Surfacing Trouble

[AeroJDK]

I am tackling a large surfacing job that requires surfaces defined by various 3-D splines. I have two questions: can a loft be created by 4 3-D splines that define an enclosed space but continue beyond that corners of that space (imagine a tic-tac-toe board with the center square being lofted and all of the line are 3-D splines)?

If not, is there a way to select the POINTS that make up the boundaries and inner surface area of that square and export them, only to then import them back using the Import Geometries tool?

Is there a better way in general of doing this?

Thanks to all for the help.

Jonathan K.

 

[Theophilus]

You can use a "fill surface" feature to do something very similar to what you're attempting (2005). The curves in the area of your surface will dictate the filled surface shape. I've come to love using this feature for just this sort of application. The only snag is that you have to have surface or solid edges as your boundary for making the fill--not mere curves or sketch entities. But you can get that simply by extruding a square as a surface and trimming to fit for your boundaries as necessary (and a lot of other ways).

Hope that helps. Check the help menu for details.


Jeff Mowry

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.

 

[AeroJDK]

Thanks for that tip. I believe I see what you mean, it's just that I will be having to do this multiple times, so the more streamlined I can make the process, the better.

When I try to do this in SolidWorks 2003 using the "Filled Surface" tool, I get error message eluding to "open boundaries", making me think that it has a problem with the tic-tac-toe like overlay lines i.e. there isn't a perfect square outlining the middle square but rather open and overlapping lines. But SolidWorks 2005 accepts that?

Any input on the point-to-surface idea?

Jonathan K.

 

[Theophilus]

Do your bounding edges form a plane, if not four bounding edges? If so, you should be able to fill the surface using each edge without problems in SW 2003 (I think).

If your bounding edges are non-planar, this could cause some problems. At each bounding edge, you can specify (in 2005) whether the edge joins the adjacent surface in a tangent or merely touching relation.

So, supposing you have 15 edges that make up your bounding edges for the surface you want to fill. You must not have overlapping edges formed by overlapping surfaces.

So, you can have a hole in a single surface that you want to patch, with lots of edge segments and it should work. The more edge segments, the more complicated you may be requiring the filled surface to be (since the single filled surface must touch all the edges for a proper fill).

You can also have a deleted surface. Let's imagine you extrude a solid cube. Then you delete one of the faces. You have four bounding edges with which to fill/create a surface, and the remaining surfaces are no longer solid (turned into a surface body by deleting one of the surfaces).

You can also project a split line (any shape, including a circle) onto a surface of any kind and then delete the split surface. In the case of a circle, you'll have only one bounding edge and it still works.

Either way, you can use curves or points to influence the filled surface. Less is more, to a degree. Don't go nuts with complicated descriptions for your surface--it's like putting in too many profiles in creating a loft--you make a not-so-smooth surface when it's all done. Keep it to a minimum while accomplishing what you need.

The "open boundaries" thing means you didn't select all of the edges. Since SW has very poor display quality in the edge selection while using this feature, CTRL-select each bounding edge first, and then select the fill-surface feature. (For some reason, SW displays the whole surface of the edge you select in green, making it too difficult to see what you've selected and what remains to be selected--poor choice.)


Jeff Mowry

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.

 

[AeroJDK]

Jeff --

Thanks a ton for your help on this. I tried the selection of the bounding curves BEFORE I clicked on "Trimming Surface", yet the tool is greyed out once I select those curves. I should add that those curves are being used as guide curves in the loft of original surface. Below is a link to the file that I am dealing with...maybe if you get a chance you could take a look at it.

Again, the sketches should make it look like a tic-tac-toe board from a top view, and I'm looking at keeping the surface that is bound by the inner square.

http://www.vadama.com/Surface

Trimming Problem.SLDPRT

Thanks again...

Jon

 

[SBaugh]

Bad link - this one works

http://www.vadama.com/Surface Trimming Problem.SLDPRT

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
faq559-716 - SW Fora Users

 

[TheTick]

can a loft be created by 4 3-D splines that define an enclosed space but continue beyond that corners of that space

Why not just make a new set of sketches that copy the curves and trim them appropriately?

