By Scott Henderson
You’ve built your surface and the hard work is done. The shape looks good. Every bend radius is correct and all of the fillets finally mesh well. There’s just one last step: Thicken the part.
And now the real fun begins.
When it comes to solving problems, start with the easiest method first. If “easy mode” works and it takes care of the problem, you’re set. If not, no big deal – it only took a brief moment to try.
Part Design Thickness
If the ultimate goal is to get a thickened, solid part, head to Part Design and use the Thick Surface ( ) command from there.
For most simple and well-constructed surfaces, this’ll get the job done.
If it’s not going to work, we’ll know pretty soon by the error messages that’ll pop up.
If the offset value isn’t necessarily set in stone, sometimes a smaller number will allow the offset to be created. If that’s not possible, then we’ll need to find other solutions.
Generative Shape Design Offset
If Thick Surface doesn’t work, the usual next step is to head to Generative Shape Design and use the Offset ( ) function. There are extra options with this command that can help us out.
If just switching commands is enough to offset the surface, then you’re almost done. Add some surfaces around the borders to close things off and you’re ready to go.
On the other hand, if the surface still can’t be offset, try playing with the smoothing options. These can allow the offset value to be imprecise, giving us a bit more leeway to create the surface. It looks like with this model, there are some areas in particular that just can’t be offset.
From here, we’ll have to do things the long way. The next move is to allow CATIA to skip any surfaces that it can’t offset. Typically, just by previewing the offset, CATIA will ask to remove the erroneous sub-elements.
The good news: There’s an offset! The bad news: The offset surface has a few holes in it and these gaps will need to be manually patched.
In this particular model, it looks like most of the surface has been offset pretty well. However, there’s an edge in the middle of the offset that’ll need to be cleaned up to help create a nicer surface later on.
We can use a spline and a split to remove the excess shape between two corner points, then Split the surface with the new spline to clean the edge. To ensure the spline sits directly on the surface, the “On Support” option is checked with the light blue surface selected.
With that done, it’s time to add Connect Curves. Ultimately, these’ll be boundaries for fill surfaces. The goal is to create a clean contour line for a smooth shape. Other wireframe tools can be used for similar results, too.
Once the curves are in, we’ll build three Fill Surfaces which will nicely finish off this offset.
To completely close the outside edges… you guessed it: more Fills.
We’ll add some Lines and Boundaries, then fill in the remaining openings at the edges of the model.
With that done, everything will be connected with a Join to create a final, singular surface.
Then as a very last step, we’ll head back to Part Design and fire up Close Surface ( ) to create a solid shape from the surface. Success!
Future Offsets
Of course, varying shapes will require different approaches. But, start with the easy options first, then dig into the complicated options if needed. Using Fills is a common approach to fix open gaps, but with all of the surface and wireframe tools in CATIA, there are a multitude of potential ways to tackle these issues.
If you find yourself needing more information about Splines, Connect Curves, Fills, Joins, etc., then the Rand 3D Introduction to Surface Design and and Advanced Surface Design classes are good resources. You can even find more info about the Close Surface and other surface/solid integration tools in there, too. Happy offsetting!
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