Advanced Surfacing

[CLinn]

Hi folks!

I've been given the joyous task of trying to create a solid model from an Excel file of points (1943 points). This is the first time I, or anyone in the company, have ever had to deal with a surfacing task.

I have managed to import the point cloud and surface it. I have also created the surface of the flat base. I now have a varying band between the two surfaces to fill so that I can create a solid. I have tried everything, but no luck.

Reading the help files, it sounds to me like "Knit" should do what I need, but it will not work. I have tried "loft", "sweep", "extrude"...I have tried every button on the Surface toolbar.

Any help would be greatly appreciated.

Thanks!

Casey

 

[TheTick]

A picture would be helpful. Could you post one?

If I understand you correctly, you have two faces that need "sidewalls between them. You could make the sidewalls using Surface --> Extrude.

Make the surfaces long enough to extend past the two original surfaces. Trim surfaces to size using Surface --> Trim. You can trim an knit simultaneously using the "mutual trim" option. Otherwise, for Knit to work, the trimmed surface edges have to match up nearly perfectly.

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

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-SolidWorks API VB programming help

 

[CLinn]

One edge is geometric. The other is ...well...just nasty.

I'm new to Eng-Tips too. How do I post a picture?

 

[CLinn]

I got a picture.

The problem is between the geometric green and the nasty red.

 

[alolesen]

Rather than making another "surface" for your base, just use the base sketch to extrude a boss and choose "Up to Surface" for the termination condition. Choose the surface generated by your point cloud. You can then Hide the surface and be left with the extruded solid body.

 

[antran7]

Have you tried the fill surface feature? The trick might be trying to select the red/white border in one selection (try the smart-select feature when you right click on part of that border). If you can make the fill surface, you when then knit it with the red and white, and voila...

If you don't mind losing some of that red data, you could extrude a surface from the bottom plane (the base of the 'mountain', and make sure you intersect both the red and green surfaces. you would then trim the three surfaces so they meet at clean edges, and then knit them together. I think this was Tick's idea, so I'm just plagarizing him.

 

[Theophilus]

The suggestions above would work--depends on what you need as your final outcome. Looks like your surfaces are "open", so you'll either need to extrude up to one of your surfaces, knit the red and green surfaces and extrude up to the new knit surface, or close the red and green surfaces by adding a Surface Fill and choosing "try to form solid" as the option.


Jeff Mowry

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.

 

[CLinn]

antran7:
The fill command will not work either. As for losing some data, that can't happen. This was measured data that we have to reproduce and test equipment to. The project requires that the data be made into a solid model, have over 2000 precision hole machines through it then put in a mockup for testing. We need to get the holes and profile CNC'd, that's why I'm having to make the model.

alolesen & Theophilus:
There is a large gap between the surfaces. I'm off for the Canadian Thanksgiving weekend, so I will try to do the suggested extrude on Tuesday morning.

Thanks for the help everyone. Any other ideas are surely welcome if this doesn't work.

 

[PlasticFantastic]

options:
1)Do a Radiated Surface from the edges, parallel to the platen. Then Knit the surfaces together and extrude to surface. Somewhat as if you were creating tooling for one side of the surface

2) Surface Extrude. I am not sure if the white surface is data. If it is not, then 3D Sketch>Convert Entities on the lower edge of the red surface, pick the green plane (or top plane) as a direction vector and extrude the curve down. Mutually trim the platen and side wall, and add a cleaner wall on the outside of the "dirty" wall

If the whit wall is data, then knit white and red. Convert entities on the red surface edge and either extrude along the direction vector of the white wall edge or sweep it along the edge.

3)Ruled Surfaces might be an option as well.

 

[PlasticFantastic]

BTW how in the world was that red surface accurately modelled and how did you find the deviation from the point cloud??

 

[PlasticFantastic]

BTW- radiated surface should be from the Red surface, and the extruded surface should rise from the green surface

 

[CLinn]

Thanks everyone for all the help. I managed to get the surfaces to join and make a solid. To fill the gap between the red and green surfaces, I had been trying to do it in one step. I ended up having to make 4 separate lofts between the two to get them to join and knit.

Thanks again for all the help. Now I'm off to add the 2000+ holes...oh joy!!

 

[overkill04]

Hey Clinn,

Wondering what macro you used to import this massive excel point cloud. Is the cloud still linked to the excel file??

And finally could you post a link to the macro.

Thanks a million.

And happy halloween everyone!

Overkill

 

[CLinn]

Overkill04:

I used "mm_24.zip" from

http://swtools.cad.de/macros.htm

The cloud points are not linked to the Excel file.

 

[overkill04]

Sorry Clinn one more thing.

What was the best way you found to apply a surface to these points?

Thanks again.

 

[rfus]

I can't believe that you were able to surface a large point cloud in Solidworks without a crazy amount of work. In most reverse engineering packages you have to go from points to polys to nurbs patches, and the algorithms to create a curve network from a point cloud is nothing that SW has in the basic package, as far as I know, and not to mention the devition from this cloud.

Yes, please tell us how this was done, I am eager to know.

 

[CLinn]

Overkill04:

My data happened to be in straight rows. I put a "Curve Through Reference Points" for ewach row of data (I had 44 rows, so 44 curves). I then made a Loft surface using the curves in order.

Hope that helps.

 

[CLinn]

rfus:

Don't get me wrong. This was A LOT of work.

My data happened to be in straight rows. So that made it easier. We weren't worried about deviation. Our purpose only requires a rough approximation of shape, not an exact replica.

 

[rfus]

Ah yes, the points in straight rows and with no noisey points makes this not too hard. It didn't appear from your image that there was an order. The process and deviation is not bad when you have gridlike order. I did one with 4096 points as a test a while ago on a 64x64 grid. You can see there is little deviation in the pic.

Red, a polygon surface with verticies seen in black.
Exported verticies and imported into solidworks.
Used selection filter to grab each row and create the curves.Lofted curves with surface loft.
Imported polygons in as stl graphic (don't try to do as surface or solid with large polygon files, you'll sit for a while and it won't do over 100K polys) And you can see the surface is a good representation of the polygons. Reverse Engineering with Solidworks is possible, you just need fairly ordered data.