How to rotate a sketch and keep dimensions oriented correctly?

[bruce.crock]

I have created a parametric sketch, it looks like a zipper and I'm using it to create the cut lines for a finger jointed laser cut project.  The sketch has X fixed size teeth in the middle, and an "arm" on each end so that I can copy/paste it, place it, and then elongate it with the arms as necessary to fit the part. 

It worked well when using it for a horizontal cut line in the xy axis. But when I rotated it 10 degrees for a different part, the dimensions dissappear.  

I tried to drag the end points and allow the constraints to rotate the sketch, but the dimensions stay in the original axis rather than rotating with the line.

Is there a way to keep the dimension measurements aligned to the lines as I rotate them?

Thanks!

[etfrench · Accepted solution]

Put the sketch with the original dimensioned lines in a component.  Copy and paste the component.  You can rotate the new component and the dimensions will follow.  

[lichtzeichenanlage]

@etfrench: I'm still not used to have components with sketches only. Thanks for this great hint!

[bruce.crock]

Thank you very much.  I'll keep my eye open for others cases where this same pattern (leveraging the function of the parent object to manipulate the child) may help me.  I don't find that pattern intuitive, though I realize it's similar for joints, and probably a fundamental benefit of Fusion once it's natural.  

thanks again for the response, saving me hours finding an alternate solution.

[chrisplyler · Accepted solution]

We figured out in another thread about a month ago, that dimensions created vertically or horizontally automatically get some sort of hidden constraint that tells them to always be vertical or horizontal. So then when the base element that is so dimensioned gets rotated, that related dimension can no longer properly exist.

I suggested that the only hidden constraint such a dimension SHOULD get is to always remain parallel to the element it is related to, but they haven't changed the behavior so far.

We did discover that if you rotate everything a bit, THEN dimension it, then rotate it back, none of the dimensions will have been created with that hidden vert/hor constraint, and will continue to work as expected during future rotates.

The reason that rotating the whole component instead of the sketch avoids this problem is that when you rotate the whole component you are rotating everything inside it, including it's origin, so that those hidden constraints are still satisfied.

[bruce.crock]

Thanks for posting this note.  I tried this myself last night before I made my post but I must have made a mistake because I thought it didn't work.  I tried again now and it worked.  This is a far preferable method since creating a new component for each of ~50 sketch parts is a lot of overhead, navigating the hierarchy becomes irritating and error prone.