Sketch error - Open profiles

[rbarata]

Hello, my friends

As an exercise, I was trying to create a sketch from this drawing. But I'm getting some errors of open profiles. I can't solve them using the "sketch analysis" tools. I getting suspicious that the drawing dimensions are not correct (but maybe that's the point of this exercise).

What do you think? How should I solve this?

Thank you.

 

[MrCATIA]

The drawing dimensions look OK to me.

The Sketch Analysis shows the inside profile is closed, but not fully constrained.

The outside profile is still in several pieces, so I would start by Trimming the two D16 circles. (the Quick Trim tool would be the quickest/easiest way to do this.) This should close the outside profile.

 

[rbarata]

The outside profile is still in several pieces, so I would start by Trimming the two D16 circles. (the Quick Trim tool would be the quickest/easiest way to do this.) This should close the outside profile.

I think I see how this works... since the circles are only used as a "support" to construct my sketch, Catia looks at them as two different pieces. By trimming the circles, what remains is just a line which is then considered as a single piece. Am I right?

About the errors, there were several associated to points. Once again, these points are not features of the part, they're just to support the sketch construction (same as before). So, by hidding them I eliminate those constraint errors. But I cannot do the same with the profiles show in the picture since they are features of the part: I cannot hide of delete them. Now, Catia allows me to create a pad but I don't understand why the features selected (in the picture) are under-constrained.

Thank you.

 

[MrCATIA]

I think I see how this works... since the circles are only used as a "support" to construct my sketch, Catia looks at them as two different pieces. By trimming the circles, what remains is just a line which is then considered as a single piece. Am I right?

Yes. But the circular arcs (after trimming) are part of the profile. Normally, a sketch must have a contiguous path of planar geometry (lines and curves).

About the errors, there were several associated to points. Once again, these points are not features of the part, they're just to support the sketch construction (same as before). So, by hiding them I eliminate those constraint errors. But I cannot do the same with the profiles show in the picture since they are features of the part: I cannot hide of delete them.

Points are used as endpoints and centerpoints, but points themselves are not part of the sketch profile.

Points and centerlines and other support geometry should be marked as "construction" geometry (dashed), not hidden. Construction geometry is not used to define the sketch profile.

Now, Catia allows me to create a pad but I don't understand why the features selected (in the picture) are under-constrained.

The Diagnostic page of Sketch Analysis shows the status of sketch geometry. It is not required, but good practice to always constrain all sketch geometry. This will "lock" the size and position of sketch geometry and avoid accidentally changing things. All sketch geometry should be green or yellow, not white.

For me, a good test to understand why something is under-constrained is to try to move it with the cursor. If it moves, it's not constrained.

The attached image shows the outside profile is green, so it's OK (fully constrained). The inside profile is not all green. I suspect the centerpoint of the R16 circle is not constrained 4mm below the centerline.

 

[rbarata]

Normally, a sketch must have a contiguous path of planar geometry (lines and curves).

And everything inside this continuous path should not be considered. I got it!.

I suspect the centerpoint of the R16 circle is not constrained 4mm below the centerline.

Yes, and also 40 mm above the R9 circle.

Thank you. Now there are no errors. Let's move to the next exercise.