How to cut on multiple faces

I have a 3-sided short, wide inverted U-shape solid part which is 3mm
thick. The short flanges are about 20mm, and the slight arc is about
320mm wide. I created this part by shelling three faces. I'd like to
create a 2mm wide by 1mm deep continuous ridge along all the three
exterior surface (similar as if I would machine/mill or lathe a solid
part), but when I created a 2mm x 1mm rectangle sketch on one of the
end edge adn performed a cut command I can only select one target in
the extrude dialog box. So I'm ending up w/ a 2mm wide recess on only
one face. I'd like to continue this feature along the adjacent arc
surface and opposite mirror surface (inverted U-shape). I also tried
to KNIT (as well as few other suggestions) the three exterior surfaces
where I wanted to cut a 2mm recess, and still wasn't able to cut a
continuous 2mm wide recess along the flat-arc-flat exterior surfaces.
I'm a novice in this program and trying to teach myself, so please be
descriptive w/ your advice. However, I have a few years experience w/
AutoCAD and Vellum. Any excellent references will also be useful.
Cheers!
Reply to
Randy
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Randy,
Sorry, I don't quite get the question.. so.. could you post the file or send the file to me... with an example of the problem or image of something similar?
..
Randy wrote:
Reply to
Paul Salvador
In sheetmetal if you are not getting the desired cut you can do a few things first try it without Normal Cut on. If that doesn't work then try using the split tool instead this works differently but may give the desired result. there are always cut revolve and cut sweep if those suit your needs.
Corey
Reply to
Corey Scheich
Paul,
Thanx for replying. I'll send you the file w/ an image of what I'm trying to do later today.
Reply to
Randy
Like Paul, I'm a bit confused by your post, since you talk about cutting, but also about a ridge. I'm also confused about which side of the U, inside or outside, you're working on. If you're trying to cut a constant depth slot into the three inside faces of your part, you can probably use a cut to an offset from a surface, using the surface knit from your three faces. You may run into problems at the edges, though, because the cut can't extend past the offset surface. You might be able to get around that by offsetting your three faces, then extending/trimming that to offset 0 faces at the two end faces.
Jerry Steiger Tripod Data Systems "take the garbage out, dear"
Reply to
Jerry Steiger
Randy,
Ok, got your files (sorry for the delay) but I have SW2004 so I can not show you the final files.
Image ref:
formatting link
There are 2 simple ways to do this cut and the sketches used can be used in either approach:
-Sweep Cut (profile and path) -Cut w/thickness (edge copy w/thickness)
Sweep Cut - (Insert/Cut/Sweep) (you need a profile and path) You already have a 1X2 groove profile sketch shown, now you need sweep path sketch,.. so, for the sweep path, using the same front plane as your extrude thin sketch... so, at the end of you "U" shape profile (w/the radii), copy the whole outside edge using (right mouse button) "select tangency" and "convert entity" (this copies the tangent edge)... Now you have a profile and path. The SW command is, Insert/Cut/Sweep Select your 1x2 groove profile and select your sweep path.
Cut w/thickness - (Insert/Cut/Extrude) Offset a plane from the front face of your "U" profile to the distance or start of your groove. (you can do this with the above as well) The above sweep "path" can be used for this sketch cut. The only difference is the plane it resides on. So now you have a copy of the "U" profile on the offset plane. Now, you do a "Insert/Cut/Extrude" with "Thin Feature" (width).. the values used will be that which define the groove width (thin feature) and depth (direction 1).
..
Randy wrote:
Reply to
Paul Salvador
Randy, You could also create a 3-d sketch of the intended path, with a cut profile at a managable place, then do a sweep cut (using the two sketches) following the profile.. might work.. worth a try..
wentz
Reply to
wentz
Paul,
Excellent solution and explanations. After spending sometime figuring out your suggestion(s), I finally got it to work. Thank you so much for taking the time and in your interest!
Randy
Reply to
Randy
So, the next time Paul gets flamed by someone for having a bad attitude, remember who it was who went so far out of his way to help you!
Jerry Steiger Tripod Data Systems "take the garbage out, dear"
Reply to
Jerry Steiger

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