We just switched from Wildfire 4 to Creo 2.0.
The copy paste functionality in assemblies has changed a bit with dependancies of parts when you copy more than one at a time. An example of something that I do regularily is a bolt and nut combination. A lot of times Patterns aren't the best option, and I generally don't like patterns a whole lot anyways.
Old (desired) way:
What I would do it constrain the bolt, and then constrain the nut to only the bolt for the first pair. Then to copy the same pair I to a different hole, I would select both the bolt and the nut, hit ctrl-c and then ctrl-v. The paste/place component of the bolt would show up and I would set the constraints and then hit OK. The nut would keep the same constraints onto the bolt and I would just hit ok.
Creo makes me define every constraint of both the bolt and the nut, irregardless of how I have them constrained in the copied components.
I'm sure that there are options to define this behavior, but I am having trouble interpreting the cryptic option list that is the configuration file.
Anyone willing to help me figure out what options are available to set this up?
Solved! Go to Solution.
Ok, I found a solution to get the copy and paste work like it used to. You have to set a hidden config.pro option.
This came from the PTC help tickets.
Set hidden config.pro option use_temp_interface_for_paste no
Gotta love it, they change something that isn't broken........again.
Why not use the repeat command? It will allow you to choose which constraint you want, or any combination of constraints.You can place numerous parts in seconds.
Try this option in config.pro:
This creates an interface feature for the 1st assembled part so that subsequent parts will follow the same inputs. This means that if you place a bolt by axis and surface, subsequent assembly of this part will only request the assembly's reference and not the component so all you need to pick is the axes and surface you want to mate to.
You can overwrite this behavior during placement.
Using pattern relation is nice, but only when they work reliably.
Would that mean that every other engineer in my company that pulls up that bolt would get that same interface? Or is is temporary?
If you all use the same screw as a library part, you can add an interface to that screw, so it would be the same placement prompt for every user, every time.
Yeah, one of the guys tried to do that (made sense to me) but some of the other engineers didn't like it, so we don't want the interface on the regular part.
So I've tried the repeat command and it works really well for what it was designed to do, repeat a single component. It, however, does not handle multiple components. An example would be a wheel, hub, spindle group with all of the hardware. I used to have to select the parts I wanted to copy, copy, then paste , and only have to select the constraints from where the the spindle meets it's hinge. Now I have the re-click for every component in the assembly which can be very difficult to remember all of the exact same steps.
Does anyone else have any suggestions on how to get it to work like it used to?