Well, it seems to work for me. I attach a toy model for demonstration:
Changing the value of the assembly parameter "POSITION" changes the configuration of this assembly.
This includes change of shape of the stationary part (1st block), the displayed labels and notes, and the constraint types of the 2nd block (the one labelled with the prime').
The logic is coded in relations at various levels (assembly, component and feature). Another important bit is use of associated parameters as this assembly involves flexible components.
There is still something wonky going on in that switching from configuration "1" to configuration "3" requires a double-regeneration (the 1st regeneration leads to a green-light, but the component is clearly not in the right place) I think that is a bug related to the slider connection having motion limits.
Modifying or debugging such a model can be a nightmare.
For example, when I was adding the 3rd configuration, I found I had to temporarily delete all the component relations in the 2nd block. Otherwise the system didn't really let me add the slider constraint set as it was failing in "finding" a connection - I think it was because the relations were in play and during the definition of the new constraint, they would try to make one of the previously defined constraint sets active (even though I disabled them all during the definition). I suppose I should have set the value of "POSITION" to 3 during this phase.
As expected, there were no helpful messages as to what was going wrong.
In summary, I'm not surprised that relations involving PTC_CONSTRAINT_SET can lead to frustration, because a lot of things can go wrong while building such a model. But if the relation logic is sound, the software does work - for the most part.
(attached models are made using Creo 2.0 - I'd be interested to hear if the "slider bug" is solved in newer versions)
Thank you for looking into this. I am using Creo 4 and switching from configuration 1 to 3 in your model requires a double regeneration for me as well.
I have made a slightly more complex dummy assembly consisting of several subassemblies and parts to show how "ptc_constraint_set" seems to not work as intended.
If you open "combustion_air_system.asm" and i.e. change the values of planes in skeleton group configuration like this:
reducer_type from value 1 to 0
silencer from value 1 to 0
heater from value 1 to 0
and then hit regenerate they are clearly misplaced.
Double regeneration doesn't do anything but edit definition fixes the placement of these components. The placement of each component is defined in relations through "ptc_constraint_set" (component level) and "distance=length1+length2+length3..." (assembly level). Why doesn't regenerate place them correctly but edit definition does?
So I got Creo 4 and had a chance to take a look at your model.
I'm pretty sure the reason it's not working isn't related to PTC_CONSTRAINT_SET, simply because isolating the investigation to AIR_INLET_UNIT.ASM shows the same weirdness.
Initially, the driving values of the following dimensions are:
REDUCER_TYPE=1
SILENCER=1
HEATER=1and the model look like this:
Upon changing the values:
REDUCER_TYPE=0
SILENCER=0
HEATER=0
and regenerating leads to:
(note the message in the log that suggests something is wrong with the design...)
Suppressing and resuming the components leads to the correct situation:
Alas, I can't really spend more time on this as your "simple" example is actually fairly complicated and involves Pro/Program interactions. I do think that it's all in the relations and pro/program code inside the AIR_INLET_UNIT.ASM (and not involving the COMBUSTION_AIR_SYSTEM_SKELETON, as making the features of that skeleton read-only does not change anything).
I'd investigate the relations and code that involve the REDUCER_TYPE and HEATER parameters, because changing the SILENCER parameter seems to work as expected.
Thank you for your reply, I understand it takes time to really dig into this.
I think the SILENCER parameter works better simply because it is controlled by fewer IF statements than the REDUCER_TYPE and HEATER parameters, as it is "first in line". I just did a test however, and the silencer part does fail placement when REDUCER_TYPE and FLAME_ARRESTOR is changed from 0 to 1.
If anyone knows why the "design inconsistent for current parameter values" message is shown, I'd be interested to know. It seems to be quite rare, a Google search didn't give many results. I didn't get this message myself for some reason (using Creo 5 now). I would also be interested to know how/why regeneration and edit definition/suppress + resume considers component placement differently.
For now I am moving the "insert here" arrow to the top to quickly suppress everything, and then back down to resume. This does fix component placements, but if anyone else has a look at this and figures out why, I would be very interested to know.
In the attached model (zip) I have moved all relations to assembly level so it should be easier to understand. I have also added some component length parameters so the distance/placement relations are much easier to read. In Pro/Program the components are only suppressed/resumed based on whether the connected parameter is 0 or 1. I don't see how that could cause or affect this behaviour.
I just did another test and changing the same three parameters that you did (REDUCER_TYPE, SILENCER and HEATER) from 1 to 0 *one at a time* rather than all at once gets the placement right. That isn't always the case however, so problem still not solved. Until someone can tell me what I'm doing wrong, it seems like some kind of bug in Creo to me, why can't it decide ptc_constraint_set and distance at the same time? And why would it behave differently when changing parameters one at a time rather than all at once? Shouldn't the logic below place the heater part correctly based on the values of connected parameters (when I click regenerate)?
As far as I can see there aren't any better ways to accomplish what I'm trying to do. I have had a look at Creo Options Modeler but I'm not sure it works well for very large assemblies and configuring both component existence and placement/orientation at the same time.
