Avoid update of translation in drawing? 1

[BrooklynW]

Hello,
I'm having a bit of a problem updating some drawings on CATIA V5:
I have added translations to my part models in order to have them at exact coordinates in my assembly but unfortunately, when I revert back to the drawing and update it, all of the dress up dimensions go haywire.
If I deactivate the translation in the part model, the drawing updates with no problems but then the assembly is off.
I would lock the view in the drawing, but we are regularly making slight adjustments to these parts and locking the view prevents any changes to be updated.
Is there any way to update everything other than the translation??

 

[Albigger]

Don't put translations in the parts. Use constraints to position the parts within the assembly where you want them.

 

[BrooklynW]

This has presented some problems regarding parts snapping on to others, sometimes where we didn't even realize they had done so until it was too late. If one part is off, every part thereafter will be off. It also makes the tree too complicated. Mainly due to the extensive tree, my boss has asked me to keep all constraints within the parts rather than the assembly.

 

[DBezaire]

Good policies will help you out with this. Use and lock the setting Tools - Options - Mech Design - Constraints - Use published geometry of any level. Also turn on Infrastructure - Part Infra - General - Restrict external selection with link to published elements and allow publication of faces, vertices and axes extremities. This will make the designer aware of what he is linking and constraining. This also will make it easier to follow what somebody else did to create the assembly. There are many other benefits of published geometry and search on this forum will highlight those.

Regards,
Derek


Win XP64
R20/21, 3DVIA Composer 2012, ST R20
Dell T7400 16GB Ram
Quadro FX 4800 - 1.5GB

 

[BrooklynW]

Awesome thank you!

 

[BrooklynW]

Now, this may be a dumb question, but "use published geometry of any level" is unpickable... How can I change this? Is that something that needs admin priviliges?

 

[DBezaire]

Is there a red lock next to Use any geometry. This will indicate admin lock out of this setting.


Win XP64
R20/21, 3DVIA Composer 2012, ST R20
Dell T7400 16GB Ram
Quadro FX 4800 - 1.5GB

 

[BrooklynW]

No, there is not a red lock.

 

[DBezaire]

That is odd, perhaps your settings are corrupt. Nothing new in the Catia world. The default location for your settings C:\Documents and Settings\user name\Application Data\DassaultSystemes\CATSettings
Rename this folder and restart Catia. If you are running LUM it will ask for your license again. You can pick it from the list or just copy the Licensing.CATSettings file from the renamed folder to the new CATSettings folder.

Side note. You should have a CATSettings folder for each version

What version are you using?


Win XP64
R20/21, 3DVIA Composer 2012, ST R20
Dell T7400 16GB Ram
Quadro FX 4800 - 1.5GB

 

[BrooklynW]

Running version 21
Got ahold of our support company and apparently our license doesn't have the right add-ons for this.
Is there, by any chance, another way to keep the part translation separate in case I am unable to acquire the add-on?

 

[DBezaire]

It's a nice feature to have but not a necessity. Do you have the other, Use Published geometry of child components only? If you dont you can still publish the constraint geometry and this will indicate to other designers or even yourself the design intent and constrain the items to the proper geometry. The constraints would automatically reconnect themselves if you were to Assembly Design replace component item A with a similar item B and the published names were the same.



Win XP64
R20/21, 3DVIA Composer 2012, ST R20
Dell T7400 16GB Ram
Quadro FX 4800 - 1.5GB

 

[BrooklynW]

Luckily we are getting a license that will allow me to change the constraint options so I can finish this the way you, DBezaire, initially recommended. Replacing items with similar is a great tip that I plan on storing in the back of my mind for future reference. You have been very helpful. Much appreciated.