Hello
I want to set the characteristic dimensions of the parts that make up my mechanism (an assembly). To do this, all the dimensions of each of my parts were parameterized. These so-called geometric parameters associated with the characteristic dimensions are inside my parts.
Note: I am talking earlier about the geometric parameters associated with the parts, to be distinguished from the position parameters which are those associated with the assembly constraints.
My concern is that I don't have a global view of all my geometric parameters. I need to open each of my rooms to see the one-room settings. It would therefore be interesting to create a copy of all my geometric parameters at the assembly level and link them to the geometric parameters contained in each of my pieces. This is the point that I experimented with copying on two assembly cases to see the impact of bringing the parameters back to the assembly level.
What do you think of this solution of bringing the parameters associated with the parts back to the assembly level?
What would you recommend for managing the parameters associated with the parts of an assembly (in other words, the geometric parameters)?
Thank you for your feedback.
assemblages.zip
Hello.
I prefer the Assemblage.1 solution after a few modifications!
Instead of associating by formula in the CATPart the user settings and the external parameters I would rather make a " replace on the user settings" by the external parameters by checking the box " delete ....... ": It is useless to keep the user settings of the CATPart and the External Settings of the CATProduct duplicated.
Why I don't like the Assembly solution.2 :
This is not a link between the user settings and the Excel table (it is a relationship in the CATProduct)
If you are only logged in, for example " Part1_assemblage2. CATPart »
With edit/link, Catia confirms the absence of a link.
If you change the parameter to 10mm for example that you create a geometry (a point or something else is just so that you are sure that it is the same part that you will see in the assembly) then you save.
You close the file and then open the assembly
The part will have the geometry modification but the value of the parameter will be the same as the value of the Excel table configuration.
In other words, if you modify out of context, the modification is not reflected when you open the assembly, it is the value of the table that overwrites it.
In solution 1 this is impossible, we can only modify the external parameter in the context of assembly.
1 Like
Hi Franck,
Once again, you answer my question perfectly.
Exactly, I felt that the assembly.1 solution but there was some cumbersomeness with these external parameters and the part parameters.
By the way, the external parameters appeared automatically when I created a formula linking an assembly-level parameter to a part-level parameter.
Regarding your remark, I didn't manage to implement it because of the "replace on the parameter" that I couldn't find.
Can you make me a short video so that I can be sure I understand you?
Thank you for your help.
See you soon
Just point to the parameter with the mouse right click / in the list there is the "replace" function you click on it and then you point to the parameter under the external reference tab.
Yes, they appeared when creating formulas
{but you can also do the same thing by copying the parameter into the CATProduct and then activating the special paste part as a result with link}.
Edit: {_} Error on my part copy/paste with link of a parameter from the CATProduct to the CATpart is not allowed.
Hi Franck,
Sorry if I'm a bit heavy at the time but it doesn't seem to work...
In fact, replacing it can only be done on the "external parameter" and not the other parameter on the part.
However, if I replace the external parameter with the other parameter on the part, it seems to me that I lose the link with the assembly parameter.
Youngest child
Are you active on the CATpart??
Watch video
remplacer.mp4
Hi Franck,
I clicked 2 times on my part to make it active and set the work object on my part as well.
So I manage to run the "replace" command on the external setting. So I can ask to replace the external parameter with the user parameter. But, I think that's not what you wanted me to do but the opposite.
On the other hand, I can't run the "replace" command on the user parameter. In fact, I run the "replace" command but no window appears in this case. So I can't do the "replace" command in the sense you recommended, namely "replace" by selecting the user parameter and asking for the replacement by the external parameter.
In copy, I put a video to show you what I do.
videomethodeassemblage.mp4
Hello.
In V5-6R2014 it works (although from my point of view it shouldn't !!).
It doesn't make sense to "Replace" something that isn't being used.
I think if you use the L1 user parameter in a "function", the "Replace" command should work.
For example, you create a straight line (direction point) with the End condition "L1" after trying to replace L1 by L1 (External Parameter).
Perfect, it works!
So, for my part, I only have external parameters used to define it and these external parameters are defined from user parameters defined at the assembly level.
That suits me well. On the other hand, there is a small point that would be really practical but I don't know if it's possible.
With this method, the external parameters in a part are defined from the user parameters at the assembly level. The good thing about this method is that you have a list of all the geometric parameters of the parts grouped together. On the other hand, it implies a disadvantage in my opinion: if I want to modify a geometric parameter for a part, I will have to get out of the part and go back to the assembly. In other words, the geometric parameters of the parts will only be accessible by putting themselves in the assembly and the definition of the geometric parameters is done only in one direction: from the assembly to the parts.
Would it be possible to allow the definition of parameters in both directions? In other words, would it be possible, in some cases, to enter the definition of the geometric parameter directly in the part. For example, if the user parameter is entered at the assembly level, then the external parameter is defined in the part. But, if we change the external parameter in the part, then this time it is the user parameter in the assembly that is changed.
Thank you in advance for your feedback.
Hello Yes there is a solution but be careful it works when working with the CATProduct open in session
Otherwise if we open only the parts we find ourselves in the case: (Why don't I like the solution Assembly.2 :).
The solution is to go through the "Equivalence" function
equivalence.mp4