Following a Boolean Subtract of a Swept feature (single closed profile along a helix), I'm left with what I am calling a 'sliver'... basically a thin undesirable area of geometry. As shown on attached jpg "sweep-leftovers-01", you can see the sketch profile I'm sweeping, and the resulting solid after having the sweep subtracted.
FYI the sliver is highlighted orange; the section cap is light blue; resultant solid body green.
It looks to me that there's a gap appearing in between the swept volume, causing the boolean subtract to leave the sliver.
To try to remedy this, I measured the gap between the 'coils' of the swept volume (shown in attachment "sweep-leftovers-02-measure"). I then adjusted the width of the swept sketch by the same amount, thinking that would eliminate the gap right?
Unfortunately the result is shown in attachment "sweep-leftovers-03-adjusted". It appears the boolean subtract is now resulting in an undesirably large solid volume (I guess because the profile is now overlapping?)
I have tried nudging the swept sketch width a little either way, but whatever happens, I either get a sliver or a big solid!
Currently I have worked around the issue by using surfacing techniques to delete and trim the sliver away, then rebuild using Filled Surface. However I'd be grateful of any suggestions to prevent the sliver happening in the first place, since I'm still at a stage of making design changes. And due to the form of the custom thread, every time I make a change, I have to re-do the surface editing. That's not a problem in itself but it just seems like there must be a better way of doing this!
I'm limited to what I can show in the images, as the design contains proprietry information. Hopefully the images give enough info to understand the core problem I'm having, but if you need more detail, I'll try to help.
Solved! Go to Solution.
Are you able to select the face?
Maybe "delete face" can help.
I will second Ruud suggestion...using DELETE FACE will be the best option once the sliver is created.
Without looking into the model it becomes very difficult to comment but yes i would sometime offset one of the swept faces (offset face) a little bit (one more feature before doing the boolean) to ensure there is no sliver face. Also try using the examine geometry check for checking these tiny sliver regions.
The width of your sketch will need to be exactly equal to the pitch of the threads. You might try tightening the modeling tolerance on the swept feature to see if that helps.
However, I would suggest a different modeling strategy. Instead of subtracting out a solid to leave the thread; subtract out a cylinder at the max diameter required then use swept to create the threadform and unite it. This has the advantage that the bumps of the thread don't need to meet exactly every pitch (in fact you don't want them to) and should make the modeling/updating a bit easier.
Thanks for your message.
Indeed, Delete Face achieved some of my goal, but I also had to use Trim Sheet to remove a final part of the sliver.
Thanks for your message and advice.
I didn't have any luck adjusting the tolerance or the sketch width, but I'm going to go with your alternative modeling solution and create the thread as a swept solid rather than using the current boolean subtract method.