Thank you for your feedback
1) For "Repère3D-2 directions", you're right. Thank you for your remark.
2) Regarding the "Landmark/Landmark" coincidence, I either misunderstood or it is not possible in hybrid mode.
Is the coincidence constraint you're talking about really that of this icon 
?
If so, I can't use this constraint only with points, lines and planes but it doesn't seem to me directly integer axis systems even when trying to select them via the construction tree.
3) Otherwise something else
In the method "adding a 3D coordinate system in a component that is being relaxed", I noticed when I did the video entitled "softening" that the 3D reference point that was copied and pasted into the softened "component" did appear in the directory where my CatProduct is located.
On the other hand, the changes I make to my 3D coordinate system when I am in my assembly also have an impact on my 3D model coordinate system.
How do I proceed to use my 3D cues put in a component in a catproduct without the changes of a 3D cue having an impact on my 3D cue model?
In other words, how can I use the 3D coordinate system and duplicate them multiple times in a component without creating a link between my 3D coordinate system and the 3D coordinate systems pasted into my component?
I think I need to change the beginning of my manipulation when I use a 3D coordinate system that I put in a component. Before copying/pasting the 3D coordinate system into the component, I think I must first copy a 3D coordinate system in the assembly under construction. Then, you have to copy/paste my 3D coordinate system inside the directory that contains the parts and the assembly but not copy/paste from the 3D model coordinate system.
Thank you in advance for your help.
Hello.
2 ) Yes it's this constraint (try to create an assembly with 2 parts even empty in Normal mode) it's weird that it doesn't work (Note the message from CATIA in the inf command bar is incomplete) we can select "CATIA help extract" marker
3 ) It's normal you instantiate the 3D reference part (it's not a copy, the fact of having it copied / pasted in CATIA is a trick when the part is opened in scession) it doesn't make a copy of the part it avoids having to insert / existing component, etc..
If you want to independently modify one or more 3D landmarks, you must have created the "Before" files , otherwise you will have to replace the component (right click on the component / replace, uncheck all instances).
1 Like
2) OK. I'll try, though, can you tell me the options to uncheck to have the "normal" operation again?
By the way, I realized that I was good in hybrid but
1) not everywhere because the hybrid design box of parameters and relationships were unchecked
2) that the wireframes visibly go into the body and not a geometric set.
Is it interesting to keep this configuration for hybrid operation? I don't really know. That's why I created a post on the main families of options. I hope I can learn some good things about this even if my post (http://www.lynkoa.com/forum/cao/une-bonne-comprehension-et-gestion-des-options-dans-catia) is maybe a bit too general.
3) You're exactly what I wanted to know. On the other hand, I need a few clarifications:
- "If you want to independently modify one or more 3D landmarks you must have created the files "Before"" Quote Franck
--> Can you tell me exactly what operations to do to create the files "before" ?
---> Is it copy/paste the part at the level of the windows explorer?
---> In CATIA, does it mean to register as with independent copy checked (see "records management panel")?
-"otherwise it will be necessary to replace the component (right click on the component / replace uncheck all instances)." quote Franck
OK. Once the parts have been created before, I will replace them via component/replace to remove the 3D reference parts that are related to my 3D model reference part.
Thank you in advance for your help.
Good evening only the box "enable hybrid design in bodies etc .... "
3 )
First of all, when you create a file, the software assigns a UID, a unique internal number, this is the computer side (code).
If you save as or copy/paste (normal) the number remains unchanged "version".
If we create from , the internal number changes "revision"
In your case, the markers are not parts intended to be produced, so I would say:
Open the 3D marker.CATPart file; modify in the file properties its name 'ex refere3D-size10mm" then have the same name as the property saved under "the right directory".
To be repeated as many times as desired.
These are the files that will be inserted or replaced in the CATProduct
When you replace a file in a default assembly the box all instances is checked in your case you have to uncheck it otherwise you will always have a single linked 3D marker
1 Like
1) Do you know where we can see this number?
