A simple sketch on a plane extruded to a radius surface and also touching a drafted surface. 'Up to next' is the ideal selection when picking extrusion termination but it is not available. An identical sketch (as far as I can tell and I've looked really good) has the 'up to next' available. What are the rules used in determining what termination is available? I've been training a newbie and he has ran across this. He is presently using a VAR installed eval copy and is considering a purchase but inconsistencies like this are hindering a purchase decision. I feel that there is something that I'm not seeing but for the life of me I can't find it. Can anyone offer a suggestion?
Can you clarify your terminology so we can home in on the problem:
When you say "Surface", do you really mean surface? In SolidWorks, a surface is a zero-thickness entity, such as would live in the "Surface Bodies" folder.
Perhaps by "surface" you meant "face", ie the face of a solid body. "Up to next" requires a solid face, and it must be a contiguous face on a single body, with no undercuts. What is perhaps confusing the issue (and many users do not realise this): the options on display will be restricted according to the direction SolidWorks picks to try and extrude your sketch. Because of this, "Up to Next" will NOT be listed until you reverse the direction of extrusion (by clicking on the "Reverse direction" icon). The reason this limitation is not widely recognised is that, in ordinary modelling, SolidWorks' default direction usually doesn't expose the limitation.
If you really did mean "Surface", you will have to use "up to Body"; "up to next" is not available. The region in question must be a single surface with no undercuts, and it must overlap the projection of the extrusion -- at least, it is sometimes problematic if the edge of the projected sketch coincides anywhere with an edge of the surface.
This different behaviour is a function of whether the surfaces are analytical or algorithmic. The former are simple geometric primitives, the latter, essentially spline based, freeform shapes, cannot be extrapolated by the software beyond the user-defined boundaries. Hence an "extrude up to surface" will happily infer where to terminate in the first category, even though the analytic surface in question is not big enough or is out of position. Features extruded up to a freeform surface must however fall within the boundaries of the terminating surface, or they will fail.
To be more specific... I said 'surface" because that is one of the terminations available. No there are no 'surfaces' on the part. Imagine a rectangular base sketch (with the corners filleted .5 inches) extruded to a depth of 4 inches with .5 degree of outward draft. This is then shelled to a thickness of .175 . A plane id created .75 inches from the inside base (parallel to original sketch plane). On this plane are sketched the simple keyway shape in the top corner and the bottom corner. Theses are two different sketches BTW. The sketches are dimensioned identically from their corresponding corners. Looking planer to the sketches you will see that when extruded they will contact first the side of the shell cavity that is drafted .5 degrees. As the extrusion gets closer to the termination 'surface' or 'face' the extrusion comes in contact with the fillet on the inside of the solid. On the top sketch the 'up to next' is available while on the lower sketch it is not. Up to surface works but there is a difference between the two visually and the 'up to next' is preferred.
I hope this is more descriptive and will lead to a more specific answer to this question. I will attempt to duplicate the issue if I am able to get away from the 'real' work today. Thanks for looking into this for me
Jeff
----- Original Message ----- From: "Andrew Troup" Newsgroups: comp.cad.solidworks Sent: Thursday, February 19, 2004 9:10 PM Subject: Re: What determines available terminations?
"Maybe Not Me" wrote in news:jWcZb.223192$U%5.1358072@attbi_s03:
Direction of the extrusion is a common reason for "up to next" not showing up when you think it should. If you just switch the direction, does it show up?
It also might not show up if any of the sketch hangs off the part and would extrude into empty space, or if there is a hole in the part where you're trying to extrude.
Thanks for the info but neither of your suggestions are the case. I've found that I can use the modify sketch command to move the problem sketch just far enough so that it overlaps another face, update, and then when I edit the feature "up to next" is available. From this point I edit the sketch again and place it back where it was, update and "up to next" is still available. Maybe a bug? Anyway, I now have a work-around.
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