How do I put a finger grip pad on a sphere?

[CraigNorms]

Basically I need to put a finger pad or grip on the side a sphere. The ridges that extrude from the sphere are used to grip the part. If anyone can help please help me.

 

[CorBlimeyLimey]

There could be several ways depending on what shape of pad or grip you want/need.

If it's simple parallel ribs around the sphere, then a Revolve would probably be OK.

Other methods could involve creating and thickening surfaces.

If you can post a sketch of what you actually need, we may be able to be more helpful. (See faq559-1100)

 

[CraigNorms]

Thank you for your reply. The ribs/grip are on the outer edge of the sphere not inner. I have a rough drawing but I'm not sure how to post an image on this forum.

I'm not sure really how the revolve would work???

I have tried to post the image here

http://img57.imageshack.us/img57/1682/gripdesigncopytx4.jpg

Thanks again for your help.

 

[ctopher]

Use the Wrap command. Create the sketch internal of the part and use wrap to extrude it outward.

Chris
SolidWorks 06 5.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 10-27-06)

 

[MadMango]

Could you also project a curve on the surface and use a Split Line, then Dome the area?

[green]"Art without engineering is dreaming; Engineering without art is calculating."[/green]

Have you read faq731-376 to make the best use of Eng-Tips Forums?

 

[CorBlimeyLimey]

This was done in SW07

http://www.mooload.com/new/file.php?file=files/150107/1168880484/GripsOnSphere.SLDPRT

 

[CraigNorms]

Thanks for your help but the wrap tool only works on cylinders and not on spheres. Trouble is that I have 2006 version of Solidworks so the over solution I cannot try. Any other suggestions. I think that the wrap tool can only be used on surfaces that have one degree of curvature.

Any further suggestion would be great.

Thanks....

 

[Theophilus]

The way I do this (since it works for conical, compound/off-center, and any other shapes) is to extrude a surface through your sphere (or other) shape so they intersect. Use the Intersection Curve tool to create a curve at that intersection. Create a plane at the end of your curve, sketch your profile (round, in this case) on the end of the curve, and Sweep along that curve. This will give you the grips, similar to what CorBlimeyLimey posted.

Note that you can extrude non-planar surfaces into your spherical surfaces to get interesting curves in your grip shapes (the profile of your surface extrusion can be a spline or arc or combination, for instance--however, if you have multiple elements in your extrusion sketch, I recommend you use the Fit Spline feature to create a single sketch entity for a more stable Curve creation for Sweeping.)

At the ends of your grip detail, create a sketch on the flat faces (semi-circle-looking faces). Sketch a circle Coradial to your profile edge there, put a centerline through the circles center, trim to a semi-circle, and revolve the profile 180* to finish off each end.

This ends up consisting of lots of features by the time you're finished, but the results can be exactly what you want (very important in industrial design applications, where you use grip features of this sort all the time). You can also cut in the negative form using this same method.



Jeff Mowry

http://www.industrialdesignhaus.com

Reason trumps all. And awe transcends reason.

 

[ctopher]

Sorry, forgot you wrote it is a sphere.
Good suggestion from Jeff.

Chris
SolidWorks 06 5.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 10-27-06)

 

[CorBlimeyLimey]

http://img121.imageshack.us/img121/3759/gripsonspheresp8.jpg

SW06 version;

http://www.mooload.com/new/file.php?file=files/150107/1168882231/GripsOnSphereSW06.SLDPRT

 

[Theophilus]

CorBlimeyLimey's solution is certainly the simplest, if those are the shapes you need (and it looks like that's all you need based on your sketch). You can create the semi-spherical end caps as I suggested for these grips, too. My suggestion works for versions as far back as 2005, if I remember correctly--certainly for 2006--if you need more complex grip paths.



Jeff Mowry

http://www.industrialdesignhaus.com

Reason trumps all. And awe transcends reason.

 

[GBor]

I have another option, although I do think Jeff's solution gives the better results:

Create a sketch plane above your sphere. Sketch the shape of your ridges on the sketch plane. Extrude up to surface and select the surface of your spere. Copy your spherical surface and scale it slightly then trim your extrusion to the scaled spherical surface. Hide the sketch plane and the scaled sphere.

Garland E. Borowski, PE
Borowski Engineering & Analytical Services, Inc.
Lower Alabama SolidWorks Users Group

 

[CorBlimeyLimey]

Theo' ... the hemispherical ends could also be created by using the Fillet tool. Then all the "domes" could be in one feature.

 

[CraigNorms]

I think I have sort of done that, great thanks for your help. Really greatful its hard to find good help like this. I will give it a go and see how it turns out thanks again for your help.....

 

[Theophilus]

Yeah, that's true. However, sometimes I get small flat facets when I try that and often the Full Radius feature won't work--and if it does, it only lets me do one at a time anyway (very fragile feature when editing things upstream anyway).

One thing I like about the revolved ends is that the centerline doesn't necessarily have to be centered on the arc/circle center--so I can make a longer transition (increased revolve radius). I do this mostly with the negative forms.



Jeff Mowry

http://www.industrialdesignhaus.com

Reason trumps all. And awe transcends reason.