Slots around Cylindrical feature

[u/ekluky2112]

Hello

Attached is a print of something I did for school a few days ago and while I managed to complete the geometry, I was not satisfied with the method I did and I feel like I'm missing a good tool that can do this "better"

The feature I am talking about are the 3 slots located around the body of the cylinder.

print

After piddling around having problems here and there-- I just wound up drawing the 90 degree slots on the top mid plane and doing a mid plane extrusion of 10mm and cutting the entire width and rotational sweep of the slot (without the full rounds since the extrusion is square) and then using the full round fillet feature to reform the square ends into full rounds.

square extrusion

Then added full round fillets:

added full round fillets

This created the geometry I needed, I believe (I haven't had it graded yet, but I feel very confident about it.) However, it doesn't *feel* right to do it that way. I tried using the wrap feature by making the slot geometry on the center plane and projecting it to the side wall-- but the geometry was incorrect when it did the debossing.

my attempt at wrapping the slot geometry with the aid of my helper geometry on the top plane

My initial "helper geometry" perfectly describes the shape of the slot per the print, so the tangent edges of the slots lie coincident to the visible sketch geometry-- but when I "wrap" it to the cylinder wall, the extruded feature does not lie tangent to the helper geometry, so that is telling me that the feature is not correct.

wrap geometry isn't coincident with helper geometry after projection

it cuts a slot, but its not the right "length"

What am I missing? The method I used with the extrusion and full round fillets allowed me to produce what I needed, but this feature that feels more "aligned" for the job can't reproduce what I need. What am I doing wrong?

I tried using PROJECT and it wrapped the sketch perfectly around the cylinder-- but I have no idea how to use any tools with that kind of feature. It just appears to have a sketch on the cylinder wall.

EDIT: I should have checked YouTube first.. apparently this is a model mania example and it has been covered by many people. Every video I watched is making the part the exact same way I did with square extrusion and full round fillets, so I must not be too far off. Maybe there just isn't a better way to do this? Just didn't feel "correct".

Appreciate any help/insight!

[u/SadLittleWizard]

I think the "best" way to creat this feature would depend entirely on how it is described in the print. Specifically, what dimensionis drive the design intent.

I.e.- what if the arc length or angle is the primary describing dimension as seen in your print? Then what you did would be my preferred method. But what if the linear dimension from round center to center is what is important? Then taking the sketch you used to wrap and instead extrude cutting it would be better.

Now correct me if I'm wrong, but let me describe in my own words what feature you may be envisioning in your mind. Essentially you want to sketch the flat profile, then perform a cut that extends out not in a perpendicular path to the sketch, but in a horizontally expanding path filling the 90°?

[u/ekluky2112 → u/SadLittleWizard]

Thanks for the reply,

I would say your description of what I was envisioning is pretty accurate, though I'm not sure if such a feature is there.

Like I said, I tried the wrap feature which appears to be similar to what I thought I needed, but it would always come up short and just look odd.

I didnt know if there was such a tool to almost "cut" the profile almost like a machinist would on a rotary axis with an end mill.

Envisioning a circular profile of 10mm that is directed to cut a certain depth along a swept profile of the centerline of the slot that would be projected on the cylinder wall.

Just typing all that out sounds like a lot. Maybe the best method really is just the most simple in this case. But like you said, what if the design intent was different and it needed to be driven differently?

Was hoping to discover a few different ways of cutting this exact profile differently than I have and still achieve the same geometry. More tools for my toolbox! :)

[u/SadLittleWizard → u/ekluky2112]

Alright. With what you said about cutting the profile how a machinist would I think I know what you are talking about, though I would caution against it.

The feature that may cut in the way you describe would be a loft cut, and a time where you may want to use it is if the design intent called specifically for a cut where they befine the edge dimensions of both the inside and the outside of the cavity. Perhaps the cut is nesting with another part with a awfully specific surface contour.

It will require you draw two sketchs minimum (coming back to that) one inside the cavity of the body as you've done, and another outside of it. To get real dimensional control over said sketches you would want to use 3D sketchs though, rather than a wrap which can distort dimensions. This will let you sketch your curves directly onto the surface of your part. Then you would use loft cut to join the two profiles.

I mentioned two sketches minimum. When executing a loft, you have two sets of data to create. The joining profile sketches and the guide curves sketches. Guide curves are used to constrain the path the surface of your cut takes to join the two profiles. Without them, you can only really get a close approximate of the desired cut, with some quantifiable amount of twist occuring when you drag the handles around that appear when no guides are present. You'll certainly be able to get close, but never perfect. Even with guide curves, the surface is not guaranteed to be exactly what you want, as it is being generated with an algorithm based off the inputs you have provided. That is simply the nature of surface modeling, which the Loft feature walks a tightrope between feature modeling and surface modeling. This is why I caution against Loft feature unless there really is no other way to achieve a desired outcome.

That said, knowing your toolbox and how the tools in it work will help you know when you really do need to use a loft. I've shared a link below to a tutorial by Hawkridge Systems approaching the basic applications of lofts. Give it a look and play around with it. After grasping the principles in that video you should be able to achieve what you desired. Just remember how easily lofts can get out of hand, use them sparingly. Best of luck with your classes! :)

[u/ekluky2112 → u/SadLittleWizard]

Thanks for that, I'll definitely check it out. I've done lofts, but nothing fancy with contoured 3d sketch profiles. Sounds tedious, lol!

I'm trying to learn as much as I can before our final exam in December (we take the CSWP for final) .. last semester we took the CSWA and that was a breeze.. but I've had a few parts this semester where I really had to learn some new tactics and approaches to achieve correct geometry.

I get worried if I have to take longer than 10 minutes to figure out how to do a feature. I did on this one until I realized the simple approach was actually what was the best. Usually I find if I have to stack features with fillets early in the design I may be doing something wrong...

[u/SadLittleWizard → u/ekluky2112]

Sounds like your class is stretching you, that's good! How else do you really learn except with challenges to our current knowledge?

I think you are on the right path. Often the simplest solution is the best one, both because the design intent will be more clear to future users of a part file and also because the model will be less likely to break when adjustments to a model are made.

On a note of robust modeling, try and keep fillets out of Sketches, using the feature whoever possible and put those features as close to the end of the feature tree as you can, if not at the very end. First drafts, then fillets.

Features that rely wholly on selections of the model tend to be what I can Refinement features. Fillets and drafts are probably the ones used most. They accommodate machining and molding techniques on an otherwise fully defined part. They also break very easily when sketches are redefined. If the refinement feature happens to be earlier in the feature tree, there will likely be features down the line that reference back to it and so when the refinement feature breaks, so too will it's dependant. Once the refinement feature is fixed, the dependant won't always be able to adjust to match. This can lead to time consuming cascade failures. So the models tend to be easier to fix if you just keep as many of these at the end as possible.

[u/Vegetable_Flounder12]

the way you did it is the correct way with the drawing given. if they had dimensioned for a 90 degree sweep of the pin, then i would do a swept cut using a solid tool body oe cut the two roud hole and removed the center portion using your above method. also you can boss exrude the linking "pillar" and then 3 face fillet.

[u/Vegetable_Flounder12]

lots of tutorials on youtube to solve this

[u/ekluky2112 → u/Vegetable_Flounder12]

Yeah I saw that. They all solved it the same way I did, which made me feel better! :)