maintain time connection in sketches

[pulici]

Hello everyone
Despite use for years catia v5 one thing I still do not happen: how do I keep that sketch updated only to previous operations and not to the next ones?
I often happen to have to modify parts at some point of the tree but entering the sketch the solid that I see in the background is the final one, often in update, this generates errors like the update cycle and also makes useless the logical tree.
Perhaps the only way is to keep the sketches inside the body and not in a geometric group, but sometimes sketches are not related to a solid operation

 

[alexfunk]

Hello, (I hope I understand your question). make a copy (non-associative) of the sketch and go to change what interests you. alessandro

 

[gianni55]

Hi.

precondition that in order to avoid (always in ambush) updating cycle it is preferable to reduce the operations that create a reference with the solid to those indispensable and strongly desired as they will be effectively reused parameterically and that in the contrary it is preferable to use simple geometries such as plans or extracted and isolated (not yellow in the sketch). .

Here, take off the premise, if you really want to proceed keeping the sketches updated before, then (I think) that the road is what you said: keep the sketches in the solid:
in case you do untreated sketches not related to a solid operation, just click on the right button on the sketch and then "object - change geometric group" you can reorder it as you think by moving it from the solid tree.
If the sketch is linked to a solid operation and you try to change the geometric group the move generates an associated copy, so if you want to reuse it clean, do as said alessandro.

(of course we are talking about non-hybrid mode)

Let me know.

Hi.

years ago

 

[pulici]

Thank you both!

I am well aware that the links between operations involve additional problems during the change but I believe that they are indispensable to have a solid parametric, unlike for example nx where you work practically opposite.
That said my problem is not to untie a sketch but to keep it chronologically linked to the logical tree.
I believe at this point that the only way is to keep them in the body, because if I try to select it with the right button I can simply move it inside a geometric group, if I decide to place it in a body he will automatically go to the last position without a chance to choose after which operation to insert it

 

[gianni55]

it is true that it automatically goes to the last position, but it is also true that if you want to insert it after a specific operation, you just define (in the object of work) that operation and perform the feature, consequently the sketch will move into the feature you have performed, taking the position you want (and you can reorder it provided it is incorporated in the feature)

you can even delete the feature and the sketch will remain in the same position of the tree without going to the bottom (but you just need it to be there or at the bottom since the sketch is always selectable (visible or invisible) in any chronological position of the solid (while the subsequent features are not visible)

 

[pulici]

it is true that it automatically goes to the last position, but it is also true that if you want to insert it after a specific operation, you just define (in the object of work) that operation and perform the feature, consequently the sketch will move into the feature you have performed, taking the position you want (and you can reorder it provided it is incorporated in the feature)

Hi.
I always work like this, only that sometimes once an operation selects the sketch and with the right button I move it into the geometric group, for a purely matter of comfort because hiding the geometric group avoided to find visible sketches within the products.
In this way he makes an associative copy of the sketch but at the same time loses the temporality of his insertion, even entering us from his operation in the body and not in the geometric group.
In short, the only way is not to move the sketches

Thanks again

 

[gianni55]

if you enter the body key dx on that features with you define in the object of work, it keeps time.

but to hide (or display) all sketches (cracks, points, lines etc.) in the products without going crazy:

menu/modification/find/general/type, write to us: piano, then in "find" selections "visible on the screen" then select the binocular "find and select" and hide.

This command is very powerful, and allows you to do composite questions: tops + points + sketches or color layer etc. also allows you to choose the "depth" of research and selection, you can create favorite searches and customize it with a macro

 

[pulici]

if I move it into the geometric group and within the sketch I see in the background the final solid, also defining the operation as an object of work

the command finds to then hide can be useful but in fact you are making changes to the individual parts for which at the time of exit it becomes difficult to understand which file is to be saved for real changes and which for the cunning fact of having hidden the geometries

 

[gianni55]

Yes, it certainly does not have to be moved/associative copy, the sketch must be only in the body...

on the fact that only to hide sketches is identified as modification, unfortunately it is annoying, but in fact modification is, so either you remember in the rescue management or you pray san blessed by norcia of not having made trouble

Hi.

years ago

 

[micknat]

I have been working with catia since 2008... I find it very convenient to keep the sketches in geometric groups in order to be able to reuse them to taste. for changes: depending on what you want to do I can hide the body affected by the change itself. if I want to continue to see it, sometimes the duplic (without connection) and I only keep on the duplicate (which then I delete); If I need to take a reference from the solid final I take it from this, then be careful to eliminate the bond of coincidence created (the instrument of diagnosis of the sketch is fundamental), leaving the entity created there where it is (possibly putting quotas and constraints later).
In general, there are always a number of possible roads greater than one