Inventor Assembly Exported To Parts Axis Not Aligned Anymore

[vliegend_duiveltje]

Hi,

I'm busy drawing ribs for a wing of a RC airplane. But when the wing ribs are exported as individual parts they don't align with the axis in the .ipt screen.

I mean that looking while it is in .iam mode everything nicely align with the axis. but when I click on the part to modify it, it doesn't align anymore with the axes.

This is the way I did it:

Created 2 work planes root and tip, imported excel coordinates that where then connected with a spline.

Then lofted from root to tip rib to create the wing.

Then shelled the wing

Created a new work plane above the wing. Then draw some rectangle shapes on that plane to cut out in the wing so that only the ribs left behind.

Then each rib I projected the geometry to create the actual rib as a new part.

True the manage tab I then created the individual parts in to a new assembly.

kelly.young has edited your subject line for clarity: Part not alligned

[CCarreiras]

HI!

This is because the parts maintain the same ucs as the original part, which is good to place the parts correctly in the assembly and without effort.

You can create create new UCS in each part if you like to use the center planes (as i like too).

[johnsonshiue]

Hi! Could you share a screenshot or an example what you are describing here? I think there should be a logical reason behind the behavior.

Many thanks!

[vliegend_duiveltje]

Here are some screenshots from the sketch. In the first one you can see that the wing profile nicely lines up with the Z axis. When I then want to begin a new sketch on to one of the wing profiles it turns. I've attached the sketch and excel coordinates.

[johnsonshiue]

Hi! I think I know why it behaves this way. This is due to the way Inventor determine sketch coordinate. When you started the first sketch, it was based on origin X, Y, and Z. Then you create a sketch based on the side face. The coordinate chosen by Inventor is based on the selected face loop. To change the coordinate, please follow the steps.

1) Finish sketch.

2) Right-click on the sketch in the browser -> Edit Coordinate System -> you will see the sketch coordinate system glyph shows up.

3) Click on the origin point on the glyph and then select the part origin point.

4) Click on the sketch X axis and then select part Z axis -> right-click -> Ok.

Many thanks!

[vliegend_duiveltje]

Just tested the solution Johnsonshiue give me. This works but I noticed I need to do this for each new sketch on the different ribs. Is there a way that it can be applied on all the parts at once?

[TheCADWhisperer]

Rather than sketch on part face, I recommend offsetting the Origin Plane and do you sketching on work planes.