Axes rotated in a part file

[Karol-Or]

The part isn't symmetrical about the YZ plane, you can see it in the sketch of extrusion 1.

Now i started a new sketch, sketch 24, and the part is positioned like in the picture, with the YZ plane not vertical.

Why?

[JDMather]

I do not see a Sketch 24.
I do not see if you specifically want Sketch 24 on YZ Plane.

I do not see an image attachment.

Sketch7 is skewed and not constrained/dimensioned.

I recommend that you DO NOT suppress Extrusion7 if you are using it for something and instead - expand the Solid Bodies folder at the top of the browser and right click on Solid2 and turn off Visibility).

Otherwise you migh loose a reference if you are using it for some purpose and then Suppress it.)

(BTW - I don't know how you are getting away with those special characters in the filename.)

[Karol-Or]

Sorry, i didn't save the file, and here is the image of the projected YZ plane

[JDMather]

Try closing Inventor and reopen.

It is perfect on my machine (YZ Plane cannot move).

[Karol-Or]

I restarted with no help. it happens on 2 computers.

In shared Sketch14 the semi horisontal body line is a projection of the XY plane.

The line on the left is just vertical, with vertical constraint, and you see it makes an angle of 90.44 degrees.

The dimensions on the right show the problem. the left dimension is to the projected plane, and it appears in the drawing made for that part, but i design with dimensions like the right one, which is just vertical to the screen, perhaps, because i don't know what happened

[JDMather]

Work Plane2 was offset from a part face that does not have a horizontal or vertical reference.

It picked the two ends of the arc for reference (that aren't horizontal to the coordinate system).

(BTW - if the part were symmetrical you would not have encountered this problem, but since it isn't symmetrical you must excercise extra caution.  Actually this is just good practice with any part to use the Origin for reference rather than anything else if at all possible.)

So then the sketch created on that workplane has a local coordinate system that doesn't match the Origin coordinate system.

I don't understand the purpose of this workplane, and in any case I would offset one of the origin workplanes rather than a part face.

I also suggested earlier that you NOT suppress the second solid body, but rather right click and turn off the visibility.

Frankly - I would use what was learned on this first attempt and start over.

[Karol-Or]

I don't understand many things, so i will start.
What does it mean that the face doesn't have horizontal or vertical reference?
I made the solid with revolution1 and extrusion1, in which both sketches are fully defined.
What do you mean by horizontal and vertical reference? i opened new sketches and made horizontal and vertical lines, i don't understand

[JDMather]

This is actually a very good problem for illustrating something in my book.

In all the years I have participated here - I don't think I have ever seen this problem in such a clearly defined way.

I like it!

I exaggerated the offset in Sketch4 so that you can clearly see that Workplane 2 was created with horizontal reference these two points.

Now if the part were symmetrical those two points would be horizontal (with reference to the Origin folder planes).

So this illustrates a very good reason to NOT use part faces for creating Reference geometry (like workplanes) unless there is no other way - or there is a very good reason for doing so.

If there is a good reason - you could Project Geometry the Origin planes and use Perpendicular and Parallel constraints rather than Horizontal and Vertical.  I think there is an Option in Tools>Application Options to set these as the Priorty, but I think it still often requires manual intervention.  Bottom line - avoid part face-based reference geometry unless there is no other way.

[JDMather]

Well, this gets even more interesting.

If I create the sketch directly on the part face the coordinate system is rotated.

This would have been barely noticeable before I exaggerated your cut.

[Karol-Or]

Good, thank you, i will use only, if i can, and even if it demands more labor, the origin planes.
But i want to understand the mechanism of the software.
You mean to say that before i even created a sketch on plane2, or at the creation, the sketch's axes were rotated?
Inventor just picks 2 arbitrary endpoints and aligns the axes?
Why aren't the origin axes automatically copied to the sketch, if the sketch plane is parallel to the origin?

[JDMather]

Hopefully someone from Autodesk will come along and comment.

For me to comment further I would have to remodel the part from scratch trying to reproduce all the steps that I think  you used, but if I were modeling that geometry I would do very differently than you did, so I am reluctant to try to reproduce your part.

Well, I was curious - so I was able to easily reproduce this behavior from scratch in a new file.

[Karol-Or]

Can i realign, in a new sketch, or even in an old one, the sketch's axes parallel to the origin?

[JDMather]

I think you can, but not sure.

I'm done with this one - I would simply start over and do it "right".

[JDMather · Accepted solution]

Well, again curiosity got the better of me.

It was pretty easy to re-align the coordinate system.

Right click on the sketch.

[Karol-Or]

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I also suggested earlier that you NOT suppress the second solid body, but rather right click and turn off the visibility.

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Why not suppress?

What's the difference between suppression and turning off visibility?

[JDMather]

Inventor is a history based modeler.

Parent-child relationships.

If you go back into history and suppress a parent - the child can't possibly exist.

If you go back into history and hide the parent - the child can still exist.

I will post an example when I get a chance.

[Karol-Or]

Thanks