Automatic part length in assembly

[Rufio]

Is it possible to set-up a part with solidworks like a shaft if I want its length to adjust automatically by mating both end on 2 surfaces in the assembly. If it is, how can I do this?

 

[TheTick]

A couple ways to do this:

1.) define the a shaft using a revolved sketch, in the context of the assembly

2.) define the shaft as an extruded section, and define the extrusion feature in the context of the assemble. Use "Up to Surface" or [/i]"Up to Vertex"[/i] end conditions for your extrusion. You can use assembly vertexes and surfaces, or define datum planes in context to use as the end-limiting geometry.

3.) define your shaft by a sweep. Define your guide curve end points in-context in the assembly.

Good and evil: wrap them up and disguise it as people.

 

[SBaugh]

But the point is here, you need to incontext the part at the assembly stage.

I have a box on my website that is incontexted. It's called "VBA controlled box"

http://www.scottjbaugh.com/Design_Portfolio/SW Models DT.htm

Download it and you can see how the parts are incontexted in an assembly and then edit the DT and change the Height, Width, & Length. Then you will see how it all works together.

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
When in doubt, always check the help

 

[JNR]

I have asked for this enhancement several times and seen nothing happening. There is a real lneed for this type of "variational geometry". Example: springs. you model them at free length, but they are always compressed in that darned assemblies. It is not practical to keep on making new configurations for every compressed spring length, specially if, like us you release and control your library part files. There are a number of type of parts this applies to. What we need is a way to have a basic configuration of a part and be able (maybe in a second configuration?) to define certain dimensions as being back driven by an assembly mate if it exists. I keep thinking that now we have the ability to back annotate design tables and use external spreadsheets as the design tables, there might be a way to make it work with some linking, but I have not had time to mess with it. We are doing similar things and have just found a wayto get the whole shahbang to up date with one click but it uses some Access database stuff along the way.

3/4 of all the Spam produced goes to Hawaii - shame that's not true of SPAM also.......

 

[APPENG]

A way to avoid the incontext is to have a reference dim on the planes in the assembly, and use an assembly level equation to make the extrude length of the tube equal to the reference dimension value.. (assuming of course that oyu are extruding the feature) if you are sweeping, or lofting you may be better off with the incontext feature.

just a thought

Regards,
Jon
jgbena@yahoo.com