I would like to put the parts contained in an assembly in groups. In other words, to have a more synthetic and clear shaft, I would like to arrange the parts of my assembly in groups. On the other hand, I would like to do this without creating subassemblies that make constraint management more difficult and updates longer.
I believe that there is an element to this effect that makes it possible to: - group parts in an assembly (only at the level of the construction tree) - without creating subassemblies in the directory that contains the assembly and parts.
Would you know this element and how I can create it?
in SolidWorks you right-click on a part in the assembly and you create a folder and name it whatever you want. After that, you can put all the pieces you want in it. It doesn't work in Catia or is there nothing similar?
With Catia you can create "Components" in your CATProduct. They will allow you to classify PART without creating an associated file; On the other hand, you will have the same problem of managing constraints.
I would add just to make it easier to reorganize an assembly internally I am changing the following CATIA options.
1 ) Allow drag/drop.
2 ) Glue "Tjrs" components with assembly constraints.
One must not forget to make the component flexible, otherwise the constraints of the parts created before the part is moved into the component will not work.
As discussed earlier, I come back with a test case.
The softened component works very well. It allows me to store parts in this component and leave the constraints at the level of the parts only and not the component (see the example Test2-Test3 which works).
By the way, to do this, I don't do the option Paste components "Tjrs with assembly constraints" (for my specific needs). This allows me to keep the constraints between parts placed all at the level of the product. This is very useful for doing a link recognition in DMU Kinematics.
Otherwise, even if this relaxed component works, I still have to see if it is not possible to automate the procedure.
Indeed, once I have added the components and dragged the parts into the components, the constraints are put in warning (exclamation mark in a yellow circle). It is therefore necessary to redo the constraints (see example part 2). This is done quickly because I had created my constraints from publications. Nevertheless, wouldn 't there be a method to create the components and put the parts in the components without breaking the constraints?
Hello indeed if you don't want to move the constraints in the components but leave them at the level of the head ass you should not select the option Paste components "Tjrs with assembly constraints".
As a result, the constraints will fail and then either you redo them or you reconnect them ( plus button).
No choice (the ideal is to organize the parts in the components before creating the constraints).
It is therefore necessary to better make the constraints between the parts after creating the flexible components.
On the other hand, the problem I have just noticed is the following. In this case, when you want to create a constraint between 2 parts after creating a flexible component, CATIA does not allow you to select the parts only the components because CATIA selects only the components.
How then can we create the constraints between 2 parts when the flexible components have already been created?
The fact of softening (a component or a sub-assembly) allows to create constraints with the external environment. You want to constrain two parts of the same component while having the constraints under the head assembly (right)?
Don't ask me where this behavior comes from?? but to be able to do this you have to select by holding the Ctrl key the two elements to be constrained before selecting the type of constraint.
I would still advise you to have a "FIXED" piece of molding at the level of the head assembly.
No, it seems to me that what I'm looking for doesn't quite correspond to your reformulation. The Ctrl or no control was not effective for me in the two examples described below.
So, I'm going to try to clarify my need.
EXEMPLE1: Let's take 2 parts (part1 and part2) respectively in 2 different flexible components (component 1 and component2): - part 1 in component 1. - part 2 in component 2. At this point, I can't create a constraint between the 2 parts because only the components can be selected.
EXEMPLE2: Another example, in my component 1, I have my built part that I would like to fix. I can't put a constraint of fixity on my built part. Catia wants to force me to put my fixity on the component. I'll leave you an example attached.
1) Can you give me feedback with these new elements?
2) On the example in copy, do you stop to put a fixity on the frame contained in component 1?
EX 1 (no PB) I create the constraints key Ctrl then I select the type of constraints
Deactivate the hybrid mode, maybe the PB comes from there?
EX 2
As I said, the part or sub-assembly must be under the head assembly, in any assembly there must be a fixed reference (this fixed reference cannot be in a "softened" component).
