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...?
Attachmentsgrooves-SW.SLDPRT, 724 KB
Wow, tnanks Steen, this is beautiful! I was just working on making my cuts consistent, and thinking of how to avoid all the repetitive steps, and voila! So much useful info, my head is swimming. As a programmer in the past, I always look for the most efficient methods, and it looks like I got quite a ways to go.
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.
Attachmentsgrooves-4-SW.SLDPRT, 500 KB
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.
Attachmentsgrooves-final.SLDPRT, 771 KB
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)
plz try to make a new model & more practice
Learning is get the key then do more practice
i try to give the key!
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.
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.
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)
Correct, Mike. 'Thrown somewhere in outer space' is a precise description. In a larger model it can be really hard to find the sketch :-)
That is how 'derived sketches' look initially before they are constrained. You need to select the centre of the circle and the path you want it attached to, and select a 'Pierce' relation in the pop-up menu. Then the circle will pop into place.
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.
I think I figured it out! Right-click on 3D sketch in tree -> show!
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.
Attachmentsgrooves-3-SW.SLDPRT, 351 KB
LOL, thanks Steen, yes, I tend to jump ahead of myself, I'll try to watch that now. Still, scratching my head at the geometry issue.
Hmm, I added a tutorial but it seems to be MIA?
Strange! I figured it out though - for whatever reason, my 3D sketch was hidden, either I did it at some point, or it does so by default, but all I had to do is right click and "Show" it to be able to select individual parts.
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....?
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!