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How to cut grooves through a concave surface?

By Mike B on 13 May 02:43 14 answers 1839 views 5 comments

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!

Added images

Square

Attachments

grooves.SLDPRT, 144 KB
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14 answers

  • Steen Winther
    Steen Winther over 2 years ago

    Hello Mike,
    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...?
    Cheers,
    Steen

    Attachments

    grooves-SW.SLDPRT, 724 KB
    Download
  • Steen Winther
    Steen Winther over 2 years ago

    Yes, this technique is not great with a triangular profile. You can get the job done by creating planes at every sharp point, doing the sweep in three separate operations. But the transitions look bad because the swept profiles won't line-up.

    Attachments

    grooves-4-SW.SLDPRT, 500 KB
    Download
  • Mike B
    Mike B over 2 years ago

    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.

    Attachments

    grooves-final.SLDPRT, 771 KB
    Download
  • Mike B
    Mike B over 2 years ago

    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)

  • saeid mirshahidi
    saeid mirshahidi over 2 years ago

    plz try to make a new model & more practice
    Learning is get the key then do more practice
    i try to give the key!

  • Mike B
    Mike B over 2 years ago

    You sure did Saeid! Using your key, I was able to take it further. There are still artifacts, but now I know how to take care of it. Much appreciated.

  • Steen Winther
    Steen Winther over 2 years ago

    Glad to be able to help. There sure are many ways to do a job in SolidWorks and they all have their strengths and weaknesses. This job, I think, will always require many repetitive steps, but at least they are very simple and quick to perform.

  • Mike B
    Mike B over 2 years ago

    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)

  • Mike B
    Mike B over 2 years ago

    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.

    Attachments

    grooves-4.SLDPRT, 428 KB
    Download
    grooves-3.SLDPRT, 277 KB
    Download
  • Steen Winther
    Steen Winther over 2 years ago

    Sorry, I didn't see that you solved the issue with derived sketches.
    I have made a few screen dumps showing exactly how the Selection Manager works.
    Cheers,
    Steen

    Attachments

    grooves-3-SW.SLDPRT, 351 KB
    Download
  • Steen Winther
    Steen Winther over 2 years ago

    Hmm, I added a tutorial but it seems to be MIA?

  • Steen Winther
    Steen Winther over 2 years ago

    Bloody hell - GrabCAD your system is broken!

    I just lost the tutorial for the second time. It saves and uploads but where has the tutorial gone....?

  • Mike B
    Mike B about 2 years ago

    Strangely, I've got some notifications about people posting tutorials here, and none appear, something must be seriously wrong with the system. Hope it's been fixed by now. Thank you all, I really appreciate all your help!

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