Automatically slice a 3D model for lasercutting... 1

[nio101]

Hello,

I'm learning to use SW, and I'm looking for a decent way to reproduce in SW what this plugin is offering to the Sketchup community, that is slicing a model into contours for lasercutting:

http://blog.ponoko.com/2010/11/11/slice-your-3d-model-for-lasercutting/

I've played with the split feature, but it doesn't seem to be the good tool.

The idea is to be able to slice a 3D model into contours of a given width (3mm for example) specifying the cutting planes.

If someone can help... thanks!

nicolas.

 

[AnnaWood]

Why not just cut a bunch of section in a SolidWorks drawing?

Anna Wood
Core i7 EE965, Nvidia Quadro 5000, 12 Gb RAM, OCZ Vertex 120 Gb SSD, Dell 3008WFP 30" Monitor
SW2011 SP0, Windows 7 x64

http://www.solidmuse.com

http://www.phxswug.com

 

[AnnaWood]

Or see what you can import into Sketchup and if SolidWorks will export a file type Sketchup can read. Then use the Ponoko tool.

Another option hire someone to write a custom program for SolidWorks to do that for you.

Anna Wood
Core i7 EE965, Nvidia Quadro 5000, 12 Gb RAM, OCZ Vertex 120 Gb SSD, Dell 3008WFP 30" Monitor
SW2011 SP0, Windows 7 x64

http://www.solidmuse.com

http://www.phxswug.com

 

[nio101]

The idea is not only to get the contours of the slices, but to use them in a model too. That means get the section contours, extrude them and assemble them.

For a great number of slices, that could be quite long and repetitive... So I was looking for a way to do that, but I guess there is no easy way for that in SW.

I can't hire someone to do that, and I can't find any resources to learn how to develop a plugin for SW, so I guess I'll look for the manual way.

Thanks.

Nicolas.

 

[Scheffers]

I'd say, use split-lines, then create several sketches (through "convert-entities") onto different planes...

see my attachment..

 

[CorBlimeyLimey]

1) Create a set of planes using the Offset Distance and Number of planes to create options.

2)) Sequentially create a sketch on each plane using the Intersection Curve tool.

3) Right click the part in the graphics area and select Body > Delete.

4) Extrude each sketch to create the slices, deselecting the Merge option to create a multi-body part.

 

[MDGroup]

Another easy way to create multiple cross-section bodies is to simply do a cut extrude. Just make it a very, very, very thin cut.

Create a rectangle on the side of the part, with the rectangle only being about 0.000005in wide. Extrude this thru the entire part and it will split it into 2 bodies with an extremely small gap between them. You can pattern the skecth (or feature) to create as many slices as you want.

Any of the methods mentioned above should work; it just all depends on what you are really trying achieve from this; and the reaulst that you are actually after.

 

[nio101]

Thanks for all your suggestions, that really helped!

I finally use the procedure CorBlimeyLimey described as it is the quickest and easiest way to get what I want...

Have a nice day!

Nicolas.