Reorder a Sketch in the Tree

[jzecha]

I use a lot of sketches for hole patterns and have always ran into this issue.

Is it possible to change the location in the tree or if its in a Geoset, the location in the tree it references when editing the sketch?
FYI, I design for a bunch of companies that do not allow the use of Hybrid Bodies, so that is not an option.

For example, I create a sketch after Hole 1, but now I would like that sketch to be referencing the part before the hole.
So when I edit the sketch, the hole is not in the part.

 

[LWolf]

Do you mean the sketch that Creates the User Pattern?... But it is consumed by the User Pattern Feature (and this feature is located below the hole you want to pattern?)

regards,
LWolf

 

[jzecha]

This sketch will be used for a User Pattern, but at this time it is not.
I created the Hole, then the Sketch, but to make the User Pattern work, I need to move the sketch before the hole and reference the hole location off of one of the points in the sketch.

 

[LucasC]

What do you mean by "but to make the User Pattern work, I need to move the sketch before the hole"? A user pattern is a transformation feature, it can't work unless the hole exists in the first place. I think you're trying to hatch a chicken before the egg has been extruded. It seems like you might be in an update cycle because your positioning the hole with resultant or projected geometry.

Steps I use for user patterned holes:

1) Create sketch with multiple points including the point(P1) location for the hole you want
2) Use the hole command, click the point within the pattern sketch (P1) to locate the hole, click the orientation reference and click OK. The hole is now located
based on the user pattern sketch. The hole sketch should only have a coincident constraint linking it to the pattern sketch, no dimensions.

so now if you want to edit the user pattern sketch, the hole isn't referencing any resultant geometry on the component, only the pattern sketch. You shouldn't need to edit the embedded sketch in the hole unless the coincident constraint is somehow broken.

 

[weagan22]

Adding onto what LucasS said, use a plane or other wireframe/surface feature to define your sketch so that it does not depend on a solid. Solids are notoriously bad at handling updates as all of the subsequent features depend on the brep name of the surface that was selected by the user and changes as the solid changes.

To answer your question more directly, you can 'Define In Work Object' farther up your tree and then select the surface to define your sketch on a surface that is farther back in the history to make the reference further up the tree and make it more robust. But at the end of the day this is still not nearly as robust as fully defining your sketch location by using a positioned sketch and selecting exactly where you want it located. Sketches are very powerful in CATIA but should be used sparingly as they are notorious for being awful to work back through when they break.

 

[jackk]

are you using the Hybrid Design mode?

 

[ali_elouajdi]

Hello
I do the same thing, but at first I create a sketch with a point to define the hole position, and after I create the hole definition which create it's own sketch, reordering hole definition or copy pasta from other bodies can create errors cause the hole definition keep the point position by it's own sketch even if you edit the first created one.