A Problem With Orientation

[Anonymous]

Hello Folks,

Vertical is no longer vertical.

I've been working on this part file and all of a sudden I noticed a change in what Inventor perceives as "vertical", the "Y" axis.

As observed in the (in sketch) "Normal" screenshot, the X, Y and Z planes appear regular; vertical, horizontal, etc. This is also realized by the appearance of some black lines coincident with the X and Y planes. Note the sketch line that I drew that locked in the normal vertical orientation.

As observed in the (in sketch) "Skewed" screenshot, the X, Y and Z planes appear regular; vertical, horizontal, etc. The appearance of the black lines are now not coincident with the X and Y planes. Note the sketch line that I drew that not locked in the normal vertical orientation (in relation to the planes) but "vertical" appears to be reoriented and locked into those black lines.

This sketch had normal orientation earlier but is now weird. I likely did something to cause it but I don't what what I did.

I don't know what happened, but I don't like it. How do I normalize my orientation situation?

Mel

[JDMather]

If possible, and practical, use only the Origin Planes for sketches. (The BORN Technique.)

Try to avoid using part faces as sketch planes (especially skewed part faces.

Also, make sure you are up-to-date on all Service Packs and Updates for your version of Inventor.

[Curtis_Waguespack]

Hi melvin.burk,

It's difficult to guess based off the screen shot alone. Can you attach the part file for others to examine?

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

[Anonymous]

Hello Folks,

I'm not used to being limited in terms of which surfaces/planes to use as sketch base geometry when modelling parts. I definitely would not be able to do my job if I limited my part design to using only the original X,Y and Z planes.

Being a SolidWorks user, I don't think I've ever heard of such a thing nor do I recall encountering this change-of-orientation behavior in SolidWorks.

As I've said before, SolidWorks is easier for me to do my job. The behavior of Inventor makes it necessary for me to create more sketches (and other reference geometry) - a more complicated feature tree - than I would using SolidWorks for the same part. Let the crucifixion begin.

I just want a solution to my problem. Please.

The file is attached and I will check for updates for my software.

Mel

[Anonymous]

Hello Folks,

The Communication Center says my product is up to date.

Build: 200, Release: 2013 SP2 - Date: Fri 04/19/2013.

Mel

[JDMather]

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@Anonymous wrote:

Being a SolidWorks user, I don't think I've ever heard of such a thing .... 

---

Using the BORN Technique in SolidWorks is considered best practice as well.

This topic is covered in several SolidWorks texts.

Most of your sketches are not fully defined.

This is usually covered in a beginning SolidWorks class.

When I add some of your missing dimensions - they are perfect.

Did you delete dimensions?  Why would you do that (in SolidWorks or in Inventor)?

I don't understand why you would create this part at (an undefined) angle.  Assembly constraints will take care of position (in Inventor or in SolidWorks).

[Curtis_Waguespack]

Hi melvin.burk,

Thanks for the part file that helps in understanding the issue.

I think we've seen this question come up in the past. Unfortunately, I don't recall the explanation, and it's not obvious to me as to why we are seeing what we are seeing. Maybe @johnsonshiue can have a look and tell us why this is. ( Note that I am seeing this in Inventor 2015, but it looks like melvin.burk is using Inventor 2013 )

For others:

To see the issue first go to the Tools tab > Application Options buton > Sketch tab > Display area, and then select the Axes check box.

• When editing Sketch 7 (look in Extrusion1)  notice that the displayed Axes are NOT rotated, and align with the UCS.

• When editing Sketch 9 (look in Extrusion3)  notice that the displayed Axes ARE rotated, and do not align with the UCS.

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

[Anonymous]

Hello JD,

I've never heard of the BORN technique but have always tried to implement the KISS protocol. I understand - and implement - the concept of keeping solid model data as simple as possible.

True. Most, if not all, of my sketches are minimally defined. Most of those sketch elements are cut-and-pasted AutoCAD geometry. I would normally fully define everything.

