Hello
I created an optimized copy of a gear on which a certain number of parameters are applied (module, number of teeth, etc).
Unfortunately when I make the optimized copy in another part, the associated parameters do not copy at all.
I tried to re-associate these famous parameters but too sumptuous so waste of time, which is not the purpose of the optimized copy.
Do you have a solution for this?
I thought of options to check in catia but I can't find anything.
I hope my request is clear, if not, I can obviously explain in more detail.
Thank you,
Simon Mougin
Hello
Generally when you want to copy parameters from one part to another in Catia, you have to publish the parameters and then copy them with links. There the links will be kept between the two pieces.
Dimitri
1 Like
Hello, have you embarked everything in the optimized copy?
I usually group under the same body everything that makes up the copy (geometry, formulas, parameters).
What should be the behavior when instantiating the copy?
Hello
Thank you for your answers.
Frank, indeed my parameters + relationships are outside the body. The problem that arises now: when moving the parameters in the body itself, I lose the associated links.
The optimized copy works very well by copying the geometric sets.
The behavior during instantiation works very well, just that the parameters are no longer driven by the parameters located in the design tree.
I'm attaching a little more explicit video of my request/problem.
copie_optimisee.mp4
How do you move parameters and formulas?
To move it is first necessary to place a container "parameters" and "formulas".
To do this, you need the KWA module or if you don't have it, bypass it by copy/paste.
We create a part in which we add a parmeter and a formula that we then delete, once we have the empty containers we copy/paste on the Part Body and then right click on the parameters to reorder, same on the formulas.
In your video we don't see what you selected for copying? with the exception of the body of the piece and the points.
EDIT: I can read up to CATIA V5-6R2017 so if you put your file I can reorganize the hystoric to show you.
Ok, I understood the manipulation.
I "just" have to reassociate my parameters located in my part body from now on.
Not an easy task :(.
I tried your method and indeed it works. I find the parameters and relationships once the optimized copy is made.
Thank you
Normally, if everything is under the body of parts (volumetric geometry, geometric sets of "constructions", formulas, parameters, there is nothing to re-associate everything follows.
I understood the manipulation well but I can only copy and paste the relationships and parameters.
He loses everything afterwards.
the video as an attachment so that you understand the problem.
copier_coller_4.mp4
This is not the right way to do Copy/paste non-empty containers inevitably creates duplicate "parameters and formulas"
You have to copy and paste in the body of empty containers . That's why we open a new CATPart in which we add a parameter and a formula that we then delete, once we have the empty containers we copy / paste on the Part Body of the sprocket part, then right click on the parameters / "reorder" or "change geometric set", The same goes for the formulas.
Thank you very much!!!
Indeed it works perfectly!!
By the way, there are two tabs that are very convenient to use in optimized copy.
Input: allows you to rename the inputs with a more explicit name E.g. "XY/plan" to "Select plan support"
Parameters: allows you to "give the possibility to change certain parameters at the time of instantiation Ex: the number of teeth, the module etc.
Oh yes indeed it's ultra interesting to give the possibility to do it at the time of instantiation :)!
It's also more explicit, yes.
Thank you so much in any case. I lacked depth of detail about it.