constraints broke sketch

[Anonymous]

Anyone can explain below ???

[asiteur]

Hi,

Could you explain what the 'LL orientation' is? Is this a custom iLogic form, an addin,....?

The pink lines in the last picture indicate that references could not be resolved. Are the lines in your sketch projected?

[Anonymous]

It makes sense when you have horizontal and vertical constraints in the sketch. Even editing the coordinate system will ruin the sketch. If you want a robust sketch for a slot then start with the center line as construction line and draw it at angle. Dimension the construction line with an aligned dimension. Then construct the slot around it, make the sides parallel and attach the arc centers to the ends of the construction line. This slot can be moved and rotated at will. Align it to references in the part.

Alex

[PaulMunford]

Or use a sketch block...

[johnsonshiue]

Hi! The error is due to the fact that the sketch coordinate system is flipped or rotated. Some constraints no longer make sense afterwards. If the workplane can rotate or move around, you might consider using UCS. The sketch coordinate system will be based on the XYZ on the UCS and when UCS moves or rotate, the sketch will adjust accordingly.

Many thanks!

[Anonymous]

Yes. It's kinda of ilogic form.
The work plane need to be rotated for ease of assembly work later.

[Anonymous]

hi Johnson Shiue

This part was actually assembled with a cylinder. I want to link the work plane with its orientation. In assembly file, one can mate their origin together and rotate the work plane to 30 deg, consequently, the part will be rotated 30 deg (plan view of cylinder)

I don't get why the sketch coordinate will flipped when the work plane is rotating (>=90 deg).

looking forward your opinion.

thanks

[Anonymous]

Lesson I learnt from working with ProE : if you need a feature that can be rotated then create it rotated, even if most of the time it is at 90° angle. You mention a workplane at angle. Start by creating this workplane. Then sketch your feature using this workplane. Project the workplane to get a construction line at angle, then "glue" the feature to this construction line. If you do it right then rotating the workplane will not invalidate the feature.

Watch out : dimensions can also be - invisibly - constraining. For instance : if you draw two horizontal parallel lines and dimension the vertical distance by clicking the lines then you are automatically constraining these lines to be horizontal. You can remove the horizontal constraint from it, you still won't be able to drag them at an angle as long as the dimension is present.

Alex

[Anonymous]

Hi Alex.

indeed, I'd created another work plane (i'd called it my workplane). "my workplane" will be as rotating used.
the sketch was created in 'my workplane' and properly constraint (well, 'glued'). the constraint will be removed once 'my workplane' was rotated more than 90 deg. sketch will be upside down, mirrored, constraint removed.... etc...

seem its only valid if you did not rotate it more than 90 deg.

[Anonymous]

What I was suggesting is to use a workplane to define the angle, not to rotate a workplane. Look at the images. Drawing on XY but using a workplane to define where the feature is created. Any angle is accepted.

[Anonymous]

hi Alex,

first thought the solution might work, hence I recreate another part by using the approach.. but same outcome was found..
hmmm (single sketch like yours is workable)
think its solely because of coordinate system changed if we exceeded 90 deg...

[Anonymous]

find attached screencast