Array an extruded object around a helical path?

[Archetype]

I’m using Inventor 2010 and am having trouble with a model I’m building. The model is of a brush on a vacuum cleaner. This consists of a 1” DIA. X 4” inch long cylinder and several (bristle type) brushes that are on the cylinder, evenly spaced in a helical pattern. There are approximately 12 brushes on the cylinder.

I have been trying to figure out a way to array an extruded cylinder (which represents my bristle brush) around a helical pattern on the main cylinder. Is this possible? I suppose if there was a way to create several points on a helical pattern on my cylinder that could work too.

Any suggestions would be appreciated.

Thanks,

[kencaz]

make your brush profile perp to your cylinder and sweep.

 

 

 

KC

[shift1313]

instead of sweeping a solid with the coil operation I would use a single line and make a surface. Then you can draw a single brush, use linear pattern and for Direction1 select the edge of your surface. Make sure you expand the options and change Compute to Adjust and Orientation to Direction1. I did this in an older version but in 2010 you will also have the option to make each brush a new part or merge them with the roller. This one i did a simple cone but your brush could be more detailed.

 

edit. my surface is above the roller only so you can see it. the surfce could be within the roller. If i were to model a part like this i would array a Hole, then add the brush in an assembly.

[Archetype]

shift1313,

This is exactly what I am trying to accomplish. When I get to my computer tonight I'm going to give it a shot. Stay tuned for the results.

Thanks,

[Archetype]

instead of sweeping a solid with the coil operation I would use a single line and make a surface. Then you can draw a single brush, use linear pattern and for Direction1 select the edge of your surface. Make sure you expand the options and change Compute to Adjust and Orientation to Direction1. I did this in an older version but in 2010 you will also have the option to make each brush a new part or merge them with the roller. This one i did a simple cone but your brush could be more detailed.

 

edit. my surface is above the roller only so you can see it. the surfce could be within the roller. If i were to model a part like this i would array a Hole, then add the brush in an assembly.

 

--------

 

Ok, I have the helical line withing my cylinder but i'm stuck on how to create a surface from the line so that i may finish the sketch as you did. I am not allowed to extrude the line at all, i thought that's how i would create the surface.

 

Little help?

 

Thanks,

[JD Mather]

-----I am not allowed to extrude the line at all, i thought that's how i would create the surface.

 

Little help?

 

Thanks,

 

Coil

 

You might want to go through this document http://home.pct.edu/~jmather/AU2007/MA105-1L%20Mather.pdf

 

Can you attach your file here?

[shift1313]

On the coil pop up you have the choice to make a solid or surface. If the line is the only thing you have, surface will be all you can do. If you have any closed sketches you will have to manually select Surface.

[Archetype]

Thanks All!

 

I am a rookie at Inventor but with your help i was able to achieve what i set out to do. Maybe not the most efficient way but I'll get better as I go. I decided to array the holes as suggested and put the brushes in the final assembly (great idea!) I'm sure I'll be back for more assistance in the future.

 

Results attached...

 

Thanks again!