How to cut grooves through a concave surface?
Hi all, I started learning Solidworks about a month ago, so please don't judge too harshly :) I know the basic tools and techniques by now, and am really looking forward to learning the more involved methods. I am faced with a challenge of cutting (etching?) grooves into a surface with concave geometry (revolved cut) inserted, and the grooves are supposed to follow the hole so to speak. How could I do this? I know swept cut won't work, so I thought maybe I could offset the curves or the surface (came across this method in my searches), but so far, no luck. I am attaching a screenshot and my part. There will be other patterns (circles, etc) eventually, but this should give you the idea. Thank you in advance, I am glad to have found this community and look forward to becoming an active member!
Welcome to the community.
I have tried my hands on your little assignment and come up with the following (which is quite similar to what Saeid suggests).
A few pointers:
- I use the 'intersection curves'-tool between surfaces to give one 3D sketch that contains all centerlines for swept geometry
- The individual sweep paths are selected in this 3D sketch using 'Selection Manager' (right-click and choose SelectionManager to open )
- I use one basic circle-sketch that is re-used in all sweeps by selecting the circle-sketch, selecting a new plane and choosing Insert->Derived Sketch. This way you only need to change ONE original sketch in order to make changes for all sweeps.
- I don't use swept cuts due to the difficulty of seeing where this fails (when it fails)
- Instead, I use swept solid bodies that I eventually subtract from the main body using boolean operation.
- I use DeleteFace-command to repair the final geometry. This step could be avoided if the original paths were drawn so that they extended beyond the perimeters of the 'box'.
Hope this gives you some useful tips...?
Can't thank you enough for your great help. I gained enough new knowledge to last this entire weekend :) Attached is my final result, which includes triangular cuts and the once again changed pocket (was requested of me). Things I learned to keep in mind is the size of the sweep tool - if it's too big for some of the corners/curves, you won't be able to complete the sweep due to "invalid geometry", 3D sketch becomes "hidden" after the first sweep, so you have to "show", and if you can't "combine" (subtract) it's most likely because your bodies were checked to merge at creation.
Thanks Saeid! I think it's very close - I was able to recreate what you did with a projected curve and swept cut, however, it only works if I suppress your original cut, and as soon as I unsuppress it, I am presented with the error as in 2nd screenshot. If I try editing my now erroneous cut, it gets even weirder (3rd screenshot). Am I missing something? Is it because these curves/cuts intersect? (the screenshots are in backward order)
This turned out to be a great exercise, as I was asked to make the "hole" bigger, and make the cuts angular instead of rounded. I managed everything quite nicely so far, but I seem to be having trouble with "derived sketch". I even checked "set the origin on curve" in all my planes, however, it's still thrown somewhere in outer space instead of snapping to what is supposed to be the origin? (screenshot attached: "sketch 4" is the original sketch on Plane 1, and Plane 2 is where the derived sketch should go, circled on the left)
Nevermind my previous comment, reading about derived sketches clarified it (still couldn't make them fully defined, so gave up on that for now, and just created separate ones).
--- EDIT: got the following sorted out, see comment below ---
I seem to have hit a wall though - no matter what I do, I can't select individual paths in my 3D sketch after the first sweep. Found Selection Manager, tried different selection tools in it, clicking on the 3D sketch from the tree does nothing.
--- END EDIT ---
While I can now select individual parts of my 3D sketch, I am now getting all sorts of "geometry" errors with this... screenshot and model attached.