This part is one of several of a course of architectural terra cotta. The part is created at an angle as, when considered in context with other "related" parts of the course, the default "plan" view of this part would make coworkers more comfortable. I likely won't create a solid assembly that includes this part.

Not creating fully defined and/or mated solid model assets bothers me, too. A lot. I've taken the SolidWorks classes and learned the "right way". In my current environment, it is considered a waste of time to fully define sketches. Some consider the use of Inventor, itself, luxurious and a waste of time. Speed is important and I want to remain employed. They don't use a lot of solid assemblies here so, there's that. When in Rome...

I also want to use the best tool available to me. Right now that's Inventor. When I become as efficient and effective with Inventor as I am with SolidWorks I'll slip-in those dimensions on the sly. I'll get there.

Mel

[Anonymous]

Hello Curtis,

This phenomenon did not occur when I initially created the part. I would not have been able to create the feature. It appeared when I attempted to edit the feature (2 holes on the top surface).

My first guess is that I accidentally hit a key or two and caused this to happen. That's where my money is.

I will create the part from scratch and see what happens.

Mel

[Anonymous]

Hello Curtis,

I did not create the part from scratch. What I did do was rotate the geometry in AutoCAD, compensating for the skewed UCS phenomenon. That worked well. Inventor did not counter compensate.

I'd much rather my UCS be normal all of the time.

Mel

[Anonymous]

Hello Curtis,

As I think about what I've done, I realize that the one different thing I did do was added a projected view of the part in the Inventor drawing, a view that wasn't there initially. I may have seen a "do you want to back annotate" type message that didn't make sense in it's appearance or relevance. Of course I clicked OK.

Clue? perhaps.

Mel

[Curtis_Waguespack]

---

@Anonymous wrote:

My first guess is that I accidentally hit a key or two and caused this to happen. That's where my money is.

---

Hi melvin.burk,

It's almost as if you edited the sketch co-ordinate system, but I can't see that happening on accident, as it's a somewhat involved process, not just a click:

http://help.autodesk.com/view/INVNTOR/2013/ENU/?caas=caas/vhelp/help-dev-autodesk-com/v/Inventor/enu/2013/Help/1310-Autodesk1310/1500-Parts1500/1501-2D-sketc1501/1503-Sketch-c1503.html

Maybe pasting in from AutoCAD pulled in a different sketch coordinate system. I used to do 3D in AutoCAD way back when, and recall having to reset the UCS in order drawing on a angled face, ect. (don't recall how to do all of that now), so maybe that brought in something odd. But I've never heard of this happening, so that seems a bit unlikely also.

As for working with un constrained  or under constrained sketches, you probably know from your years using Solidworks that it's almost never a good idea to do so, but I still can't see that causing this issue.

http://inventortrenches.blogspot.com/2011/03/inventor-101-simple-fully-constrained.html

Note too that if you're basing this part off of other related parts,  there is likely a multi-body workflow that would simplify the process a great deal. Allowing you to make all of the parts in one file, and then write them out as individual parts and place them in an assembly, all in the push of a few buttons. If interested post some images or simple details, and I'm sure someone will demonstrate a quick example.

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

[johnsonshiue · Accepted solution]

Hi Guys, This behavior is related to how Inventor locate the sketch coordinate system. You can see the coordinate system by exiting out of sketch environment and right-click on the sketch -> Edit Coordinate System. What is confusing here is how the sketch coordinate system is defined. Inventor sketch tries to take the selected face loop into account and align the coordinate system to a straight edge when applicable. The rationale is that if a face is selected to place a sketch, the coordinate system should be tied to the face. This behavior makes sense when the design is build on top of each face. It can be confusing when the design needs to be based on origin coordinates. We are investigating on how we can improve the behavior and make it more predictable. In the meantime, you may want want to consider creating UCS or redefining the sketch coordinate system aligning to origin axes. Many thanks!

[Anonymous]

Hello Johnson,

I was able to straighten-out the coordinate system-per-sketch as you outlined here. It wasn't perfect but is was effective.

Thank you,

Mel