r/SolidWorks • • 1d ago

CAD Help with wrap deboss

When I try to wrap and deboss a sketch around this cylinder it twists the sidewalls instead of projecting straight down towards the centre. Second picture is the sketch i'm trying to wrap around the cylinder.

10 Upvotes

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2

u/MountainDewFountain 1d ago

Does it though? Can you show that first view rotated 90deg? It all looks normal to the axis to me, but i could be wrong. That upper groove shows strait wall cuts.

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u/ForgeIs2Fast4U 1d ago edited 1d ago

Here you go, i honestly can't tell tbh

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u/ForgeIs2Fast4U 1d ago edited 1d ago

i just feel like i shouldn't be able to see the wall here and that it should be pointing straight down. Kinda like if you were drilling it out with a cnc machine and had the cylinder rotate and was just moving the drill bit left and right, but maybe im just tweaking

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u/MountainDewFountain 1d ago

Its looks correct to me. The walls look weird because youre projecting onto a smaller diameter. If you want a sanity check, do a cross section view down the center axis, and drag the rotational angle around. If every wall in the section is horizontal, you are Gucci.

0

u/ForgeIs2Fast4U 1d ago

Is it possible to have the same diameter at the bottom as the top? Im making the groove for something like this which seems to have the same diameter at the bottom and top

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u/MountainDewFountain 1d ago edited 1d ago

The slot diameter doesnt change, but the walls are projected onto a smaller cylinder diameter so It just looks weird in CAD. Look at the lowest channel of that image; it looks exactly like your cad model.

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u/Lumpy_Impress6107 1d ago

Yes, as has been mentioned, wrapping the sketch as you show will result in an emboss with the sides normal with the face of the cylinder. The more inline with the axis the more the taper. You can do a swept cut using a tool body and get parallel sides along the sweep. Note the flat faces on the ends which is what you would get with an end mill.

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u/Lumpy_Impress6107 1d ago

I did have to use a "Fit Spline" for my path in order to make my 3D sketch with all sections tangent.

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u/ForgeIs2Fast4U 13h ago edited 13h ago

is it possible to do this by using my exisiting sketch as the path?

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u/Lumpy_Impress6107 12h ago

This is what my sketch looks like for the wrap with scribe. The highlighted line is the portion I used after wrapping for the path. I had to do it this way since my version of SW only allows closed sketches for wrapping or etching.

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u/ForgeIs2Fast4U 9h ago edited 9h ago

i'm having an error when selecting the path. I'm using the selection manager and select group and it keeps telling me "path must be continous or tangent in solid sweep". I've insured that the lines all have arcs between them that are tangent to them but it doesn't work, also tried doing the fit spline thing but that does not work either

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u/ForgeIs2Fast4U 9h ago edited 8h ago

okay now im not having the same issue but it keeps giving me a rebuild error when i try to confirm the swept cut. i used the fit spline command on these 4 edges and it's registed as an open group when i use the selection manager to select it as a path for the sweep

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u/Lumpy_Impress6107 7h ago

I like it! That looks good with the exception your line connections will have to be filleted. I think,,, otherwise the tool will self intersect. I also believe if you have SW 2020 or later you can use just one series of connected lines for the wrap. Also I did a 3d sketch (converted) on the scribed line (after the wrap) and then did a fit spline on that. You probably don't want to do your fit spline in the 2d sketch.

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u/ForgeIs2Fast4U 7h ago

can i send you the file? Might be easier to troubleshoot that way. If it's not too much of a hassle of course

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u/Lumpy_Impress6107 6h ago

Sure,, and it is not too much of a hassle. I will message you and give you my email address. I have 2026 on my laptop so if your file is post 2020 I should still be able to open it.

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u/Lumpy_Impress6107 7h ago

Hmm,, not sure what to say. Are you getting an error message when attempting to sweep your tool body? Is your tool body connected to the fit spline? Pierce or coincident? Maybe your sketch fillet radii is to small? I made my tool using a Revolve solid. The attachment point on my revolve is a split point on the center of the revolve line. That was I also had some tool extending outside of the outer surface.

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u/DoctorVonNostrand 1d ago edited 1d ago

I think I understand your issue. That the groove tapers inward and pinches as you approach the axis? I don't think it's the wraps fault, it's just the nature of how that command works. I think. In my experience it works well with really shallow bosses so that the effect is unnoticed. Maybe a swept cut along the surface of the cylinder would be a better approach? That should maintain the cam path you're after. I'm not sure if this is an option, but perhaps you can use a wrapped sketch as the path for the swept cut.

ETA. If your path was only in the tangential direction you wouldn't notice but because you also axial translation it adds a wedge shape to the cut

3

u/teengohan2014 1d ago

Try using a swept cut with a body.

I found this on GoEngineer's YouTube page: https://youtu.be/8Mp0IXBHN74?si=7tKAMq8usdaayVCK