Ribs in Sections

rmb on hatch, crosshatch properties..., select "none" & apply to body

To which I would add: convert the edges (into the drawing, each view behaves as though it was a sketch) of the lines representing edges of the body other than the rib, which define the outline of the area(s) which (I assume) you still want hatched. Add lines and fillets at the junction of the rib with these solid hubs, rims, or whatever; the places where the part being sectioned suddenly gets thicker. These can be sketch lines, but if possible add relations to hidden features or sketches from the part model. If you temporarily go back to the part's feature manager and RMB "Show Sketch" on a particular sketch, you can show sketch geometry from the part in the drawing. (You will also have to turn on the global "Show Sketches" in the drawing.) Remember to RMB "Hide Sketch" in the part before you finish, especially if you want to save a dxf version of the drawing, otherwise the lines will mysteriously reappear.

Once you've got a closed contour of sketch lines in the drawing view, you can use "area hatch" to hatch the interior of the contour(s), leaving the thin rib section unhatched, so it looks like a "proper" drawing.

Haven't explained this very thoroughly, so please come back if I've been unclear.

Thanks Kenneth, but all that did was remove the hatching. I do want to retain the hatch in the parent solid. Just remove it from the rib profile.

ooops, i was thinking more about the weld (separate or multi-body part). my error.

check out what andrew suggested above, kind of a pita though.

I think the best way doing it is making the Rib as a diffrent body, then you can right click the hatch-->hatch properties and select none.

Akiva Litinsky CAD App. Eng. Systematics - Tel-Aviv - Israel

Brilliant !

Good example of how habits, formed during the years before the option of multibodies, have become ingrained. I remember thinking when multibodies were announced that some of the subtler ramifications would take years to discover.

What I understand you to be saying is to simply uncheck "Merge" when creating the rib (I never use the rib feature, but I presume that's an option) When I reflect on it, I've used similar methods (as I'm sure many of us have) to model, say, deep groove ball bearings as single part, bearing in mind they're purchased as a single part- here again, this allows a section through the balls to a) show their outline separately and b) not to hatch them just as for a rib

Always presuming, of course, that we have edit access to the original part... If not, might have to resort to the PITA method I suggested

Thanks for that, Akiva

Unfortunately that is not allowed, there is no merge check box available when you create a rib with the rib tool (logical if you think about it). Andrew's methode is the only resonable solution that I have found to depict webs in drawings.

Thanks to all for the suggestions. I tried Akiva's approach this morning and it seems to work well. Although there is no option to "don't merge" when creating the rib, I was able to "split bodies" after adding the rib to create a multibody part. I was then able to un-hatch the rib area in the drawing. Like Andrew, I have been doing it the "old, pita way" of sketching new boundaries & rehatching. This is MUCH better.