Inventor 2011 redefined sketch always rotates and is unable to be rerotated

[smiz]

Autodesk users,

I am looking for any information on this issue. Most of my workk is done in a single sketch and revolved, often times hours of time is spent on this sketch. Several times the original plane the sketch was on needs to be changed. Every time I redefine my sketch to a new plane it rotates the sketch 90 degrees. I am then unable to rotate it once it is redefined.

Our work aroudn for this was to always start a sketch on a newly created plane revolved around the z axis, so if I do need my origin sketch at a different relative angle you can just reposition the plane via its angle. The strange this is that even if I redefine the sketch to a new plane that is in the exact location of the original it will still rotate 90 degrees.

I have had soem success previously with deleting and vertical or horizontal constraints and then being allowed to rotate, but in my current instance this is no longer working. If anyone has any tips as to why this is happening or how to fix it that would be great!

Thanks 

[mcgyvr]

Why do you need to redefine the sketch plane in the first place?

[smiz]

By practice we only derive dimensions via sketch driven inputs, so inorder to retreive the dimension in a section veiw the section line in your drawing needs to match the plane your sketch was drawn on. 

[Curtis_Waguespack]

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@smiz wrote:

... often times hours of time is spent on this sketch.

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Hi smiz,

Sorry, I don't have an answer to your direct question, but would you be able to post an example file of a part, or some screen shots of a part, that requires a sketch that takes that much time? I suspect your workflow could be adjusted to makes life easier. But I might be mistaken.

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

[smiz]

The time isn't as much spent on actually drawing it, it is more in the interpretation of getting to the end product. This is what I'm working on now. As you can see the centerline is now facing vertically when it was drawn facing horizontally. I am also unable to rotate this sketch at all and get an error when doing so. 

[Curtis_Waguespack]

Hi smiz,

I don't see that as a single sketch to create a single Revolve, but rather one base feature that has many more simple sketched and/or placed features. If you took this approach your base sketch would be a simple shape that would allow you to redefine it much more easily:

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

However, I'm not sure I understand why you'd redefine a part's base sketch to retreive a dimension for a drawing view?

In any case, are you using the Rotate tool on the sketch tab?

and if so are you looking at the >> button to see the options to relax constraints, etc.?

If not how are you attempting to rotate it?

You mention an error, can you provide more information, a screen shot of that?

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

[blair]

"Hours spent on a single sketch"

I keep my sketch's very simple and try to limit them to a single feature within the item. If I need to create a revolved shaft with snap-ring grooves at each end. I revolve the shaft by it's self and then create a new sketch for the groove and revolve it. If the grooves are the same at each end and symmetrical about the middle of the shaft, the second groove gets mirrored. If the shaft has chamfers at each end, they get processed as a chamfer feature.

It's much easier after to correct an items without spending much time. I only need to suppress or delete the desired item in the model browser window.

[smiz]

The issue that we run into if we were to make this a "simple sketch with multiple other sketches off of it is the fact the most of the geometry is defined by other features. In order to make the part fully defined we would either need to do a lot of math to create dimensions from the origin point, or use projected geometrey which we do not use. 

As far as redefining a sketch to the retrieve dimensions command, this is because your drawings section line needs to match of with the sketch plane. For example if we are making a just a revolved box aroudn the z axis and need a section line vertically on the top of the part, the part would need to be sketched on a plane in that location or it will not properly pull the dimensions. So in my case I drew the original sketch in the wrong spot so it does not match up with my section line in the drawing, therefore my retrieved dimensions will not properly get pulled.

With that being said whether my sketch is simple or complex the issue is still occuring. And in this case this is actually just the base sketch with many other smaller sketches defining it. This is just the first revolve.

As for rotating, yes I am within the sketch and I am relexing all sketch constraints. The error is coming in choped of but it is attached below. 

[smiz · Accepted solution]

UPDATAE!

Thank you all for taking the time to help me on this. I ended up finding the issue.

When I redefined a sketch to a different plane it was changing the direction of the x and y axis. Rotating it 90 degrees. I noticed the "edit cordinate system: button upon right clicking my sketch. This allowed me to re position the axis to where they should have been and flipped my sketch back in the correct posisition. After constraining my center line the sketch is now back to what it was, and on the correct plane!

Thanks again everyone!