Regeneration and Relations 2

[treddie]

I have a problem with regeneration of parameters in a relation. After some checking of the available posts, it seems the following is not possible, but I am curious if there is at least SOME solution, somehow:

I have DTM2 driven by DTM1 via a relation...When DTM1 moves, the relation determines the new position of DTM2. The problem is that although DTM1 is moved and after I hit OK, regeneration does not move DTM2...I have to regen a second time for it to take effect. So it seems that either the relation is properly executed during the first regen, but the parameter for DTM2 is not updated until second regen, or that during first regen, the relation is never run and will not run until a regen of the whole part. Either way, this seems crazy because I can have points that always lie at the intersection of a DTM and some curve, and only one regen is ever required for the points to move along with the DTM. That is in essence a "relation" in itself.

Is there no way to force an automatic regen of the whole part once DTM1 is moved?

Many thanks!

 

[looslib]

What version are you using?

On WF4, I created a datum plane, DTM1, a fixed distance from TOP. Create a second datum plane, DTM2, offset defined by a relation of 2 X the distance of TOP to DTM1. When I edit the DTM1 offset value and hit OK, the dimesnion turns green and does not move DTM1. When I hit regen, both datum planes move.

On Creo, DTM1 & DTM2 will move when you hit OK, if you have auto regenerate turned on. If not, it acts just like WF4.




"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[treddie]

I am using Creo. I have been looking for an auto-regen, but could not find it in Options (even after doing a search). Could not find it by Googling either. Where is it? Because it definitely sounds like you do not have the same problem I have.

 

[looslib]

When you have your model open, select the Model tab. On the left is the Regenerate Icon and word. Click the word with the arrow under it will open the menu to allow you to toggle Auto Regenerate on or off.

There is a config.pro setting to control it.
enable_auto_regen
yes*, no
Controls whether a model is automatically regenerated when you edit entities or dimensions in Edit mode.
yes—The model is automatically regenerated.
no—You must manually regenerate the model after edits.

* indicates the default behavior.

Somehow your system has it turned off.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[treddie]

Hm...I think we may be in parallel universes here. I have no Model tab. My version is Creo Elements/Pro 5 M080.
Also, when I go into Options > Current Session and search for "enable_auto_regen", it does not come up. Weird.

 

[jvian]

Treddie,

Just an FYI but Creo/Elements Pro 5.0 is just a renaming of Wildfire 5.0 and is not the same as the official Creo 1.0/2.0 release. I have made similar relation driven datums and have not had the issue you are describing. Some of what you describe can happen if the relations are multilevel (i.e. different relations and parameters across different parts in an assembly or features in a part) but if all relations are on the same component level it should work. Some calculations do however require a second regeneration as they are based on the first regen results but I can only recall that as I described above and with parametric equation curves and helix sweeps or with relation driven parameters which drive a relation.

As a workaround you can create a 'special regen' mapkey that will dual regenerate which shouldn't cause any problems unless you struggle with large regen times. Otherwise if the second regen is not necessary a message will show stating such.

Hope that helps and good luck,

- J -

 

[treddie]

Ahhh, pre-Creo Creo. The bastards!

Thanks for the info. The 'special regen' key idea sounds like a good way to speed up things a bit, until I can move over to REAL Creo.

Thanks again, all!