Sahaj Panchal's Blog

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Use non-connex elements from sketch in 3d–CATIA V5

You can create more than one guide curves, even profiles in a single sketch.

I am referring here features which support selection of two or more guides and/or profiles (solid modeling or surface modeling). Let’s have a look at an example.

The example contains two sketches to be used as cross-section profiles for multi-sections surface (red and green) sketched on same plane, different sketch feature, and a guide curve (blue).


So creating a multi-sections surface results in this, with correct coupling direction.


The ‘tip’ part: Instead of creating the profiles in different sketch feature, I can sketch them in a same sketch. But then selecting it while creating the surface will result in an error that the selected element is a non-connex element. Simplifying this, the software is telling me that the selected sketch is not point continuous, it is having gaps between sketch entities. So what now?

Here’s the answer: Create the profiles in the same sketch plane(ZX), same feature, with a guide in a different plane(XY) as shown. Make sure to create the guide such that it intersects with the profiles. Edit this profile sketch, and create an ‘output feature’ from any of the sketch entity, say the arc.


  • Tools toolbar > Output feature tool
  • select one entity
  • do the same for the second entity

Exit the sketch. This is the result(guide curve not shown).


Now you can use this two output features as two different profiles, like they’ve been created in different sketches!

Note that you can apply this technique to guide curves as well if they share same sketch plane and in each feature which lets you select more than one guide and/or profile.

Extending this capability further, you can use the two or more profiles/guide curves to create any number of features. One output feature in a multi-sections surface creation, the other in swept surface, as an example.

What if the guide/profile is made up of two or more sketch entities, say a line and a tangent arc. Well here the output feature doesn’t work the same way, as it can only be applied to single sketch entity. Instead you can use the Profile feature tool which lets you select more than one connected sketch entities.



Even while creating this features, you can name them, select a unique color if required, and perform different continuity checks as well.

That’s it! Thanks for visiting! Come back soon for more!Smile


One response to “Use non-connex elements from sketch in 3d–CATIA V5

  1. Girish April 20, 2012 at 11:19 PM

    Many thanx for the solution !!!

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