2) "In your case, the markers are not parts intended to be produced"
"> I don't really understand what that means. Can you tell me more about it?
In any case, if I understand correctly (with the handling with save as), the 3D coordinate system copied in the assembly directory should keep an identical number to the 3D reference model but this is not a priori annoying.
3) "Open the 3D marker.CATPart file; modify in the file properties its name 'ex refere3D-taille10mm" then have the same name as the property saved under "the right directory".
--> in this case, without making an independent copy, are we sure that the "3D coordinate system" copied into the assembly directory from the 3D model coordinate system no longer have any links?
Sorry, if I ramble a little, but I often find myself with problems in the recordings and that's why I try to erase all my doubts.
Thank you for your help
1 ) I think it's visible from the Smarteam PDM (not sure I don't know).
2) "Produced", machined, molded etc, your markings are just dressing, you are not going to make them.
3 )-> in this case, without making an independent copy, are we sure that the "3D coordinate system" copied (saved) in the assembly directory from the 3D model coordinate system no longer have any links?
Saved not copy , Yes these are different files with no link.
1 Like
Super. Thank you for your very clear explanations!
This post should soon come to an end...
But I still have a few small remarks.
1) A small detail: in the single coordinate system that I use in the "component + insertion 3D coordinate system" method, I realized that I had two axis systems. The first is called the "absolute benchmark". The second is located in the ordered geometric set and is called "3D Reference". I think that, for this method, there is only a need for a benchmark. The one in the geometric set is "historical", it comes from the unused method related to optimized copies. For the moment, I only use the "absolute coordinate system". Won't it be good to leave only the necessary elements in this 3D coordinate system inserted in a component? What do you think?
2) I am very happy with the realization of these 3D markers inserted into a component. On the other hand, for my use, I realize that I am missing one last key element to facilitate my configuration, namely "3D angular sectors".
To better understand this last element I need, here is the illustration below:
Do you have any ideas for building this 3D element?
The difficulties are :
1) that it will be enough for my parameterization, i.e. to adapt to the changes in values of my angle.
2) that we must remain simple as for the benchmarks so as not to make a gas plant and that it is simple to implement.
My first ideas are:
1) to make a curved wireframe element from the angle constraints
2) maybe to create an "angular sector" part that we would add to the component. to see...
P.S: I'll copy you the example
ang.zip
Hello
1 ) If it is not useful, you should delete.
2 ) Is that it ?
A CATPart " Angles " at the first level of the assembly will not work in the " softened " component.
Principle, we instantiate the optimized copy on the X(n) lines of the 3D coordinate systems.
Construction of the copy :
Create 2 lines (coincident on their starting points).
Create a geometric set under the first.
In his second set create :.
- 1 plane (by these two lines)
- 1 point on one of the two (see options on screenshot)
- 1 Sketch positioned (on the plan, no selection for the origin, H on the same line that was used to create the point.
In the sketch, the 2 lines and the point are imported as construction geometry.
We create the sketch " portion of camembert " (be careful to remove any horizontal and vertical constraints.
Yes, that's almost it.
The only thing missing is a shape to show the orientation of the angular sector.
Here's what I'd like to build:
A 3D curved arrow should allow me to represent my oriented angular sector.
On the other hand, it would have to be thinner than the one I drew.
Do you have any ideas to build this style of elements and arrange it as for the landmarks in a component in order to separate what is assembly from what is packaging?
Thank you in advance for your help.
Hello
The PB if the angle goes to zero it won't do it and if it's 1 or 2 ° the arrow won't be visible.
I'd rather draw something like this 
On the other hand, on your screenshot there is an error.
It is not a simple rotation of a coordinate system but a rottation plus an inversion of the blue and green axes in the second coordinate system ( ? )
OK Thank you for your remarks.
1) Indeed, I think you're right. For the precise location and configuration, I think I'll export wireframes and finish my cinematic diagram under video.
2) For my benchmarks, I had done this quickly and there is indeed an inversion between two axes.