Need some advanced surfacing tricks

Can you try importing the file to Rhino3D and doing the work there? It really does surfacing much better than Solidworks.

'Sporky'

Joel Moore wrote:

Sporkman wrote in news: snipped-for-privacy@bigfootYETI.com:

I had an eval of Rhino installed for a while but once we got SW 2004 I stopped using it. I pretty much only used Rhino for untrimming surfaces and now SW does that.

In general, Rhino frustrated the hell out of me so I never got too deep into it. Maybe I'll put some more effort into it once I have the time.

seems to me that you would not need to use surfaces but then again I hardly ever use surfaces but you might just draw a box where the vertical edges are pierced to the tangent points of the fillet -- then use one tangent edge as a sweep path & the other tangent edge as a guide curve. You will probably have to create separate sketches for your path & guide curve by creating two

good luck

Steve Tietz

oop I just had another look at the image -- a box probably will not work since the vertical edge would not match the curvature of that front face... sorry

so you might try using offset surfaces with values of 0 then untrim all surfaces & extend up to surfaces to get the edge to meet then Knit all surfaces together

then try making those surfaces closed by offsetting & trimming with the fillet & solidifying those surface & Join the solids or just create the corner as surfaces & extrude a solid shape upto that surface.

maybe that will help?

Hard to know without having the actual model Steve Tietz

Joel,

So, deleting the blends and extending the faces and trimming does not work? Anyhow, try and delete the green highlighted blends and extend the boundaries and trim. Or, if it is faster, instead of deleting the blends, copy offset "0" the faces you need and and extend them and trim/blend. There are other ways you can also approach it if the surfaces are not behaving but it means rebuilding those faces, such as, fill surface or lofting.

Good luck.

..

Joel Moore wrote:

First make sure you do a Tools, Check on the geometry, with validation turned on. Next, I would run an import diagnosis, and ask it to improve the geometry. You can also use import diagnosis to remove faces, but I would do that with the feature based tools, because diagnosis leaves no history of what you did or way to undo it other than reimport.

Are you having problems deleting the faces or closing the gaps? Have you tried to delete all the faces of the fillet and let SW close the gaps on the solid (without leaving it a surface model) automatically?

If you have to do this manually, the section where the smaller fillet runs into the flat face (blue arrow) will need to be trimmed square before it will knit solid. That combined with the fact that the edge that feathers into the smaller fillet (red arrow) is likely to create some very nasty small edges will give you some challenges. You may need to construct a new surface in this area instead of trying to extend the green arrow face. The new surface will need to be an extension of the face indicated by the black arrow, or it may be easier to delete the black arrow face and just recreate it altogether, and trim it with the flat face with the hole on it.

The larger fillet looks fairly easy from this distance.

If you get really desparate, email the part. It may take some swearing, but I think this can be done.

matt

If the model is solid or there are no gaps on the fillet edges, remove the fillet faces using "Delete Faces". This will allow the adjacent surfaces to grow back together. Then apply a matching fillet in SW (be sure to save a backup copy to measure).

You will need to experiment to see how many faces you can delete at once. Usually deleting an entire continuous face set works well.

if you knit the faces and have a good import you can also insert a thicken feature to make it a solid and then do the same thing The Tick suggested

Corey

Thanks everyone for the replies. Most of what you're saying agrees with how I figured I'd have to approach it.

Part of the problem is that the original import wasn't able to form a solid due to several translation problems (the customer is using IDEAS).

So I essentially just peeled apart the model using the surface offset (0 offset) feature and exported the various sections into new models that represented the various pieces of the mold. So the result is that none of these fillets are solid.

I guess the thing that started driving me nuts is realizing that a surface can't be extended up to or trimmed to itself. So replacing those missing fillets requires a lot of face duplication at the least.

But at least I see now that this is pretty much the way to do it.

Thanks for the advice.

Joel Moore

Not even with surface>untrim? I have had great luck with that, but I think it has to be a BREP model (untrim modifies the boundary exposing the full, untrimmed surface)

Joel, something you said here made me realize there's a trick that may help you. In importing your file from IDEAS select Options (from the bottom right of the "Open" dialog box) and select the radio button that says "Do not knit". Doing so will import your surfaces separately so that they CAN be knit later. If you don't select this option you get a single COMPOSITE already-knit surface that cannot be knit to itself (when you try to use the Knit command).

Mark 'Sporky' Staplet>