Continue to Site

Eng-Tips is the largest engineering community on the Internet

Intelligent Work Forums for Engineering Professionals

  • Congratulations MintJulep on being selected by the Eng-Tips community for having the most helpful posts in the forums last week. Way to Go!

How to cut on multiple faces

Status
Not open for further replies.

Toolless

Mechanical
Apr 28, 2004
1
I have a 3-sided short, wide inverted U-shape solid part which is 3mm thick. I created this part by shelling three faces. I'd like to create a 2mm wide by 1mm deep continuous ridge along all three exterior surface, but when I created a 2mm x 1mm rectangle on one of the end edges and 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 the three exterior surfaces where I wanted to cut a 2mm recess, and still wasn't able to cut a continous 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. Cheers!
 
Replies continue below

Recommended for you

If I am understanding you right, it sounds like you need to try a sweep instead of extruded cut. Use the same sketch that you are trying to extrude and add another one on a perpendicular plane as a path that follow the shape of your "U".
 
Go to the SW Help Topics & in the Index section, type sweep for explanation & examples.

Also go to the SW Help Online Tutorial section & work through the Revolves & Sweeps tutorial.

[cheers] from (the City of) Barrie, Ontario.

[lol] Everyone has a photographic memory. Some just don't have film. [lol]
 
If your surfaces don't lend themselves to the sweep option you might be on the right track with the offset from surface feature. Try this:
1. Create a new surface with a zero offset by selecting the three surfaces. This should be similar to your knitting but I find it to be cleaner and faster for subsequent selections (because it is a separate feature in the tree and you can name it).
OR 2. Create a single surface offset by the intended depth of the cut by again selecting the three surfaces.

You might then create the sketch on a plane above the part and extrude it to a depth offset from the surface (#1) or just up to the offset surface (#2). Be aware that your sketch must be completely within the boundaries of the selected surface. You cannot have any of it overhanging.

If you are trying to do a sweep there are a couple of things to look for. One of them is zero geometry. I've seen this when a sketch is using a part of the surface and an edge of the part. Due to the changing shape of the part you are sweeping into this converted edge or the edge of the part can duck inside the part as it cuts and leave slivers hanging out. I think this has become less of a feature failure issue since disjointed bodies are now possible. However, it is poor modeling practice. Think of making this cut as if you were running a mill or lathe. Create the sketch lines that give you the cut boundary you want and removes the rest of the material. This is easy to do by making the sketch go outside the surface instead of being even with it - think if it as the body of the mill cutter extending from the final face all the way out to the collet. This has solved MANY sweep problems for my cohorts.

- - -Dennyd
 
Status
Not open for further replies.

Part and Inventory Search

Sponsor