Sketch mode -- How do I disconnect a line segment from another without deleting?

[Jaimie]

Hello,

When you draw a series of lines in creo it automatically creates some hidden constraints between the segments so that they act like joints and move together (coincident). Similarly, if you use the coincident constraint to move an existing line to another, the constraint also does not show up and acts as if it was an initially drawn line segment. How do you find the constraint and delete it so you can separate the entities without deleting the entity? 

In the attached example I want picture 4 to go back to picture 1's state without ctrl+Z (which is no longer possible if its a modification of an existing sketch and not something you just did, or if you did a lot of sketch work before realizing you need it unattached). This has caused me to redo entire sketches and features and break all existing references before which can be an enormous amount of work on a part like a casting.

In this particular case one of the only ways I found without scrapping half the sketch is to add divide marks, redraw the last line,  delete the last 3 segments and redefine all the dimensions/constraints that existed before, but that is still somewhat destructive and would like to just delete the coincident constraint like you can in other parts of the sketch (the point circled in the picture)

Similarly, is there any way to undo the divide command? Is there a line rejoin option I'm unaware of?

I'm wondering if there is maybe a configuration setting that I can turn on to see the implicit coincident constraints on line segments. 

Thank you,

Jaimie

[pausob · Accepted solution]

Consider using the rotate/resize tool (in the editing group of the sketcher's ribbon) to move your sketched geometry around.  This will allow you to "disconnect" segments that share endpoints.

[Jaimie]

Thank you, that does work. It's not quite the same as just deleting the coincide, and breaks some other constraints (namely dimensional ones) but its way better than deleting the sketch and redrawing from scratch.

Thanks,

Jaimie

[pausob]

From another thread related to sketching, I came upon a hidden gem of sorts - if you hold CTRL key you can sometimes drag these "coincident" points apart.  Without any tools active in the sketcher, just hold CTRL and drag an endpoint.  It should allow you to extend / shorten one of the lines emanating from the common vertex.

[Jaimie]

Thank you! This is the simple response I was hoping was the case!

I knew about the ctrl+click drag to extend/shorten lines, but didn't realize it did in fact break that inherent coincident feature! I swear I tried with all the different commands, ctrl, shift, alt, ctrl+shift, etc but couldn't get it to work. Must have been because while you drag it away it's stuck inline like it is still clearly coincident, so I must have stopped there and didn't place it first to check if it was broken. As soon as you place it the constraints are broken and then can move it at an angle now. 

Thank you very much!