I could be the world's greatest underachiever, if I could just learn to apply myself.

http://www.EsoxRepublic.com

-SolidWorks API VB programming help

 

[AeroJDK]

Thanks much for the correction...I'll be curious to see what you guys think.

Jonathan K.

 

[Theophilus]

I don't quite follow the surface trimming idea. I was talking about the "delete face" feature, wherein you can define one surface from another with a split line, then delete the face that remains.

In the example you posted, I can delete the face in the middle of your lofted surface, but then have no end caps to constrain a surface fill (remembering I need edges of surfaces as bounding entities for such a fill). So the loft would need to be larger than the surface you need to fill, so the deleted face would be deleted from within the rest of the surface instead of taking out the full width of the surface and having no bounding edges to rebuild a filled surface with.

I think I'm missing the nature of your design intent on this one, too. Care to ellaborate on what you need to do with the loft surface from this point?


Jeff Mowry

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.

 

[AeroJDK]

Sure...sorry for the lack of thorough explination on my end. I'm really trying to isolate and have ONLY the center square remaining with a loft. Eventually I want to have a thickness there, which is actually going to be representing the skin on an aircraft, but the way I currently have the lines and the skin thicknesses in different areas, I'm going to have to end up lofting larger areas, such as the example, and trimming away around it to leave only the center square so I can define a specific thickness for it. I will then be laying up locks around that center square that may change in thickness.

Am I going about this the completely wrong way?

Thanks again for the input and help...

Jonathan K.

 

[Theophilus]

Well, this depends on what you're ultimately making. If your lofted surface is OK for now, don't try using your guide curves in the loft to isolate the surface--that's not what they're for.

You should be able to create your lofted surface, and then thicken to your nominal thickness. You can then offset your outer (or inner) surface to the thinner surface depth you mentioned, and then simply perform a cut with a surface (might need to build some walls around your cutting surface for better direction indication in the surface cut).

But if I read what you're doing correctly, you should be able to make the bulk of your thickened surface in the primary thickness, and then merely trim away some of the solid using a surface offset from your initial surface (with a surface cut or other method). That offset surface can be trimmed using other surfaces as trim tools or by using other methods.

Anyway, I'm not quite sure I understand the ultimate intent, but I'm fairly confident you can do it with surfacing tools within SW since there is such a large variety of accomplishing the same thing within SW.


Jeff Mowry

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.

 

[AeroJDK]

Maybe this will help. I'm trying to fill the square the is bound by the selected (green) lines.

http://www.freeimagehosting.net/uploads/080b5e05df.jpg

"Fill Surface" nor "Surface Loft" will allow this to happen. From what I understand that you are saying, this should be possible though...I'm definitely confused.

Thanks...

Jonathan K.

 

[Theophilus]

I haven't been able to use sketches as boundaries, but I just found out in a similar thread that it can be done.

If I understand what I read there, you can open a new 3D sketch and convert the entities of the four sketches you need into your 3D sketch. Trim the extra stuff so you have a curvy square. Exit the sketch and use the 3D sketch as your bounding entities.

The problem I see with this is that you have no tangency control of your surface out around the edges since you have no surface around which to refer. But maybe you don't need that.


Jeff Mowry

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.

 

[rfus]

jeff,

you don't. you'll get the message 'Tangent constraints cannot be applied to boundaries containing sketches' if you try and control this in the surface fill command. Try making yourself some wierd surface with the flex command. Then use sketch tool -> face curves on that surface, then make some 3d sketches with these face curves and use surface fill. Then do it again with all kinds of constraint curves. you still get tangency every time.

I wish SW would make a copy surface feature rather than having to enter 0 in offset surface.

 

[PlasticFantastic]

The guide curves are allowed to be overbuilt-not the loft sections. I would probably use one set of curves as guide curves and then trim converted entities to create loft sections. alternatively you can work in top down-create a large loft and then create offsets at different distances of the larger surface. Thicken the surface and then split the solid body. Then use the offsets as trim sheets to create the different tile thicknesses.

You will invariably get better surface quality with a top down approach as Theophilus describes