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Horizontal and Vertical Constraints is reversed ???

16 REPLIES 16
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Message 1 of 17
EbbeFN
4062 Views, 16 Replies

Horizontal and Vertical Constraints is reversed ???

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.

16 REPLIES 16
Message 2 of 17
JDMather
in reply to: EbbeFN

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.


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Message 3 of 17
EbbeFN
in reply to: JDMather

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

Message 4 of 17
JDMather
in reply to: EbbeFN

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?

 

Coordinate System.png

 

If X is defined as Horizontal when on XY plane - should it still be defined as the Horizontal when on XZ plane for consistency?

 

Glass Cube.png  Do you get the behavior you expect if you click on this arrow?


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Message 5 of 17
EbbeFN
in reply to: JDMather

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

Message 6 of 17
johnsonshiue
in reply to: 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!

 



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Message 7 of 17
EbbeFN
in reply to: johnsonshiue

🙂

 

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

Message 8 of 17
JDMather
in reply to: EbbeFN


@efn 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.


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Message 9 of 17
johnsonshiue
in reply to: EbbeFN

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 Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Message 10 of 17
rkeller
in reply to: johnsonshiue

Johnson,

 
Thank you for the link.
 
I have the files with me here at home so I'll try duplicating the same problems I've been experiencing at work here after making the option changes you suggested.  
 
We skipped 2014 install because of constant crashes and difficulty installing it with our Virus protection installed. "F- Prot "  
 
Working with the Beta team on Dyson and the folks at CRYEN AV we've solved those issues now so we jumped in with 2015 but it is driving us nuts with constraint issues.  Tangent, and angle constraints don't work at all like they used to.
 
And once I finally was able to constrain a part using angles and tangent constraints after changing the view using F6 the parts flipped to the inside of the tank.  Aggravating doesn't even come close to describing the way I was feeling today. 
 
Rodney 
Message 11 of 17
johnsonshiue
in reply to: rkeller

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!

 



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Message 12 of 17
EbbeFN
in reply to: johnsonshiue

🙂 solved the problem - THANKS 🙂
Message 13 of 17
harm
in reply to: EbbeFN

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?

Message 14 of 17
Mark.Lancaster
in reply to: harm

@harm

 

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.

Message 15 of 17
harm
in reply to: Mark.Lancaster

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!

Message 16 of 17
peter.kapitola
in reply to: EbbeFN

Here is a description of the behaviour that apparently makes sense to Inventor but is confusing to users: 

 

  1. Create a new part.
  2. Create a new sketch.
  3. Click on the XY plane. By default, the View Cube now shows "Front" view with the word "Front" in the correct orientation. 
  4. Horizontal and Vertical constraints are now as would be expected. Y is vertical, and X is horizontal. 

    peterkapitola_1-1649060704556.png

     

    Now, 
  5. Create a new sketch.  
  6. Click on the YZ Plane.  By default, the View Cube now shows "Right" view with the word "Right" in the correct orientation. So we've essentially rotated the view 90deg around the Y axis, keeping Y pointing in the same direction. But Y is now considered "horizontal"! No wonder people are getting confused. We have just rotated the view 90deg to the right around the Y axis, keeping Y pointing upwards (vertical), but now Y is no longer vertical! 

    peterkapitola_2-1649060811036.png

Things are somewhat less confusing if you go and select "Align with Local Coordinate System". 

peterkapitola_3-1649061204127.png

 

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! 

peterkapitola_4-1649061337404.png

 

So in summary I would recommend "Align with Local Coordinate System" as the default option. Otherwise you end up with "vertical" not meaning "vertical".  

Message 17 of 17
johnsonshiue
in reply to: EbbeFN

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!



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer

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