I have assembled a turnbuckle and I have placed the two spindles with 'slider' constraints. However, I would like both spindles to move symmetrically related to the body of the turnbuckle when one spindle is dragged. I thought that it was possible to create a relation that would make the distance from the body of the turnbuckle to the spindle half of the extension.
Does anyone have experience with this?
2 helical sweeps, one left-hand, one right-hand, with cylinder and planar constraints on the center, and slider and slot constraints on the ends.
I have converted it to a flexible component in the assembly in which it is used. Then I have introduced a relation that makes the distance from the centre of the pin to the centre of the body half of the pin-to-pin distance. This works to some extent, but constraining it in the upper level assembly is still a bit tricky.
....you can never make it too fancy. However, project managers do not appreciate creativity so sometimes we need to stop early if we don't want to listen to their whining.
That works too, I guess I just (maybe incorrectly) assumed you'd meant that you wanted to be able to turn the turnbuckle and have the ends come in. And I TOTALLY agree on the managers having any sense of what we actually do. You can be the best, most valuable CAD wizard on the planet, and you will never get any respect for it. In their minds, you're just a glorified "drafter".......
If you leave the link unconstrained as a cylinder, you should be able to constrain the holes at both ends at the next level.
You can also apply some relations to the turn-buckle to set the span in the higher level assembly. The relation can be associated to a measure feature, for instance.
I'd have to do it to give more info, but it is a fairly straight forward process. Learn it once and save a reference model for later.
Fairly straight forward.
The ends are assembled as cylinder connections. Do not apply regen values.
The turnbuckle assembly has a relation for the distance of one to the other.
This remains variable but equal.
The next level assembly has the axes for setting the distance.
In this case, changing datum 4 location also changes the strut length after the 1st regen.
To get the green light, you have to do one additional regen.
Creo 2.0 attached
You could use a slot and follower connection. It uses a curve to determine the movement of a point. Just create a helical curve on the surface of the "threaded" shaft. one right hand the other left and two points that will lie on those curves.
CAD / PLM Systems Manager