How to offset a sketch in 3D

[mattbarb101]

Hi,

 

Thanks to whoever helps me out here. Im trying to offset a sketch I've done in 3D basically its a zig zag line that I need to offset so i end up with a circle with teeth (see image) I'm unable to offset in 3D do i have to draw the other line or is there a quicker way to do this.

 

Many thanks for helping me out.

 

Matt

[JD Mather]

I suspect there is an easier method to obtain the geometry - can you attach or link a picture of what you are trying to model?

[shift1313]

something like this? I drew a circle, extrude surface form that circle, then i drew the profile of one tooth in 2d. Used that to cut one tooth, thicken the surface, then did a circular array.

[mattbarb101]

Very nearly. The difference with what I'm trying to do it that the teeth aren't uniform I've attached a quick sketch of what I'm trying to do.

 

Thank you for helping me out here.

[JD Mather]

Very nearly. The difference with what I'm trying to do it that the teeth aren't uniform I've attached a quick sketch of what I'm trying to do.

 

Thank you for helping me out here.

 

I'm thinking create an Extruded surface.

Create a 2D sketch with baseline length PI*dia

Sketch the teeth and then wrap the cylinder.

Split the surface and then Thicken.

 

What version of SolidWorks are you using? Can you zip and attach your original file here?

[mattbarb101]

Ah, I think you're right! Sorry to sound thick but down do i get the circumference of a circle in Solidworks?

 

Thanks

 

Matt

[mattbarb101]

I manages to get this working well sort off however Im unable to close the curve as the points dont exactly meet up. I tried this with just a line this worked however there was a piece left over which i wasn't able to remove (intersecting curves).

 

I wonder if there's a way to do this with a curve of a surface?

Any help is greatly appreciated.

 

Thanks,

 

Matt

[mattbarb101]

Hi,

 

OK so I got this to work in the end so thanks for your help. What I'm actually trying to do though is to get it to wrap around (and cut) from a slanted vase like object but im unable to assume because the bottom line of the sketch is too long now.

 

 

Please help.

 

Many thanks

 

Matthew

[shift1313]

well there are several ways that i think this can be achieved. The first one that comes to mind is probably not the best but ive never had to approach a problem like this one. The Flex command seems like it would be appropriate here.

 

Lets say you know the circumference of the bottom edge of you vase and the angle. Start by drawing what is essentially your saw tooth pattern unwrapped. Extrude that a distance greater than your taper angle(this will make more sense in a second). Go to Insert>Features>Flex. The standard flex settings will have the clipping planes in the correct position for this so dont fool with them. Enter a bend angle of 360. This will give you the wrapped around saw tooth pattern you are lookin for. Now you need to get your angle. Depending on the end goal this can be done several ways. You can create revolved surfaces and trim the solid. You can revolve a solid(without merging) and combine them with the Intersect option under Insert>features>combine.

 

The next thing I did(because i didnt plan out the work planes) was create a work axis based off the cylinderical inner face, then an offset workplane based on my front plane and that axis. Now i can create a sketch and revolve around this axis for the rest of the operations. Its probably a good idea when planning this out to create a section view so you can better plan out your sketch.

 

You have to be careful with the overlap section from the flex and it may involve some extra work to plan this out.

 

Like i said there are other ways but this was the first that came to mind since you are dealing with a non-pattern.

[mattbarb101]

Thanks so much. Excuse the delay ive been sick but Ill try this method tomorrow.

 

Thanks once again!