[Michael El]

I am not that advanced in doing lofts, but I managed to cut out the bottom portion with a loft, and now I wanted to loft out the top. The bottom loft cut goes from bottom to top, and the top loft cut goes from left to right.

http://i53.photobucket.com/albums/g6...shin/loft1.jpg
This is a picture of the 3d sketch and 2 guide lines

http://i53.photobucket.com/albums/g6...shin/loft2.jpg
This is the preview of the loft cut, which results in a zero thickness error.


any ideas? The loft sketches aren't referenced to the top sketch of the bottom loft, I deleted them manually after constructing them.

[JerryFlyGuy]

Michael, your zero thickness issue is coming from the inside edge of the cut. I always try to never cut right along the surface. Instead, if you were to simply cut from one profile to the next, you should not get a error, if you do it's because one edge of the profile is directly on the surface. Instead, if you were to add to those profiles and extend them through the surface, into the center cavity just a little bit you'll lose the error in short order. Also your guide curves shouldn't have to follow the surface on the inside, instead they should be able to go directly across from one profile to the other. On the outside, you'll want them to follow your profile, but on the inside it will be just cutting through air, so it won't matter..

Hope that's all clear..

J

[Michael El]

Ok I have extended my profile in both directions so that
a) it extends past the inner wall into the cylinder bore
b) it extends downwards past the surface (maybe thats bad?)

I also changed the inner guide curve to go straight across

Here's a picture:

http://i53.photobucket.com/albums/g6...shin/loft3.jpg

but alas, the same error message. I'm still tinkering to find a way around. I think maybe when I cut downwards it might error although I've removed the relationships to that plane sketch..

There's nothing on the outside that is interfering at all and there is plenty of material to cut through

[JerryFlyGuy]

Michael, that is really strange.. I don't suppose you could post the file? Can you get it to repeat if you do the same thing in a new file [just to try and duplicate the issue]?

I've done 1 or 2 lofts in my day.. I might be able to figure it out but not w/out the file unfortunatly..

[Michael El]

Thanks for helping out Jerry,

http://myfreefilehosting.com/f/36cef2411b_5.86MB

solidworks 2007 SPO

it's the last in the list.

[JerryFlyGuy]

Michael, I didn't get time to reach a completely conclusive answer last night, but it does seem that there is still some geometry issues. I think the zero thickness is coming due to the loft cut earlier in the tree. Also you'll not be able to use that 3d sketch for profiles as you need two profiles for a lofted cut. Lastly, there seem's to be some issue w/ the 3d sketch. I extracted the two end profiles into their own 3d sketch's and tried to do even a lofted body w/ them. For some reason it still won't loft so I'm thinking there is some form of corrupted geometry there.. not sure at this point and I ran out of time to mess w/ it last night.. I'll give it some more thought tonight..

J

[Michael El]

thanks a lot, i'm new to lofting, and going tonight to pick up some reference books, it seems like a very picky piece of code, and its not entirely intuitive. hopefully tomorrow i will get some new info that will help with these errors

[JerryFlyGuy]

Michael, well the only book I can recommend is Mr Lombardes SolidWorks Bible.
The thing about lofting is.. it's something you pretty much have to learn by doing, or watching others do it. It's a pretty tough thing to learn by reading a book. [I've tried ]

Anyway, I think I've found out the issue w/ your model.

The two end profiles are not planer. Now, I've never tried to do loft w/a 3d [non-planer] end profile before so this was new to me. I finally used the near vertical straight line [inside the cylinder] and the point where the guid curve meets the outter edge and created a plane there. Then I converted the edges of the 3d sketch on the the plane and using the existing guid curve [on the outside] as well as 1 new on drawn as the 3d sketch between the two bottom corners of the profiles, was able to get the lofted cut to work. I've included a couple pic's to show some of the nasty edges that come to be an issue w/ this geomerty. I'm using 2008 so you'll not be able to open it w/ 2007 and see how I did it [unless you've upgraded?] I can email it back to you or post an iges or.. whatever you'd prefer if it'd help.

I'm thinking that maybe instead of doing this cut [it's an induction port on the side of the cylinder?] in two or more cuts that you should try to do this in one complete cut from top to bottom. It will require more geometry to get it all in one cut and it may require some simple extruded cuts afterwards to clean stuff up.. but it might give you better geometry to work w/.

Another option would be to use a bunch of lofted surfaces and then knit them together to form a solid, and use the solid to subtract the volume from the main body [or use the surfaces to do a surface cut in the solid.

W/ geometry as complex as this is, while maintaining exacting control of surface contours, using surfaces over solids will get you alot farther, alot faster than trying to work w/ solids.

Hope that helps!
J

[Michael El]

thanks a lot jerry, it was the last piece that was giving me trouble

just had to convert it to a planar sketch instead of using a 3d one..i wonder why

[JerryFlyGuy]

Not a problem. I rather enjoyed the challenge. Unfortunatly, I don't always get to spend the time on these challenges, when I want to so it can take longer than normal to get through them.

The reason you can't use a 3D sketch for that lofted cut [or lofted solid for that matter] is because it's a solid form.

A lofted cut is nothing more than a lofted solid w/ a 'combine' feature, using the lofted part as the 'volume to subtract' from the main body. If you look at that same loft as a surfaced loft you can see why it won't work. The end profiles of a lofted solid, must be planer. The end of a loft either in the cut or lofted body, are always flat [at the profiles]. This is why surfaces would do what you want to do, alot better.

I've been messing around w/ some lofts here the last couple days and banged out this model. I'm using some of the edges of existing geometry to be the new profile for the next loft. NONE of them are planer [it's all splines driving the shape] and they work rather well. The other nice thing is that the surfaces can be open, you don't need a closed profile to do a surface loft.

Anyway, play w/ it.. it's really the only way to learn it.. unfortunatly.

I've learned a few tricks from watching others do lofting and surfacing stuff, but mainly you just gotta get your hands 'dirty' so to speak..

Best..

J