Here's a simple challenge for everyone. Use your favorite CAD software to model this part. We're not looking for the fewest features - we want the best way to model this (in your opinion). Please include the history tree when you grab a picture of your model so we can see how you did it, Thanks to Anath Mech for the drawing!
(ignore the mounting holes in the flanges)
I started with one simple parametric base sketch that will be shared across multiple features. It contains most all the constraints so changes made here will propagate throughout the model.
Two revolutions from the base sketch.
Then a sketch for the sweep profile. The base sketch was shared for the sweep path.
Finally the 15mm radii were added at the ends of the sweep.
 I used Inventor.
Or maybe it looks more like this. (I noticed the absence of the diameter symbol on the 225mm dimension.)
Done in a similar manner as the model with the round flanges.
Interesting Base sketch, Bob.
Good catch on the missing Ø symbol. The original drawing shows hidden lines for mounting holes (but no dimensions), that only work with square flanges.
Which CAD did you use?
Here's my CATIA V5 version of the Elbow, with square flanges. Similar modeling steps as Bob and Steve, but I mirrored the top flange to make the second one. I also like to add holes at the end.
I especially like the mirroring of the flange. Innovative!
Mine was rotated and stretched to get the round tube
I don't know, it's okay to do this, I don't understand very well.
A 45° revolve forms the curved bit.
The top flange is Extrude1. Extrude2 is a Derived Sketch so the bottom flange always matches.
I don't usually stack sketch profiles (i.e. circles and squares) in a single sketch to get two features for one but it made sense in this case to form the 88mm bores along with the flanges.
Nice to see you again Fred! And thanks for contributing to this challenge. Are your flanges square or round?
Thanks. I stop by from time to time to see if GC has turned around or is maintaining a downward spiral.
My first attempt had round flanges but they made no sense as a bolt would never fit. Then I saw Bob's post regarding a missing diameter symbol so I made a few edits to the extrusion. Squares make more sense.
I post weekly challenges for some of my co-workers and figured I'd see what's happening in this group.
can you share your challenges with us?)
which software, Nathanael?
Looks good Jeroen, but don't forget to round-off the flanges
(corrected spelling of Jeroen's name)
If you write my name correctly I will fix it ;)
I didn't model the round-off on purpose because I did not see them on the drawing. Or as my dad always says: "A single view is not a drawing."
That is Solidworks. But with a CATIA/FreeCAD type backdrop. :)
Sorry about the spelling - I corrected my mistake.
I thought you skipped the R10 round-offs, but I see them if I look closely at your model. Again, my mistake, and no fix required.
Does your Dad always draw more than one view for flat parts like gaskets?
The spelling is alright man, I'm already happy that you are giving feedback.
I prefer to have one more view than to miss a mate or feature. In CAD you can fix this by adding another view without a lot of trouble. But when my dad learned to draw it went something along the lines of; catastrophic mistake = bin = redo the entire thing by hand. I think this is especially true in a single-view drawing because piecing together what a mate/feature is can be very difficult (at least more so than in a multi-view drawing). So I think that's why he said "A single view is not a drawing." when he looked at this monstrosity.
After digging through my drawing book I found these pages, they are in Dutch but the image clarifies it enough I think. (?)
So according to the book you can "save" the original drawing by doing something like this.
Please let me know if I did something wrong.
I would create the drawing a bit differently. This isn't to say yours is wrong. No doubt an ASME 3rd angle perspective is "wrong" to everyone outside of the United States.
The one part I don't understand in your drawing is the "bottom" auxiliary view. The extra lines extending beyond the center-line confuse me. Why does the "top" auxiliary view not have similar extensions?
The other change I propose is the angle of the cross hatching for the section view. Most software defaults to 45° so the hatching at the bottom of the model ends up parallel to the model which is to be avoided.
Your drawing is certainly a lot clearer to read. The Dutch drawing system is a bit odd. We use the American viewing system but everything else is DIN/ISO.
The lines you saw on the bottom auxiliary view were supposed to be dimensions. since this wasn't very clear I changed them.
So if I stick to the partial auxiliary views you get something like this;
feedback is very welcome.
This looks great.
I see how I misread the dimensions in the prior drawing as being a portion of the auxiliary view.
I love the thicker lines used in this version for the part edges.
Rotate the section view cross hatching so it's not in-line with the bottom of the part and I'll give it two thumbs up ;)
Here you go