SW 2005 surface modeling question

I am having trouble making a fillet along the edge of a solid created from a
surface. The surface is an imported iges from Surfcam. There is a ripple
which prevents the fillet from forming. How can I smooth out that ripple so
I can thicken the part and make a fillet? You can see the part on my
Solidworks page:

http://home.bellsouth.net/p/s/community.dll?ep=16&groupid=145864&ck=

Mark

 

Send it back to the SurfCam user & have them fix it.
WHY IN THE WORLD ARE THEY DOING DESIGN IN SURFCAM?

 

The surface comes from a point cloud. This is how it comes into Surfcam. Can
you suggest how to fix the ripple in Surfcam, as I am new to Surfcam and am
doing the tutorials this weekend.

Mark

 

Hi Mark,

You're probably going to have a tough time fixing that kind of stuff in
Surfcam. One thing you might try is to split the surface on either side of
the ripple. To do this you'll need to create surface splines with which to
break the existing surface. (it's been forever since I tried to edit
geometry in Surfcam) Once the offending is split out and deleted, you can
create a blend surface to replace it which will be tangent to the originals.
This would be under create>surface>blend.

Your adjacent geometry may no longer match up enough to be closed in SW
after, though... This is something that would be a lot easier in a surface
modeler like Rhino, or perhaps directly in SW. If you don't get any
satisfaction, I've e-mailed you with my address, you can send an iges or
Surfcam file to me and I'll see what I can do with it in Rhino.

 

Please remove 'nospam' from my email address to get the correct address.
Mark

 

You could trim it
You could Delete Face and use the Fill surface command
You could Delete Face and then Loft

You can also consider different kinds of fillets:

Face Fillet gets around a lot of irregularities
Face Fillet with Hold Lines allows you to manually specify the edges of
the fillet, but is more of a loft or fill, not a strictly "arc based"
fillet.
You could also just do the whole thing manually by trimming the surfaces
back on both sides of the edge and then lofting the blend from one side
to the other.

If you're gonna work in SolidWorks surfaces, you'll get good at all the
dances you have to do to make things work.

Matt

 

Nope.
But I crossposted it to AMC where someone else may
have clues <G>.
Without knowing the design intent .... looks like someone
goofed from here.
I'd still send it back to be fixed. The SurfCam guy may
have to send it back or request new data too. Anything
else is just guessing.

 

What is AMC?

 

Usenet newsgroup alt.machines.cnc.

 

Mark,


It looks symmetrical, and has one good side. Split it and mirror the result.


Regards

Mark

 

alt.machines.cnc

 

I got the part done by trimming off the bad edge and lofting back to a
smooth composite sketch of the edge. I used three sections in my loft. The
sections were created by pulling lines off the surfaces using the
intersection curve function. I thickened beyond the necessary thickness and
then filleted. I then used an offset and extended the surface to cut away
the not needed thickness. Thanks to Matt all who gave suggestions. No thanks
to those who said send it back to the other guy to fix. See results on my
web site as mentioned above.

Mark

 

But you have no idea at all if it's correct.