to a hard coded behavior that is not expected when a user's template is set to a home view orientation other than the default. Further, I would expect your "simple" solution to cause more problems later. 

I maintain that it is best practice that users turn off origin and work plane visibility at the level they exist. In this case meaning that the planes should be turned off in the part file.

So the problem with offering the idea of turning the origin planes on in the template as a solution, is that users will then need to turn off the visibility of the origin planes before they save each part, and then turn them back on if they later decide to edit the part and add another sketch & feature ... and then turn them back off before they save again... and back on... and back off.. and so on.

If the users leave the work planes on they end up with situations like these:

• https://forums.autodesk.com/t5/inventor-forum/turn-off-work-planes-and-sketches-in-assemblies/m-p/68...
• https://forums.autodesk.com/t5/inventor-forum/prevent-planes-becoming-visible-when-unhiding-part/m-p...
• https://forums.autodesk.com/t5/inventor-forum/all-planes-amp-sketches-turn-visible-when-editing-an-a...
• https://forums.autodesk.com/t5/inventor-forum/reappearing-unwanted-work-planes/m-p/3706570/highlight...
• I could likely find about 10 more of these discussion with a little more effort...

Turning on the planes in the template and then turning them off in every new part, and on and off again after every edit quickly becomes a bother, and a lot of aggravation just to work around an issue that Autodesk has created by adding this behavior without making it aware of the template's "home view" orientation.

But putting the work plane visibility aside for a moment, my question would be:

If Autodesk has implemented this feature to help new users sketch on origin planes, why should we expect design departments that use templates with "Z = up" to configure their Application Options and template origin planes in a way that doesn't allow their new users to take advantage of this helpful behavior? 

This behavior of making the origin planes visible and rotating the part in order to help new users create a sketch on an origin plane should be tied to the home view orientation of the view cube, so that users that that do use "Z = up", do not have to turn on origin planes and modify Application Options in order for their templates to work the same as people that use "Y = up".

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

[IgorMir]

Thank you, Curtis!

I second your post. These types of "enhancements" serve only one purpose - to annoy the users. More often then not I am missing those days when design software were designed with real engineers input.  Nowadays it seems more and more that the software is designed by some kids, who are out of work but still - need some income. And their papas and mamas are helping them to get through some companies door. 

Cheers,

Igor.

[johnsonshiue]

Hi Guys,

Making origin planes visible in the template file is a way to suppress the view rotating behavior on creating a sketch without any visible geometry. Like I mentioned before, when you create a new sketch with no visible geometry to select, it can be confusing to some users, particularly new users what to do next. This is a design choice. There is room for improvement for sure. It would have been better if there was a way to suppress the behavior using an option. We cannot assume everybody likes the behavior. There is a lot of interesting debates and discussions about this exact topic on Inventor Beta forum (sketch coordinate, orientation, and so on). I don't think the status quo is ideal. There should be ways to make it better.

Regarding making workplanes visible, if I recall correctly, it was considered standard practice for 3D feature-based parametric solid modeling. There is no reason to keep the origin planes visible after the model is stable. Also, after there is visible geometry to select, the view rotating behavior would no longer happen.

Many thanks!

[SBix26]

I like the current behavior and routinely start new parts by simply hitting S on the keyboard, which displays the origin planes for selection.  But I agree that the orientation should respect the View Cube definition of Top/Front.

Sam B

Inventor Professional 2018.1.2
Vault Workgroup 2018.0
Windows 7 Enterprise 64-bit, SP1

[Curtis_Waguespack]

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@johnsonshiue wrote:

... Also, after there is visible geometry to select, the view rotating behavior would no longer happen.

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Hi johnsonshiue,

Ahhhh, indeed you're correct. My assertion that the user would need to turn the planes on and off and on and off for edits was wrong. 

I'm still not sold on the idea of having a template with origin planes visible as a solution to this issue, but as a workaround I suppose it does suppress the unwanted rotation.

I'll visit the beta forum later if I have a chance, and look for the discussions on sketch coordinate, orientation, etc.

Thanks!

Curtis

[mcgyvr]

Hey @Anonymous Come back and help these guys out and give us more details about what you really want so they can stop this assumption party they have going on in here.. 

[Anonymous]

Sorry just arrived back. Many thanks for all replies

1. open a new part file .ipt

2. select 2D sketch

3. Opens in correct View orientation

4. When i then hit the Home button it changes Orientation

5. I want the View Orientation to remain as #3 above

I know i can at #3 above, right click on the Home Button select Current View as Home then select Fixed Distance and it will resolve the issue ....but is there a way of setting a default so that when i start a new sketch the View remains always as image #3

Can i set this up as a template?

I am off again now but will check in tomorrow...thanks to everyone

Cheers

Ray

[Curtis_Waguespack · Accepted solution]

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@Anonymous wrote:

Can i set this up as a template?

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Hi @Anonymous,

Yep that's what you want to do, here are the steps:

1. Start a new part file using the template you want to update
2. Use the view cube to set the correct orientation (don't create a new 2D sketch, just click the view cube corners)
3. Right click on the Home button select Current View as Home then select Fit to View (not Fixed Distance)
4. Go to the File tab > Save As > Save Copy As Template
5. Save the file as the same name as your template (so that you're replacing/updating the template)
6. Close the file
7. Start a new part file using the template you just updated
8. Test to see that the home view is now updated.

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

[Anonymous]

Many thanks Curtis