Help? I usually live in the solid world so surfacing tends to elude me at times. I'm trying to simply build upon a set of profiles created by ends of lofts. From there, fill the surface and knit to thicken.
I need your help in that I can't seem to figure out why the knit shows up with heavy lines at the tangents. They are tangent though. Then, when I try to thicken, the lines carry forward and thus, no smooth surface.
SW2010 please, I'm waiting until my clients migrate
thanks
Carter if you talking about these edges then those are correct in behavior. Creating tangent doesn't means that the edges will go off.
Thank you Deepak.
Yes, those lines are my problem. I am looking for all seams to be 'seamless' and smooth as in this screen image:
The final part needs to be smooth as the arrows are pointing out. I just can't see where my geometry is different between the two seams. I must be missing a fundamental rule somewhere.
Carter,
I cannot load SW2010 right now, so let me just explain. Your model has surface-lofts. This tool can only create true tangency (and curvature continuous) at the start/end constraints. You need both the start/end and the sides to be curvature continuous. This means you need to use the boundary-surface tool, which is both more robust, and allows for curvature continuity in all directions.
Model it mostly the same, but instead of loft, use boundary surface. First, model the four sides. Second, model each corner. For your edge constraints, set them all to tangent. You would get an excellent shape if you replaced your arcs with splines that are curvature continuous, but that depends on your design intent!
Inside your surface loft(edit feature) you need to add start/end constraints with the edge of the previous surface. I believe you can handle this in other ways as well either with a sweep, one loft, or a boundary surface. It appears you are using a pre 2011 version so i cant upload any files for you.
Looking at your sketches if you are going to loft this thing you should mirror your first loft and then use it as your end edge selection rather than the sketch you created. The reason i say this is because your corners will be different. If the mirror wont work(it also appears your Part isnt symmetric) then create your opposite corner loft first.
what is defining sketch 18? Your sketch 27 doesnt intersect the endpoint of the arc in sketch 18. The fact that the radius on the bottom is so much smaller will end up causing you some grief. Your sketch 22 and sketch 25 intersect both the upper and lower radii. You have to be very careful when defining your guide curves and rails or the results you get might not be acceptable.
You can see the edge at the bottom is not visible but the other edges are. What is more important here, the upper and lower profiles or the cross sections? If you can give us a little more info on the part/layout/constraints you have maybe we can help you lay out the sketches in a more useful fashion for this.
Matthew,
That did the trick. I knew it was something small but necesary.
Charles, Your suggestion actually has switched on a light bulb over my head. As another great SW contributor once taught about spit line usage (Mr Lombard), your idea makes great sense to me. I've experimented already and I'm going to rebuild the model using the boundry.
Thanks all! Great help and very much appreciated.
Carter,
I haven't used loft in three years. It has all-but been obsoleted by boundary-surface. If you ever have a need for centerline-loft, that is one thing it can do that boundary can't. I've only ever needed that once, and back then I didn't know what I was doing so I didn't use it.
Inside your surface loft(edit feature) you need to add start/end constraints with the edge of the previous surface. I believe you can handle this in other ways as well either with a sweep, one loft, or a boundary surface. It appears you are using a pre 2011 version so i cant upload any files for you.
Looking at your sketches if you are going to loft this thing you should mirror your first loft and then use it as your end edge selection rather than the sketch you created. The reason i say this is because your corners will be different. If the mirror wont work(it also appears your Part isnt symmetric) then create your opposite corner loft first.
what is defining sketch 18? Your sketch 27 doesnt intersect the endpoint of the arc in sketch 18. The fact that the radius on the bottom is so much smaller will end up causing you some grief. Your sketch 22 and sketch 25 intersect both the upper and lower radii. You have to be very careful when defining your guide curves and rails or the results you get might not be acceptable.
You can see the edge at the bottom is not visible but the other edges are. What is more important here, the upper and lower profiles or the cross sections? If you can give us a little more info on the part/layout/constraints you have maybe we can help you lay out the sketches in a more useful fashion for this.