Hello
Can you remind me how I can insert two different (unrelated) parts into an assembly from the same part?
For the moment, by doing the "insert a component in an assembly twice on the same part", I get two instantiations from me. So if I make changes on my part, these changes affect the 2 instantiations in my assembly.
Thank you in advance for your help.
Hello
What software do you work with?
For the moment it is logical. If you insert the same piece into an assembly 2 times, if you modify one, the other one follows.
If you want 2 different pieces, you need 2 different files.
See this CATIA user manual
https://moodle.univ-tln.fr/pluginfile.php/40797/mod_resource/content/2/LIVRET%20CATIA%20V5.pdf
Solidworks can do it with configs!
Two different configurations of a part can evolve together in an assembly!
Hello
If you work on Solidworks, I know that if you make your parts "virtual" in your assembly, it breaks the links with their origins.
EDIT: Sorry I didn't see that it was for CATIA. Invalid answer then;)
You just have to copy and paste directly from the part in the assembly but make a special paste... / break the links of the dependencies
+1 Frederic +1BBPoulet.
Two different parts mean either two CATPart files, or two bodies of parts (in the same Catpart).
Of course, CATIA manages External or Internal Referrals
Ex if it's two pieces have a common base but independent adaptations.
Thank you for your advice.
A simple method that seems to work well.
I open the part that I want to insert into my assembly.
Then, in this part, I do "save as" and I save under a different file name.
So I then have 2 different parts because with two different file names.
I can then insert them into my product and they no longer have any links between them.
Complement:
This method works very well, I just make a clarification:
When you do "saved as" you create a new CATIA file with the same one (ID N° internal) which allows you to relink the plan that points to the old version.
If you do "Create from" you create a new CATIA file with a different ID (you can't relink the plans of the old version).
"which makes it possible to redo the link of the plan which points to the old version"
Can you tell me a little more about it so I can see what it means?
If it's not too complicated, I'd be interested in a little example.
Hello
A copy to windows (renamed) or a saved under (new name) from CATIA does not change the internal ID of the file, any files created in these ways can be re-associated with a CATDrawing pointing to any of these files. The CATDrawing update will take into account the changes made in the file on which it is pointed.
A create from (change the internal number) you will not be able to point the plan of the old file to the new one.
Under CATIA, the best practice when you want to create a version of a 3D file, you have to first open the 2D file, then edit / link open the linked document(s), (then you save the 2D and 3D at the same time) there you are sure not to lose any links.
Very clear, thank you.
And if I summarize, I think that I will very rarely use "create from".