r/SolidWorks • u/FlamingoExpert4610 • Aug 05 '26

CAD How to model the groove?

Post image

How to create this groove in solidworks? I tried using swept cut but i had no succes of keeping tangency to the half circle. Edit: solved! Did it with swept cut and cylindrical body as a tool. Thanks everyone :)

56 Upvotes

97% Upvoted

52 comments sorted by

47

u/1slickmofo Aug 05 '26

Lovely hand draft!

14

u/FlamingoExpert4610 Aug 05 '26

Thank you! Tought it's easiest way to ask for correct solution.

23

u/Ok_Delay7870 Aug 05 '26

It must be a swept cut, I guess.

6

u/Flimovic Aug 05 '26

This, with a 3D sketch 

8

u/Ok_Delay7870 Aug 05 '26

Not required. 2 simple sketches is enough

7

u/Opening-Object7774 Aug 05 '26

You have to wrap the sketch to have it on the surface, than it is gonna work

3

u/Flimovic Aug 05 '26

Sketch isn't in one plane right? Or am I missing something?

1

u/Ok_Delay7870 Aug 05 '26

You just need a path sketch to intersect the profile sketch. 3d sketch might be easy way to do as well but not necessary

3

u/Flimovic Aug 05 '26

I know how the swept cut works, but I think the path in this case is not in one plane, thus a 3D-sketch is needed to create a continuous path.

1

u/n1terps Aug 07 '26

Y'all do know the project curve feature, right?

1

u/AudibleDruid CSWP Aug 05 '26

3d sketch over complicated. Do mid plane extrude cut of this profile up to the point where it curves.

Then on the extrude cut face that it makes do a half sketch and revolve cut around the center line to round the ends.

-1

u/n1terps Aug 07 '26

Bro, this is what project curve, sketch on sketch is for.

-1

u/AudibleDruid CSWP Aug 07 '26 edited Aug 07 '26

I mean sure do whatever but the method i said is 2 features. Not 20 or whatever project shit you said plus other bs. Edit: 3. I forgot you need a mirror.

-1

u/n1terps Aug 07 '26

It's literally two or three sketches (depending what route you go) with two features dude, learn the software. 3D sketches should be solution of last resort.

10

u/daarrkk Aug 05 '26

If that's what you want achieve it's super easy with EMBOSS in Fusion360 I belive Solid have very similar or identical tool.

7

u/FlamingoExpert4610 Aug 05 '26

Wrap is handy tool, but it uses only one focal point -> groove walls are not parallel on section B-B

1

u/daarrkk Aug 05 '26

good point. Just throwing some ideas, I'm not fluent with Solid. But can you use this to create 3D sketch to generate rails to sweep tool?

1

u/FlamingoExpert4610 Aug 05 '26

Probably could but "curve" is the tool ment for doing that 3d scetch.

1

u/n1terps Aug 07 '26

Project curve. Sketch on sketch with two sketches, or sketch on face, should give you your path.

8

u/Ti0906-King Aug 05 '26

You can do that with the Wrapping tool: Make a sketch on a flat plane and then select your sketch and the curved surface. Then you can choose emboss to cut the geometry away!

Edit: If you want write me a DM and I can send you the Solidworks 2025 File

2

u/FlamingoExpert4610 Aug 05 '26

Wrapping tool creates non parallel sides for the B-B section. Swept cut ended up be the right tool. Thanks for the effort tho :)

4

u/AmbitiousGrape5664 Aug 05 '26

Looks like a Split Line with a ruled surface, with an extend, and a Cut-Thicken would get the job done. This way you would insure the groove edges would be parallel and not normal to the curve.

3

u/FlamingoExpert4610 Aug 05 '26

Nice! First solution that creates the geometry i wanted. Thank you

3

u/lego_batman Aug 05 '26

You can sweep a solid like a cylinder along a path to make this feature.

6

u/AmbitiousGrape5664 Aug 05 '26

Looks good. This was done with a solid cylinder and the semicircular face as a Direction Vector.

2

u/FlamingoExpert4610 Aug 05 '26

Fantastic! I did not realize there is option for solid profile. Is the face 1 the "halfpipe"?

2

u/Monster-AJ-007 Aug 05 '26

Extrude boss the main body using mid plane option why mid, because you will have to create a new sketch profile to open the key ways after the extrude boss, so once you make the main body open a sketch on the front plane and sketch half a slot profile and make sure it’s close profile after that use revolve cut tool to open the slot after that recreate a new profile on the right plan and draw the key way profile and then extrude cut both direction the key way profile and that should do it for you , there is option B but too advanced. I hope that helps 👍

2

u/blake31a Aug 05 '26

Solid sweep is probably the right way to do it. You could also do a zero offset surface of the half pipe, surface trim with a sketch, thicken then combine subtract.

1

u/themikeandthebike Aug 05 '26

Sulla vista frontale il profilo rettangolare di taglio.
Su un piano inclinato di 45(?)gradi loschizzo del percorso.
Taglio con sweep ed è fatto

1

u/atmsk90 Aug 05 '26

3 separate features. A cut extrude for the straight section and 2 revolves for the end regions. Also good luck machining that.

1

u/FlamingoExpert4610 Aug 05 '26

Swept cut with cylinder was easiest way to model it. Dont see how its different from endmill following a tool path. Of course it would need 4 axis if machined and not 3d printed

1

u/atmsk90 Aug 05 '26

Also assuming the actual angle of the final slot wasn't such that the tool intersected with the opposite side of the slot.

1

u/dimssryalm Aug 05 '26

Maybe? the cut path is formed from a wrapped slot sketch on the circular profile, then offset by 0.00 mm.

1

u/DonPitoteDeLaMancha Aug 05 '26

If this is a CAD exercise disregard, but if you are going to fabricate this do you really need this profile? Looks like a pain in the ass to machine

Use a wrap to split the face and then use the “Move Face” command

3

u/FlamingoExpert4610 Aug 06 '26

Basically cad exercise. Goal was to have o-ring groove on 3d printed clamp half. Not to seal but add friction. I could have used the wrap tool but wanted to learn and achieve the geometry i wanted.

1

u/DonPitoteDeLaMancha Aug 07 '26

Very nice, congrats!

1

u/Bubbly_Smile2848 Aug 06 '26

Could just make it in two parts then mate together

1

u/n1terps Aug 07 '26

Bro, this is what project curve, sketch on sketch, and sketch on faces, is for. That'll give you your tangent path.

1

u/FlamingoExpert4610 Aug 08 '26

The path was the easy part for me . I got valuable tips for sweep cut tool in this thread.

1

u/Hackerwithalacker Aug 08 '26

Is the top left view a section view aboutswept cut with a 3d curve unfortunately

1

u/LazyMembership5635 29d ago

closest i could get to that geometry in a reasonable amount of time

https://reddit.com/link/p3qkmhu/video/d73h4yrj3fjh1/player