Why Inventor do not add feature change Z Axis up?
Hmm. I only tested in 2020 with 4 templates: New->Templates->en-US->Metric
1. Standard(DIN).ipt: View Cube TOP , z down on screen
2. Standard(mm).ipt: View Cube TOP , z down on screen. No change
3. Standard(DIN).iam: View Cube TOP , z pointing out of the screen
4. Standard(mm).iam: View Cube TOP , z down on screen
Conclusion: Setting 3 looks good to me, but setting 1 needs a change
Walter Holzwarth
Hi @WHolzwarth
I have 2 points:
1/ It will make confuse if you use View Cube long time.
2/ When you export other format such as STEP file, it will be come issue with Axis.
Hi Travis,
Changing Z-axis up is pretty straight forward. In a Y-axis up file, click on Front in the ViewCube -> click on the downward arrow button below ViewCube -> set current view as Top -> rotate the ViewCube to a desirable Isometric angle -> Set Current View as Home -> Fit to View. Do the same to your template file. So all newly created files have Z-axis up.
I was not aware the Fusion offers a command to facilitate the behavior. I do think it will be useful in Inventor too. Let me work with the project team to understand it better.
Many thanks!
Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
In Inventor, the modeling orientation is determined by the file (.iam, .ipt). It looks as if Fusion 360 does it differently, where the modeling orientation is set as an application preference. I'm sure each has its advantages and disadvantages, but the reasons for the different choices are not shared with we users. Nevertheless, it is easy to change the orientation in each application, when you know how.
In Inventor, it's simply a matter of changing your template files as @johnsonshiue described.
Sam B
Inventor Pro 2021.1 | Windows 10 Home 1903
LinkedIn
I follow your instruction, there are issue when I click new sketch:
What I should do next?
Did you try export other format such as STEP file? Is it keep Z axis up?
Hi Travis,
I believe that you redefined Top and Front but you did not redefine Home. Please reorient the ViewCube in an isometric direction (Top/Front/Right). Then click on the downward button under ViewCube -> Set Current View as Home -> Fit to View (or Fixed Distance).
Many thanks!
Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Hi Travis,
I see the behavior. This is yet another well-intended enhancement leading to awkward behaviors. What you are seeing is about the ability to show origin planes for creating a 2D sketch when nothing is visible. Inventor will rotate the ViewCube to the Y-up orientation (hard-coded internally). To disable the ability, you need to make origin planes visible. Whenever there is geometry to select for placing a 2D sketch, the ViewCube will stay put.
Many thanks!
Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
1/ It can keep Top when I turn on Visibility Origin Plane.
2/ Did you try exporting STEP file?
I open it in Rhino 6:
I feel like they only orient view port, it not really change Axis?
Please add new feature to change Z Axis.
Travis, I reproduced your settings. STEP has no change in axis, both in Inventor and in Rhino.
But I'm wondering, if your settings here are as intended.
With View Cube in TOP position, shouldn't Z of World coordinate system point out of the screen? In your setup it's pointing vertical on the screen area.
2019 IPT and STEP in Zip attached.
Walter Holzwarth
Hi @WHolzwarth
I recognize your point. I set up again:
Open STEP in Rhino 6
There are serval steps to do, I summarize:
1/ Orient Z axis to UP
2/ Set current view/As Top
3/Set current view as Home/ Fix Distance
4/ Turn on Visibility of Origin Plane (in order to keep Z up when create new sketching)
I save as Template.
Then I try import file 3dm to Inventor.
They will not keep Z axis up.
I think about change default template to new template Z axis up.
Do you have any suggestion to do it? or other solution?
As far as I know, STEP import uses the settings in Standard.IPT template. Some like it, others have separate preferences. The only way seems to be declaring adapted settings as new Standard.IPT, after doing a backup of the initial file.
Here's another thread with similar questions:
https://forums.autodesk.com/t5/inventor-forum/step-file-import-template/td-p/7624948
Walter Holzwarth
There is another issue that arises from using Z-up which hasn't been brought up, and one that I think is far more pernicious than the view rotating when creating the first sketch (although I am unsatisfied with the existing workarounds for that).
The issue I am referring to presents itself when using with frame generator. If I create a frame in a Z-up system, some components will be rotated in undesirable ways depending on the direction of the skeleton frame member. I provided an example in the embedded image. The assembly has a Z-up coordinate system with the viewcube corrected to match. When I insert W-flange beams to align with the floor opening edges, the beam members will rotate in odd orientations instead of being oriented the same way as they would in a Y-up system. I can rotate these members after the fact, but it's tedious, and would just be easier to model everything in Y-up.
This issue alone prevents me from being able to model in Z-up entirely, even though I work architecture where Z-up modeling is standard in other programs like AutoCAD and Revit. I would like to model in Z-up so that I can export Inventor models to those programs without needing to rotate them.
I really wish there was an option to change the modeling orientation from Y-up to Z-up like there is in Fusion 360. Baring that, it would be nice if the frame generator was better at recognizing how "up" is defined. Lastly, if I adjust the viewcube, I shouldn't have to turn on a work plane to prevent the view from rotating on its own when making the first sketch. Though I would not do that. Instead, I would click the home button to reorient it. Either way, it's an extra step that is a waste of time and one that users should not be forced to do for every new part.
Please consider these suggestions as changes to implement in Inventor. It would make working in this program a much, much more enjoyable experience and remove the frustration I feel everyday by being limited by the default UCS system.
