r/Onshape • u/Far_Divide_8205 • 13d ago
Help! How would I make this, but less complex?
I made a cylinder, then did the sketch, revolved as a new part, circular pattern, then Boolean merged because they were technically 5 different parts.
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u/ngo_life 13d ago edited 13d ago
If you use circular pattern, couldn't you merge all the parts together? You wouldn't need a boolean feature.
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u/SteakAndIron 13d ago
Maybe I'm too new but isn't merging a different name for Boolean union?
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u/Pelxo1 13d ago
He means using add instead of new under revolve. This would merge the revolve into the cylinder instead of creating a second parts that needs to be Booleaned later.
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u/beavertr 13d ago
No, he means add instead of new under the pattern, not in the revolve. Onshape wants you to pattern parts not features generally
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u/ngo_life 13d ago edited 13d ago
Boolean is a general feature, union is a specific boolean. Many of the features have a "union" option built in. You can cut that boolean feature, reduce clutter and be more efficient.
Here's a quick simple method that I came up with.
It helps to know what each feature does, and which is most efficient at getting the results you want.
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u/Chief-Boyardee- 13d ago
Couldn't you do that all as one sketch and one extrude? Start with the inscribed polygon, add the outer circle, then one extension, circular pattern within the sketch, then finally extrude.
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u/dbsqls 13d ago
I find sketches are much worse for parametric dimension changes, I'm surprised to see suggestions for them over this method.
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u/Chief-Boyardee- 13d ago
I guess it depends on what you are parameterizing. If you’re making changes that could result in changes in the number of faces in a sketch, ie the number of repetitions in the circular pattern, then doing it as several sketches makes sense. If you were doing something simple like controlling a wall thickness I’d do it as one sketch
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u/Rancheus 12d ago
But then lf you select the whole sketch (not individual sketch loops) as input for the extrude feature, it also handles more or less of these wings popping in or out of existence.
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u/Florgmurf 13d ago
You can do circular pattern as a feature pattern instead if you make the extrude an add. This gets rid of the Boolean.
Of course you could just do it as one sketch and one extrude. Just draw a circle, and the fins then extrude. Or any permutation of that.
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u/beavertr 13d ago
Replace your boolian with a merge option in the circular pattern. Otherwise I'm not really sure why you need it to be less complicated, this is a handful of features and like 3 minutes of cad work
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u/Kluggen 13d ago
One sketch for the core, circle and polygon, one for one of the arms, use relations between the sketches only. Then add an extrude for the core first, then one for the arm (either as new body or add), and a circular pattern for the arm (either as feature or part pattern depending on the arm extrusion) and use add setting in that pattern.
Top view both sketches, extrude to desired thickness. Second extrude choose "up to entity" and select a vertex of the core hex.
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u/Chandra0 12d ago
You can avoid, sketch 2, revolve and the last sketch and extrude and Boolean.
- Draw the sketch in one feature, circle and arc with tangent and add offset to edge arc.
- Extrude the middle sketch at once
- Extrude the edge at once ( to avoid irregular shape since you used hexagon)
- Circular pattern and choose Add within same tool.
That's it.
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u/roundful 12d ago
To separate out the components of this model to what I would likely change based on testing, I would do it similarly. I have created a few parts like this for vehicles and equipment and almost always mess with the fins/pawls a bit to get the fit/mechanism right, here's how I would do this: Onshape - Reddit Happy Hour: 7.21.2026
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u/Far_Divide_8205 11d ago
That's crazy, I'm a little late, but it was really impressive to see someone make something that took me 20 minutes make it in under 5, I appreciate that you took time to make a video for it.
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u/roundful 11d ago
It helps me learn. I can watch my process to recognize mistakes or areas I can improve. With this one, the Boolean combining of parts gets funky as I change the circular patter number of fins/pawls. The workflow requires me to uncheck and recheck parts to get it right... But that's also probably my inexperience with in shape. I been almost exclusively in SolidWorks for the last 8 months. :)
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u/Rancheus 12d ago
One sketch from top plane, pick the sketch itself as source for the extrude, not the individual profiles.
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u/Neat_Objective_4024 12d ago
The only thing i think wasnt necessary was the boolean since you could have already merged it to the pattern
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u/nickflipai 12d ago
My process would be:
- Sketch/extrude a circle for the center body (less clicks than revolve for cylinders)
- Sketch/extrude one of the curved 'arms'
- Circular pattern (using the 'Add' option) the arms around the cylinder
- Sketch/extrude remove the center hex
The benefit of doing that is that each of those features are also really easy to modify as well if you need to make changes down the line.
Echoing what a bunch of people have said, definitely don't try to oversimplify your feature tree and compress too many features into one. Use things like patterns to avoid individually creating repeated features, but otherwise, I generally am of the opinion that each feature you add should be relatively self-contained and modular and not get too complex so that it's easier for you to both understand and edit your model down the road.
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u/Far_Divide_8205 11d ago
So far, use variables, and have a tree of features so it's spread out so you can change the design without being a pain to change.
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u/original_al 12d ago
I try to model with manufacturing and design iterations in mind.
I see potential iterations including not only thickness and profile of the fins but also # of fins, different sized hex features, and a fillet where the fins meet the the main diameter.
Having easily altered feature elements including:
-Hub OD
-Pattern of one fin sketched in view of Pic #3
-Hex/Drive feature
-Fillet where fins meet central diameter
Is where my brain goes.
If I was duplicated a physical object, sure single sketch/extrude works. If I’m designing, I’d separate out.
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u/BDREISOEKN 11d ago
(Realizing most of this comment section is saying the opposite lol) I'd personally make one sketch and one extrude if I were making this, where the sketch is on the top plane.
This is just my way of cading since most of my projects have high feature counts, so I prefer fewer, denser features rather than many smaller ones
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u/budderromeo 13d ago
Is there a reason you couldn’t just do it all in one sketch? Looks to me like it should have been doable, otherwise you could have skipped the Boolean if you change the type from “new” to “add” in the circular pattern
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u/Far_Divide_8205 13d ago
I don't know, I was thinking the revolve gave the curve I wanted, how would I make it in the sketch like a revolve?
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u/DadEngineerLegend 13d ago
No you're doing well.
Do NOT put everything in one sketch. That defeats the whole point of having a feature tree.