In simple words, can this be done?
Given that you can only create one closed split line profile per sketch and you don't SEEM to be able to pattern the split line when it's created as a feature. Is there any way this can be done? Any workarounds?
Thanks,
George.
Wow, yeah, that won't work. As for workarounds, you could try "pattern faces", which might work depending on what you are doing. If you do a 0 offset of the split faces and pattern the surface body it might help. It all depends on what you are trying to do with the new edges / faces. If you are looking to make draft, that's tough. You might consider cutting the part down to its smallest symmetrical form and patterning bodies. You might also try to use extruded surfaces instead of sketches, pattern the surfaces, make a big planar surface and do a mutual trim with the extruded surfaces (to get a single surface body), then do an intersection split line with the single surface body. Lots of different things might work, it's hard to give you good advice without knowing what you're trying to acheive.
matt
I use split lines for this purpose quite often George. Unfortunately you are correct, split lines can't be patterned. I have searched for a work around for a while and I haven't found one. I search for ways to incorporate as many face splits as possible using one closed sketch. It's like trying to piece a puzzle together. It can be very frustrating.
Ahoy Georgy!
Aye, 'tis a bit of a pisser indeed. One note that may or may not be of use to ye.... sometimes a cagy trick that's worked in the past be t' draw a zig zagy line that runs off the surface then loops back like a drunkin sailor with a shoddy map and compass. Thereby creatin' what amounts t' seperate surfices through lacin ye sails with wild loops....
Arrrrrr
YARR! I get ye me hearty! That might be crazy enough to work... could possibly get it all to work in one sketch.... still, it'll be a bit of a pain in the rear to do, but it'll get me away I think.... still.. would be nice if SWX could add pattern functionality to split lines.... it'd come in dead handy sometimes!
Aye,
Cheers to that Matey...
Arrrrr
perhaps you can extrude the sketch as a surface, and then array this surface. Create the split line with the intersection option with the arrayed surfaces
You can use a Wrap. It allows you to have multiple profiles in the sketch. Exit the sketch, then Insert/Feature/Wrap.
As I recall, Wrap only works on one face, but you can have multiple profiles. Split Line works on multiple faces, but you can only have one profile. Unless something has been added in SW06, there isn't an easy way to have multiple profiles on multiple faces.
Jerry Steiger Tripod Data Systems "take the garbage out, dear"
well- if you have a surface (made form multiple profiles) that intersects the target face/surface (made from multiple surfaces) then the intersection option in the Split line feature allows you to create split lines on the surface with multiple faces. Plus you can have multiple disjoint faces allowed as well.
This is pretty much all I use these days as it seems a more robust splitting tool.
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