Hi out there
Is this just me - invetor 2015 - new part - create sketch - and then when I use the vertical constraint it makes things horizontal and vice versa ......... ???
Vh Ebbe F.N.
Solved! Go to Solution.
Solved by johnsonshiue. Go to Solution.
Create sketch where? What plane? What orientation of the View Cube? What orientation of the coordinate system?
Attach file here that exhibits this behavior.
Show screen shot including coordinate system indicator in lower left corner of screen.
Hi - it works ok when sketch is on XY-plane - but not at XZ-plane.
Note its IV that decides whats up on the sketch when I choose edit sketch !!
Vh Ebbe FN
I do not see any discrepency.
1. Your View Cube is rotated 90°.
2. Your Horizontal Constraint does match the X axis.
3. Note that with the black axis lines that one is thicker than the other. The thick axis is always horizontal.
When moving around in 3D space - all is tied to a common coordinate system.
I do not see any difference than previous releases?
If X is defined as Horizontal when on XY plane - should it still be defined as the Horizontal when on XZ plane for consistency?
Do you get the behavior you expect if you click on this arrow?
Hi
I know what you mean - but I have been working in Inventor since no 1 - and this is new to me. I accept that I can just rotate my sketch - but in previous versions (upgraded from 2012) when editing a sketch Inventor normally "auto-rotates" the sketch so that up is "up".
If i am going to check the wiev-cube and the coordinatesystem when editing a sketch - why the this "auto-rotation" ???
Mvh EbbeFN
Hi! Indeed, if you pick a planar face to create a sketch, Inventor will determine the sketch coordinate based on the edges constituting the face. Sometimes, it could be opposite to what you have in mind. Have you tried UCS? You should consider creating UCS associated with the face. Then create the sketch on XY plane of the UCS. In this way, X-axis and Y-axis are always in the direction you would like (in sync with UCS XY).
Thanks!
🙂
I dont think I am able to explain the problem 🙂 - its obviously about the "autorotate" done by Inventor when I pick "edit sketch" ! 🙂
I see the thick and the thin lines correspond to the axes - but why on earth isnt the horizontal lines "auto-rotated" to be horizontal 🙂
I can live with it - but it dosnt make sense.
Thanks for your time.
Vh Ebbe FN
@Anonymous wrote:
I see the thick and the thin lines correspond to the axes - but why on earth isnt the horizontal lines "auto-rotated" to be horizontal 🙂
I can live with it - but it dosnt make sense.
I agree entirely with this.
Your original problem statement was about Constraints, not the auto view orientation.
Hi! I think this is about the behavior that the view is rotated "unpredictably" after the sketch is created, not about how the sketch coordinate system is created (though they are related). There is indeed a new option controlling how the view rotates on creating a sketch in R2015. By default, Inventor tries to minimize the view rotation from the current view to the sketch view. The option is located at Tools -> Application Options -> Display -> "Look At Behavior" at the bottom. The default option is "Perform Minimum Rotation." To restore the legacy behavior, click "Align with Local Coordinate System" option instead.
Thanks!
Johnson
Johnson,
Hi! It seems like you are experiencing something different (not view rotating or sketch coordinate issues). Could you post the files here or send them to me directly (johnson.shiue@autodesk.com)?
Many thanks!
Hi
I have the same problem. Also use inventor since version 2!
horizontal is not horizontal on the display
verttical not vertical!
how did you solve this?
Did you read the solution to the problem? What version of Inventor are you using?
Mark Lancaster
& Autodesk Services MarketPlace Provider
Autodesk Inventor Certified Professional & not an Autodesk Employee
Likes is much appreciated if the information I have shared is helpful to you and/or others
Did this resolve your issue? Please accept it "As a Solution" so others may benefit from it.
Maybe, I am gonne try the folowing
"
The option is located at Tools -> Application Options -> Display -> "Look At Behavior" at the bottom. The default option is "Perform Minimum Rotation." To restore the legacy behavior, click "Align with Local Coordinate System" option instead.
"
Viewcube, I never use, never need, so took no notice of the view being not "upright"
I understand this new option, but by default maybe better on "Align with Local Coordinate System"
thanks!
Here is a description of the behaviour that apparently makes sense to Inventor but is confusing to users:
Now,
Things are somewhat less confusing if you go and select "Align with Local Coordinate System".
Now, when you create the second sketch on the YZ Plane, vertical and horizontal are at least still pointing vertically and horizontally on the screen. The view cube shows that we have now rotated 90deg around the Y axis and then another 90deg around the X axis. We're now tilted on the side. But hey, at least vertical is now vertical!
So in summary I would recommend "Align with Local Coordinate System" as the default option. Otherwise you end up with "vertical" not meaning "vertical".
Hi Peter,
Indeed, this option may help reduce the likelihood of the offending behavior. However, it does not completely resolve it. It is because when a planar body face is selected to create a sketch, the sketch coordinate will be based on the face loop (boundary). This process is solely determined by Inventor. As a result, depending on the face loop shape and orientation, the XY may be aligned accordingly. You will need to edit the sketch coordinate. Or, use UCS instead.
Many thanks!
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