Crooked views in a drawing or assembly drawing

[jniessen]

We have had a number of students start an assembly drawing only to find their object out of alignment (crooked). I found out that what they had done was to use the free rotate tool on the base object and turning the object out of square. Why they can do this I am not too sure as the piece should be automatically grounding. But they don't.

This link is to the site I found the first solution and since have found a better one. Below the link is the reply I posted with what i think is the better of the two solutions.

http://forums.autodesk.com/t5/Invent...y/td-p/3439093



I am a school teacher and this is the first year we have had this "crooked" views problem. We, meaning the kids and I have two solutions of which the second is by far the best.

Before I get to the solution I would like to point out that the first part put into an assembly is not always grounded. Or, in our case, it’s never grounded. Anyone know why not? All other years it has been, so i think maybe the installers have changed something.

As for the solution, the one above, constraining to planes, works well but not always. If the planes show up in "red" when you go to select them it will work. If they show up in "White" you won't be able to select them. We have not been able to figure out why they are white sometimes and red others. Anyone know why?


The best solution is to;

While in the assembly view
Select the "view" tab
Go to the "navigate" section on the far right
Choose the "look at" option
Select the face of your object you want to be the front.
The object will rotate into a square view facing you

Right Click the view cube
Choose the option to set the current view as front view

Go back to your drawing and the view will be correct and straight.


Hope this helps.

[Bunny]

This behavior changed ( ...in the last release or the one before.. I do not remember...) After selecting the first component, or subsequent components for that matter, RMB and you will see an option to "Place Grounded At Origin" This will align the 2 coordinate systems and ground the component. If you want the first part/assembly to always be grounded, go to Application Options, Assembly tab and check "Place and ground first component at origin". To align an unconstrained component that is already in the assembly, go to Assemble tab > Productivity Panel and click on the fly-out under Create Substitutes. Toward the bottom of the fly-out you will see "Ground and Root Component". Select it and then the component, and the command will align the origins and ground the part/assembly.

HTH

[jniessen]

Thanks for the reply. We didn't get a chance to try your solution as we found another way.

Our solution was to enter a new sketch on one of the flat surfaces. While in sketch mode right click on the view cube to "set current view as front". exit sketch mode and it is straightened.

[BWMCDOWELL]

Thanks for the reply. We didn't get a chance to try your solution as we found another way.

Our solution was to enter a new sketch on one of the flat surfaces. While in sketch mode right click on the view cube to "set current view as front". exit sketch mode and it is straightened.

Are they not constraining their parts or assemblies to the origin?
If they constrain the parts/assemblies to the origin (planes/lines)then that will set the view angles no matter how they were last viewed.