Reference Behavior to Sketches with only one element

[Albigger]

I'm wondering if this is just how CATIA works or not:

Say I have a sketch, with only one element (a point, or a line), called "Sketch Name"

Now if I reference that element in another sketch, or for a hole, etc... the reference is "Sketch Name". Now I go back to the original sketch and add another element, another point for example. Well all the children of that sketch have to be re-linked to the original point, and now the reference is something like "Sketch Name\vertex.1"

So, if my sketch only has one element, why does CATIA link to the whole sketch, and not just the vertex within the sketch? I have wondered this for a while.

-- Jay

 

[catiajim]

Generally, linking to a vertex (or edge) of anything is a bad idea. CATIA tends to re-identify these frequently. Instead, in your sketch, set your point as an Output Feature (right click on the point inside the sketch and go to the Point Object). This will allow you to use the point outside of the sketch, and keep CATIA from re-numbering it when you add another point to the sketch.

Note: when working with vertexes and edges of non-sketch geometry, you will find more stability if you actually create an Extract element first, and then use the Extract Element.

 

[Albigger]

The output feature is nice, but is this required if I have a sketch with many points? Typically I have a layout sketch with the centers of many holes, and to create an output feature for each point seems somewhat tedious.

Are there other advantages of using output features?


Yes I have noticed a greater stability using extracts, and I do try to do that.

Thanks for your help.

 

[catiajim]

The biggest advantage to Output Features is stability. Otherwise, CATIA will renumber all of the vertices and edges when you add more geometry to the sketch.

 

[Albigger]

OK, so (playing devil's advocate here for a moment) why wouldn't CATIA by default make every sketch feature an output feature, so that it never had to re-number the items?

 

[Azrael]

If every sketch element would be an output feature then you would need to join them afterward to be able to use the domain .

The output feature capability is useful when you want to have multiple outputs from the sketch for different usage.

 

[itsmyjob]

to Albigger

For you original question I do have this answer...

The main purpose of a sketch is to define a Profile for a construction feature in PartDesign or GSD.

When the sketch actually define a possible profile: a circle. then CATIA will consider the complete sketch when you select circle.

If the Sketch does not define a profile, you do have a circle and a point (not construction element), then CATIA will not consider the Sketch as a profile and will use only the selected element for profile definition... (Sketch.1/Edge.1)

When the sketch does have element of the same dimension (curves and lines, not point) the sketch is considered as a profile, even is non connexe.

For a several point sketch you actually have to select the sketch in the tree, if you pick a point, Catia will select a vertex.

When sketch has element of different dimension (line and point) then catia will not consider it like a possible Profile.

You can eperience this in GSD easier than in PartDesign as PartDesign will need the Profile to be connexe and not self intersecting to actually be good for construction.

Eric N.
indocti discant et ament meminisse periti ​

 

[Albigger]

OK, this has all been very good information. It seems to me that I have been doing things the right way.

Let me ask this, if I typically have several holes or features, I lay out a "master" sketch with a point at the center of each hole.

Then I use this sketch to put in the first hole and pattern the rest. This seems to be working just fine for me, but is there a better way to accomplish this task?

 

[jackk]

I do the same thing, Jay. Works well especially if you define the first hole as a revolved shaft (or groove).