Worm Part - Cut-Sweep problem

[Bouke]

Hi There!

I've got a problem creating a worm-like part the way I want it. Basically I want to create something like this:

http://img139.imageshack.us/img139/8108/worm1sg4.jpg

The problem is; I do not want to simply cut-revolve a circle around a helix with a variable pitch like in this part. I want to cut extrude a cylinder instead of a flat 2D circle.

Like this:

http://img88.imageshack.us/img88/4323/worm3ke5.jpg

But I cant find an easy way to create this part. To make it a little bit more clear; next screenshot shows the same helix with a section view through the center. I marked the area's where there is material where there shouldn't be with arrows:

http://img132.imageshack.us/img132/5411/worm2vl7.jpg

Any got a good idea how to solve this?

Thanks in Advance!

Bouke

Bouke Brouwers
M-Des
The Netherlands.

 

[CorBlimeyLimey]

SW2008 has included the ability to sweep-cut a solid.

 

[dgowans]

CBL,

I was thinking the same thing, but didn't want to mention it in case Big Brother (Scott) is watching.......

In all seriousness, a swept solid is the only way to accurately do this. Please be aware that a swept solid is brand new functionality and will more than likely behave as such.

 

[Bouke]

Hm, thanks for the quick response.

Although I'm afraid this is not really helping me, I'll be happy if I got SW08 in April/May and this part should have been made already. Our machines software did not seem to have the functionality we expected it to have so now I need a good model of the worm.

I can simulate the shape of the cutout by doing numerous normal cut extrudes from planes that I keep rotating 1° and then use the section view edge. But this will not work with the variable pitch. Bah, I'm quite at a loss here. Silly machines never do what you want em to do.

Bouke Brouwers
M-Des
The Netherlands.

 

[CorBlimeyLimey]

There is a way to simulate an approximation of a swept solid, but it would be a fairly slow process if I remember correctly. It involves creating a spiral pattern of the cutting tool surface, then creating actual cutting surfaces from the patterned ones. I will try to find a link for it and repost.

Meanwhile, can you adjust the normal swept cut profile and angle (to the helix) to produce what you need?

 

[CorBlimeyLimey]

Found it. I'm not sure where it cam from, but it was probably someone from this forum. Hopefully they will step in and explain further.

 

[handleman]

Well, if you can post a part file that includes everything up to the swept cut (i.e. the tool body, the main part cylinder body, the proper helix, etc) then perhaps someone with '08 could make the swept cut, save as a parasolid, and post it back to you. I would volunteer to do it myself, but I leave for vacation in an hour. If you can get the stuff posted within half an hour from now I may be able to do it for you myself. Here are the requirements for a swept body cut from the SW'08 help file:

Solid sweep (cut sweeps only). Creates a cut-sweep using a tool body and path. The most common usage is in creating cuts around cylindrical bodies. This option would also be useful for end mill simulation.




Tool body and path
Cut sweep





Profile . Sets the sketch profile (section) used to create the sweep. Select the profile sketch in the graphics area or FeatureManager design tree. The profile must be closed for a base or boss sweep feature. The profile may be open or closed for a surface sweep feature.

Tool body (cut sweeps only). The tool body must:

Be a revolved feature

Contain only analytical geometry, such as lines and arcs

Not be merged with the model.

Path . Sets the path along which the profile sweeps. Select the path sketch in the graphics area or FeatureManager design tree. The path can be open or closed, and can be a set of sketched curves contained in one sketch, a curve, or a set of model edges. The start point of the path must lie on the plane of the profile.

Neither the section, the path, nor the resulting solid can be self-intersecting.

For cut sweeps only, when you select Solid sweep, the path must be tangent within itself (no sharp corners) and begin at a point on or within the tool body profile.

 

[ShaggyPE]

Not sure if the technique I will propose below is the same as the model that CBL provided (I am using 06).

Could you do a curve driven pattern of your cylinder around the helix (not merging bodies). If you have a ton of instances of the cylinder it will approximate a smooth sweep. You could then merge the bodies of the cylinders, but not the worm. After that, "combine bodies" with the "subtract" option selected.

Don't know if the above is clear, or if it will work, but it may be worth a shot.

-Shaggy

 

[CorBlimeyLimey]

Here's an image of the part I uploaded.

 

[Luca83]

Try this...

Sweep Surface:

http://img.photobucket.com/albums/v161/LC1983/SW1.jpg

Copy and trim cylinder face:

http://img.photobucket.com/albums/v161/LC1983/SW2.jpg

Cut thicken:

http://img.photobucket.com/albums/v161/LC1983/SW3.jpg

SW2008 Premium SP0 - Rhino 4.0

 

[Bouke]

Aah, there are some idea's. I just arrived home from work and I'm afraid I only got a 2006 license myself so I cant open the part. But I'll check it out first thing tomorrow morning.

I'll upload the part with the helix and the cutting tool according the above description also, would be a great help if someone with 2008 could make a step or parasolid file from it.

I quite like the curved driven pattern idea, I quite overlooked that option. I reckon I could make a (quite computer heavy) body with all the patterned instances of the tool and then try to make 1 smooth body from it and substract. I'll mess around a bit with 2006 and if succesfull I'll get back to you.

Thanks again

Bouke Brouwers
M-Des
The Netherlands.