Automatic Constraints

[ptc-5122510]

I've been having an issue since installing Creo 2.0 where I'm trying to create an assembly and pull in parts, but they're not constraining correctly. I was watching a Creo Primer video, and the speaker said that Creo is smart and will automatically learn the constraints you've been using on a part and will apply them the next time you pull the part in. My problem is that mine will not automatically learn the constraints, and I have to go back and re-select the parts and constrain them manually. This isn't a terrible issue, but it is annoying when the video says that something SHOULD happen and it doesn't. The first file that I put in for the assembly file was the cube and then started adding cubes and shafts (cube file isn't labeled as cube currently).

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[ptc-4314565]

Vladimir,

After reading your reply a little more carefully, I went back and checked what the setting was on my personal laptop with WF5. Create_temp_interfaces was indeed set to 'no' as a default. This then makes me wonder why WF5 and Creo 2.0 were behaving differently when placing multiple instances of a part in an assembly as I described in my reply to Antonius. Interesting, but now that I've got your trick for placing the same component multiple times in one placement session, the point is moot to me.

[vzak]

Aleksey,

I have no explanation to this - there should be no change. Neither we heard such effect from other users.

if this effect continues, can you send data + environment to TS with this question (config files etc - just note that you need to grab all config.pro files on the path, in the eay they get loaded when starting Creo)

[fmueller]

Hi,

I am also VERY annoed by ne new behaviour of Creo 2 (compared to wildfire 3, which we had before) when I'm placing components in an assemby.

Due to the new placements like "normal" this is alway the one chosen by Creo as standard. I am askin myself (and PTC) now why the hell is Creo thinking, that when I place axis to axis or datum plane to datum plane I want them normal (90°) to each other by default???

For me (and I hope I'm not alone in this wide world) the standard would always be that the objects I chose shall intersect each other ( in german: "Zusammenfallend"). So please change that standard behavoiur back as it was before Creo came up with a placement like "normal".

That would already help a lot, even, when the automatic contraints and use interfaces by default is disabled.

[vzak]

Hi FRIEDER,

Neither Creo always forces Normal, nor you have to use new capability at all. Normal is just one more constraint while Coincedent and Angular already had this smartness - if respective position of 2 surfaces was above certain angle it siggested Angle and not Offset. Its just a big enhancement (not an annoyance) that Creo supports now Angle and Normal for lines as well as for surfaces.

Now about controls :

1. If you set auto_constr_always_use_offset = Yes - you will ALWAYS get Coincedent as default suggestion, for planes / lines / planes+lines.

2. If you keep auto_constr_always_use_offsetn = No - this means you accept Creo smartness to suggest MOST CLOSE contraint to your current situation. Current situation may be more close to Distance, or Angle, or Normal.

Correlation by the three is defined by 2 config options which are self explanory :

- comp_angle_offset_eps

- comp_mormal_offset_eps

Configuring those you get full control on which default type would appear in which case.

Hope this clarifies and you will feel more comfortable with the software.

Regadrs

- Vlad

[fmueller]

Hi Vlad,

thanks for your clarification. Nice to learn some new things. I'll try a little with that options and see what fits best for me.

regards

Frieder

[fmueller]

Hi Vlad,

I have today played a little with the different options and found that I like the automatic but the defaults are too sensitive for a roughmotoric like myself ;-).

I prefer the following more coarse value for

comp_angle_offset_eps 15

and the more fine value for:

comp_mormal_offset_eps 5

Question an obviously not (yet) existing option "comp_distance_offset" would be very nice too. Do you think it's possible to integrate that in the future too? That would allow to "snap" to coincident just when the distance is smaller or equal than a certain amount.

regards

Frieder

P.S. Bold typing can't be deactivated in the formatting of the editor. Maybe an error in the Forum Software?

[vzak]

Hi Frieder,

Eventually we have a setting for what you asked - I just missed it out in my list. This setting is :

auto_constr_offset_tolerance = (0.5 of the model size by default).

So posting corrected flow of "decision making" now with this config :

1. If you set auto_constr_always_use_offset = Never - you will ALWAYS get Coincident as default suggestion, for planes / lines / planes + lines.
2. If you set auto_constr_always_use_offset = Yes - you will always get offset type of constraint, never Coincedent
3. If you keep auto_constr_always_use_offset = No (default) - this means you accept Creo smartness to suggest MOST CLOSE constraint to your current situation. Current position may be more close to Coincedent, Distance, Angle, or Normal.

Correlation of these four is defined by 3 additional config options and the check works in the following order:

1. a. Check if position fits Angle or Normal. For this use values set for options:

- comp_angle_offset_eps
- comp_mormal_offset_eps

1. b. IF position does not fit ANGLE or NORMAL, then it will be either Coincident or Distance. Here decision is made based on the value of :
   
   auto_constr_offset_tolerance = (0.5 of the model size by default). If initial distance is biggest than this value you will receive Distance, if less – Coincident. Note that value is relative to the size of each component being assembled.

[TomD.inPDX]

Thank you, Zak. You bring a world of clarity to the forum with your detailed posts. Indeed, these are things one misses easily when looking at the assembly interface at "face value" if you will.

I can only say that hiding basic functionality like "repeat" under the RMB is troublesome. I have run into several occasions where such an important feature is essentially "hidden". Developers need to know that RMB options should only be "quick access"; secondary... to easily accessible features in the current feature tab. This would solve so many missed opportunities.

Is there a good tutorial that explains all those options you mentioned above so we can take a minute to review a better overview of core Creo assembly capabilities?

[vzak]

Antonius,

You are more than welcome. As to tutorials - I'll check next week what help files include, though I doubt they have too many details. There is also a thing called "learning connector" (not sure if it is for free though) - I heard they have real professional movies, and by a couple that I saw they really do.

Given this topic gained that level of attention, I'll try to make a short demo avi to cover Interfaces for the forum audience later next week ... just can not commit when I can get to this :-).

Are there any upload limitations to keep in mind (file types / size? )

Best,

- Vlad

[TomD.inPDX]

I am not sure if there is a file size limitation for the video. However, YouTube video quality is much better but limited to 10 minutes. Format also doesn't seem to matter. I upload AVI but MP4 should be more compressed.

I have the learning connector. It is very dependent on what you have for options. Base Creo users don't get a lot of relevant videos.

I once had access to many more tutorial videos and reviewed many of them. They are indeed good quality lesson plans. The only problem I find with them is they are not clear as to whether they apply to an optional extension or core Creo. All to often I was disappointed by fining out my version didn't have those features... which is probably why I didn't realize we had the ones you and others mention here because a lot more features are found in the advance assembly extension.

Anyway, Vladimir... thank you again for all your effort in making more of the tools we have.